Download ASAS (Non-Linear)

ASAS (Non-Linear)
User Manual
Version 12
ANSYS, Inc.
Southpointe
275 Technology Drive
Canonsburg, PA 15317
[email protected]
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494
© Copyright 2009. Century Dynamics Limited. All Rights Reserved.
Century Dynamics is a subsidiary of ANSYS, Inc.
Unauthorised use, distribution or duplication is prohibited.
ANSYS, Inc. is certified to ISO 9001:2008
Revision Information
The information in this guide applies to all ANSYS, Inc. products released on or after this date, until superseded
by a newer version of this guide. This guide replaces individual product installation guides from previous
releases.
Copyright and Trademark Information
© 2009 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited.
ANSYS, ANSYS Workbench, AUTODYN, CFX, FLUENT and any and all ANSYS, Inc. brand, product,
service and feature names, logos and slogans are registered trademarks or trademarks of ANSYS, Inc. or its
subsidiaries located in the United States or other countries. ICEM CFD is a trademark used by ANSYS, Inc.
under license. All other brand, product, service and feature names or trademarks are the property of their
respective owners.
Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE
SECRETS AND ARE CONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS
SUBSIDIARIES, OR LICENSORS. The software products and documentation are furnished by ANSYS, Inc.,
its subsidiaries, or affiliates under a software license agreement that contains provisions concerning nondisclosure, copying, length and nature of use, compliance with exporting laws, warranties, disclaimers,
limitations of liability, and remedies, and other provisions. The software products and documentation may be
used, disclosed, transferred, or copied only in accordance with the terms and conditions of that software license
agreement.
ANSYS, Inc. is certified to ISO 9001:2008
U.S. Government Rights
For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement, the
use, duplication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS,
Inc. software license agreement and FAR 12.212 (for non-DOD licenses).
Third-Party Software
The products described in this document contain the following licensed software that requires reproduction of
the following notices.
Formula One is a trademark of Visual Components, Inc.
The product contains Formula One from Visual Components, Inc. Copyright 1994-1995. All rights reserved.
See the legal information in the product help files for the complete Legal Notice for ANSYS proprietary
software and third-party software. If you are unable to access the Legal Notice, please contact ANSYS, Inc.
Published in the U.S.A.
ASAS (Non-Linear) User Manual
Update Sheet for Version 12
April 2009
Modifications:
The following modifications have been incorporated:
Section
Page(s)
Update/Addition
Explanation
All
All
Update
Conversion to Microsoft® Word format
Table 5.1
5-4
Update
Changes for neutral RAO input
5.1.1
5-6
Update
Allow 32 character hydrodynamic file name
5.1.6
5-11
Addition
Add Note 4 on frequency analysis
5.1.11
5-16
Update
Add HYDR command
Allow 32 character hydrodynamic file name
5.1.18
5-24
Update
AP20 option replaced by APIW
App I.1
I-1
Update
Delete references to legacy programs ASDIS, PICASO
App I.2
I-2
Update
Delete references to legacy programs ASDIS, PICASO
App I.3
I-2
Update
Delete Section I.3 (ASDIS Interface)
App I.6
I-15
Update
Delete Section I.6 (PICASO Interface )
App M.3.2
M-3
Update
AP20 option replaced by APIW
Table M.1
M-7 – M-8
Update
AP20 option replaced by APIW
App M.6.5
M-11
Update
AP20 option replaced by APIW
App M.6.17
M-34
Update
AP20 option replaced by APIW
App M.6.387
M-53
Update
AP20 option replaced by APIW
App M.6.45
M-58, M-59
Addition
Add definition of phase offset data
App M.7
M-65 – M-66
Update
AP20 option replaced by APIW
ASAS (Non-Linear) User Manual
Contents
Table of Contents
1. Introduction ............................................................................................................................. 1-1
1.1 General Capabilities ....................................................................................................... 1-1
1.2 Using this Manual .......................................................................................................... 1-1
2. Types of Analysis Available.................................................................................................... 2-1
2.1 General ........................................................................................................................... 2-1
2.1.1 Static Linear Elastic Solution .................................................................................. 2-1
2.1.2 Static Non-Linear Incremental Solution ................................................................. 2-2
2.1.3 Transient Non-Linear Incremental Solution ........................................................... 2-2
2.1.4 Eigenvalue Extraction ............................................................................................. 2-3
2.1.5 Steady State Heat Solution ...................................................................................... 2-4
2.1.6 General Field Analysis ............................................................................................ 2-4
2.1.7 Piezo-resistivity Analysis ........................................................................................ 2-4
3. Program Features ..................................................................................................................... 3-1
3.1 Types of Element ........................................................................................................... 3-1
3.1.1 Uniaxial Element..................................................................................................... 3-1
3.1.2 Plane Stress/Strain Elements ................................................................................... 3-1
3.1.3 Axi-symmetric Solid Elements ............................................................................... 3-2
3.1.4 Three-Dimensional Solids....................................................................................... 3-2
3.1.5 Gap/Interface Elements ........................................................................................... 3-3
3.1.6 Plates, Shells and Beams ......................................................................................... 3-3
3.1.7 Spring/Dashpot Elements ........................................................................................ 3-5
3.1.8 Linespring Elements................................................................................................ 3-5
3.1.9 Uniaxial Field Elements .......................................................................................... 3-5
3.1.10 Two Dimensional Plane Field Elements ............................................................... 3-6
3.1.11 Three Dimensional Solid Field Elements ............................................................. 3-6
3.1.12 Axisymmetric Solid Field Elements ..................................................................... 3-6
3.2 Material Model Types .................................................................................................... 3-6
3.2.1 Elasticity.................................................................................................................. 3-7
3.2.2 Plasticity .................................................................................................................. 3-7
3.2.2.1 Yield Criteria ................................................................................................... 3-8
3.2.2.2 Hardening Rules .............................................................................................. 3-9
3.2.3 Creep ....................................................................................................................... 3-9
3.2.4 Failure ................................................................................................................... 3-10
3.2.5 Field....................................................................................................................... 3-10
3.2.6 Piezo-Resistivity ................................................................................................... 3-10
3.2.7 Heat Convection .................................................................................................... 3-10
3.2.8 Heat Radiation ....................................................................................................... 3-10
3.3 Loading ........................................................................................................................ 3-10
3.3.1 Nodal Loads .......................................................................................................... 3-11
3.3.2 Prescribed Displacements ..................................................................................... 3-11
3.3.3 Pressure Loads ...................................................................................................... 3-11
3.3.4 Distributed Loads .................................................................................................. 3-11
3.3.5 Temperature Loads................................................................................................ 3-11
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
i
ASAS (Non-Linear) User Manual
Contents
3.3.6 Face Temperature .................................................................................................. 3-12
3.3.7 Body Forces .......................................................................................................... 3-12
3.3.8 Centrifugal Loads .................................................................................................. 3-12
3.3.9 Angular Accelerations ........................................................................................... 3-13
3.3.10 Nodal Fluxes ....................................................................................................... 3-13
3.3.11 Prescribed Field Variables .................................................................................. 3-13
3.3.12 Flux Densities...................................................................................................... 3-13
3.3.13 Wave Load .......................................................................................................... 3-13
3.3.14 Tank Loads .......................................................................................................... 3-13
3.3.15 Load History........................................................................................................ 3-14
3.4 Node Numbers and Coordinates .................................................................................. 3-14
3.5 Element Numbering ..................................................................................................... 3-15
3.6 Global and Local Axis Systems ................................................................................... 3-15
3.6.1 Coordinate Local Axes .......................................................................................... 3-16
3.6.2 Element Local Axes .............................................................................................. 3-16
3.6.3 Skew Systems........................................................................................................ 3-16
3.7 Structural Suppressions and Constraints ...................................................................... 3-17
3.8 Solution Procedures ..................................................................................................... 3-17
3.8.1 Non-Linear Static Solution Procedures ................................................................. 3-17
3.8.2 Non-Linear Transient Solution Procedures ........................................................... 3-19
3.8.3 Contact Analysis Solution Procedures .................................................................. 3-19
3.8.4 Fracture Mechanics Solution Procedures .............................................................. 3-19
3.9 Program Organisation .................................................................................................. 3-19
3.10
Post-Processing ....................................................................................................... 3-20
3.11
Data Units ................................................................................................................ 3-20
4. Data Preparation ...................................................................................................................... 4-1
4.1 General ........................................................................................................................... 4-1
4.1.1 Data ......................................................................................................................... 4-1
4.1.2 Data Formats ........................................................................................................... 4-3
4.1.2.1 General Principles ........................................................................................... 4-3
4.1.3 Special Symbols ...................................................................................................... 4-6
4.2 Data Generation Facilities .............................................................................................. 4-8
4.2.1 Repeat Facilities ...................................................................................................... 4-8
4.2.2 Re-Repeat Facilities ................................................................................................ 4-9
4.2.3 List Generation in the Preliminary Data Section .................................................. 4-11
4.2.3.1 A Simple List................................................................................................. 4-11
4.2.3.2 Generating a List with a Topological Variable ............................................. 4-11
4.3 Description of Each Data Block................................................................................... 4-13
4.3.1 The Preliminary Data ............................................................................................ 4-13
4.3.1.1 General .......................................................................................................... 4-13
4.3.1.2 System Control .............................................................................................. 4-13
4.3.1.3 Solution Algorithm ........................................................................................ 4-14
4.3.1.4 Model Behaviour ........................................................................................... 4-15
4.3.1.5 Output Control ............................................................................................... 4-16
4.3.2 Structural Description Data - see Section 5.2 ....................................................... 4-16
4.3.3 Boundary Condition Data - see Section 5.3 .......................................................... 4-18
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
ii
ASAS (Non-Linear) User Manual
Contents
4.3.4 Loading Data - see Section 5.4 ............................................................................. 4-19
4.3.4.1 Proportional Loading ..................................................................................... 4-19
4.3.4.2 Load Functions .............................................................................................. 4-20
4.3.4.3 Pseudo Times ................................................................................................ 4-20
4.3.5 Additional Mass Data - see Section 5.5 ................................................................ 4-21
4.3.6 Initial Conditions Data - see Section 5.6 ............................................................... 4-21
4.4 Description of Output................................................................................................... 4-21
4.4.1 Data Input Echo and Checking ............................................................................. 4-21
4.4.2 Analysis Results .................................................................................................... 4-22
4.4.3 Analysis Summary ................................................................................................ 4-24
4.4.4 Journal Files .......................................................................................................... 4-24
4.4.5 ASASNL Output Markers ..................................................................................... 4-24
5. Data Formats ........................................................................................................................... 5-1
5.1 The Preliminary Data ..................................................................................................... 5-2
5.1.1 AQWA Command ................................................................................................... 5-5
5.1.2 BLOCK Command.................................................................................................. 5-5
5.1.3 COMMENT Command ........................................................................................... 5-6
5.1.4 CONVERGENCE Command ................................................................................. 5-7
5.1.5 EGEN Command .................................................................................................... 5-8
5.1.6 EIGN Command...................................................................................................... 5-8
5.1.7 ELGROUP Command - (Group Section Only) ...................................................... 5-9
5.1.8 END Command ..................................................................................................... 5-10
5.1.9 FILE Command ..................................................................................................... 5-10
5.1.10 GROUP Command - (Group Section Only) ....................................................... 5-11
5.1.11 HYDR Command ................................................................................................ 5-12
5.1.12 INTEGRATION Rule Command ....................................................................... 5-14
5.1.13 ITERATION Command ...................................................................................... 5-15
5.1.14 JOB Command .................................................................................................... 5-16
5.1.15 LOCYCLE Load Cycle Command ..................................................................... 5-17
5.1.16 MONITOR Command ........................................................................................ 5-17
5.1.17 NEWSTRUCTURE Command ........................................................................... 5-20
5.1.18 OPTION Command ............................................................................................ 5-21
5.1.19 OUTPUT Command ........................................................................................... 5-23
5.1.20 PARAMETER Command ................................................................................... 5-25
5.1.21 PASS Command.................................................................................................. 5-27
5.1.22 PINO Pressure Interpolation Order Command ................................................... 5-27
5.1.23 PROBLEM and TITLE Command ..................................................................... 5-28
5.1.24 PROJECT Command .......................................................................................... 5-29
5.1.25 RESTART Command ......................................................................................... 5-30
5.1.26 RESU (or POST) Commands.............................................................................. 5-31
5.1.27 SAVE Command ................................................................................................. 5-33
5.1.28 SCALING Command .......................................................................................... 5-34
5.1.29 SKIP Command - (Group Section Only) ............................................................ 5-34
5.1.30 SLEEP Command ............................................................................................... 5-35
5.1.31 SOLUTION Command ....................................................................................... 5-36
5.1.32 SOLVE Command .............................................................................................. 5-39
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
iii
ASAS (Non-Linear) User Manual
Contents
5.1.33 SPIT Command ................................................................................................... 5-40
5.1.34 SRESTART Special Solution Restart Command ............................................... 5-42
5.1.35 START Command .............................................................................................. 5-43
5.1.36 STRUCTURE Command .................................................................................... 5-43
5.1.37 SYSPAR Command ............................................................................................ 5-44
5.1.38 SYSTEM Command ........................................................................................... 5-45
5.1.39 TEMPORAL Command...................................................................................... 5-46
5.1.40 TEXT Command ................................................................................................. 5-47
5.1.41 TITLE Command ................................................................................................ 5-48
5.1.42 UNITS Command ............................................................................................... 5-48
5.1.42.1 Global UNITS Definition ............................................................................ 5-48
5.1.43 UPDATE Command ........................................................................................... 5-50
5.1.44 WAKE Command ............................................................................................... 5-51
5.1.45 WEIGHTS Command ......................................................................................... 5-52
5.2 Structural Description Data .......................................................................................... 5-53
5.2.1 UNITS Command ................................................................................................. 5-53
5.2.2 COORDINATE Data ............................................................................................ 5-56
5.2.2.1 Local Coordinate System Header .................................................................. 5-57
5.2.2.2 Local Coordinate System Orientation ........................................................... 5-57
5.2.2.3 Node Coordinates .......................................................................................... 5-60
5.2.2.4 Coordinate Imperfection Data ....................................................................... 5-62
5.2.3 Element Topology Data ........................................................................................ 5-65
5.2.4 Material Property Data .......................................................................................... 5-67
5.2.4.1 Elastic Material Properties ............................................................................ 5-70
5.2.4.1.1 Isotropic material properties .................................................................. 5-70
5.2.4.1.2 Orthotropic material properties.............................................................. 5-72
5.2.4.1.3 Woven material properties ..................................................................... 5-74
5.2.4.1.4 Anisotropic material properties ............................................................. 5-75
5.2.4.1.5 Hyper-elastic material properties ........................................................... 5-77
5.2.4.1.6 Laminated Material Properties .............................................................. 5-78
5.2.4.1.7 User Material Properties ........................................................................ 5-80
5.2.4.1.8 Field Material Properties ....................................................................... 5-81
5.2.4.1.9 Piezo-resistivity Material Properties...................................................... 5-81
5.2.4.1.10 Convective Heat Material Properties ................................................... 5-82
5.2.4.1.11 Radiant Heat Material Properties......................................................... 5-83
5.2.4.2 Plastic Material Properties............................................................................. 5-84
5.2.4.3 Creep Material Properties .............................................................................. 5-89
5.2.4.4 Failure Material Properties ............................................................................ 5-91
5.2.4.4.1 Lamina Failure Values ........................................................................... 5-92
5.2.4.4.2 Plastic Lamina Failure FLW1 Values.................................................... 5-93
5.2.4.4.3 Plastic Lamina Failure FLW2 Values.................................................... 5-94
5.2.4.4.4 Laminate Failure Values ........................................................................ 5-95
5.2.5 Geometric Properties Data .................................................................................... 5-98
5.2.5.1 Geometric Properties - (WST4 and SST4) .................................................... 5-99
5.2.5.2 Geometric Properties - (SPR1 and SPR2) ................................................... 5-101
5.2.5.3 Geometric Properties - (Laminated Construction) ...................................... 5-103
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
iv
ASAS (Non-Linear) User Manual
Contents
5.2.5.4 Geometric Properties - (Rigid Surface Elements) ....................................... 5-106
5.2.5.5 Definition of geometric properties for beam elements having local axes
definition and/or rigid offsets ..................................................................................... 5-108
5.2.6 Section Data ........................................................................................................ 5-114
5.2.6.1 Section Types and Dimensions ................................................................... 5-116
5.2.6.2 Fabricated Plate Sections............................................................................. 5-120
5.2.7 Skew System Data............................................................................................... 5-123
5.2.7.1 Skew Systems - Direction Cosines .............................................................. 5-123
5.2.7.2 Skew Systems - Nodal Definition ............................................................... 5-125
5.3 BOUNDARY Conditions Data .................................................................................. 5-126
5.3.1 UNITS Command ............................................................................................... 5-126
5.3.2 FREEDOM Release Data .................................................................................... 5-126
5.3.3 SUPPRESSED Freedoms Data ........................................................................... 5-129
5.3.4 Prescribed Freedom Data .................................................................................... 5-131
5.3.5 CONSTRAINT Equation Data ........................................................................... 5-133
5.3.6 RIGID Constraints Data ...................................................................................... 5-137
5.4 Loading Data .............................................................................................................. 5-140
5.4.1 UNITS Command ............................................................................................... 5-140
5.4.2 LOADING Data .................................................................................................. 5-142
5.4.3 NODAL LOADS Data ........................................................................................ 5-143
5.4.4 PRESCRIBED Displacements, Velocities and Accelerations Data ................... 5-145
5.4.5 PRESSURE Load Data ....................................................................................... 5-146
5.4.5.1 UNIFORM Pressure Load Data .................................................................. 5-148
5.4.5.2 NON-UNIFORM Pressure Load Data ........................................................ 5-149
5.4.6 DISTRIBUTED Load Data ................................................................................. 5-154
5.4.6.1 Local Beam Distributed Loads .................................................................... 5-158
5.4.6.1.1 BL1 and BL2 Load Patterns ................................................................ 5-161
5.4.6.1.2 BL3 Load Pattern ................................................................................. 5-162
5.4.6.1.3 BL4 Load Pattern ................................................................................. 5-163
5.4.6.1.4 BL5 Load Pattern ................................................................................. 5-164
5.4.6.1.5 BL6 Load Pattern ................................................................................. 5-165
5.4.6.1.6 BL7 Load Pattern ................................................................................. 5-166
5.4.6.1.7 BL8 Load Pattern ................................................................................. 5-167
5.4.6.2 Global Beam Distributed Loads .................................................................. 5-168
5.4.6.2.1 GL1 and GP1 Load Patterns ................................................................ 5-171
5.4.6.2.2 GL4 and GP4 Load Patterns ................................................................ 5-173
5.4.6.2.3 GL5 Load Pattern ................................................................................ 5-174
5.4.6.2.4 GL6 and GP6 Load Patterns ................................................................ 5-175
5.4.6.2.5 GL7 and GP7 Load Patterns ................................................................ 5-176
5.4.6.3 Panel Edge Distributed Loads ..................................................................... 5-178
5.4.6.4 Curved Beam Distributed Loads ................................................................. 5-181
5.4.7 TEMPERATURE Load Data .............................................................................. 5-183
5.4.7.1 NODAL Temperature Data ......................................................................... 5-183
5.4.7.2 ELEMENT Temperature Data .................................................................... 5-185
5.4.7.3 UNIFORM Element Temperature Data ...................................................... 5-186
5.4.7.4 NON-UNIFORM Element Temperature Data ............................................ 5-187
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
v
ASAS (Non-Linear) User Manual
Contents
5.4.8 FACE TEMPERATURE Data ............................................................................ 5-191
5.4.8.1 Nodal Face Temperature ............................................................................. 5-191
5.4.8.2 ELEMENT FACE TEMPERATURE Data ................................................ 5-192
5.4.8.3 UNIFORM Element Face Temperature Data .............................................. 5-193
5.4.8.4 NON-UNIFORM Element Face Temperature Data .................................... 5-194
5.4.9 BODY FORCE Data ........................................................................................... 5-197
5.4.10 CENTRIFUGAL Loads Data ............................................................................ 5-198
5.4.11 ANGULAR ACCELERATION Loads Data .................................................... 5-199
5.4.12 NODAL FLUX Data ......................................................................................... 5-201
5.4.13 PRESCRIBED Field Variable Data .................................................................. 5-202
5.4.14 FLUX DENSITY Data ...................................................................................... 5-203
5.4.14.1.1 UNIFORM Flux Density Data........................................................... 5-204
5.4.14.1.2 NON-UNIFORM Flux Density Data................................................. 5-206
5.4.15 WAVE LOAD Data .......................................................................................... 5-212
5.4.16 TANK LOAD data ............................................................................................ 5-213
5.4.17 LOAD Functions ............................................................................................... 5-215
5.5 DIRECT Mass Input Data .......................................................................................... 5-217
5.5.1 UNITS command ................................................................................................ 5-217
5.5.2 LUMP ADDED MASS Data .............................................................................. 5-218
5.6 Initial Conditions Data ............................................................................................... 5-220
5.6.1 UNITS Command ............................................................................................... 5-220
5.6.2 RESIDUAL Initial Stresses................................................................................. 5-221
5.6.3 RESIDUAL Initial Stresses for Stiffeners WST4 and SST4 .............................. 5-222
5.6.4 Initial Conditions................................................................................................. 5-224
5.7 STOP Command ........................................................................................................ 5-226
6. Running Instructions ............................................................................................................... 6-1
6.1 DATA AREA Requirement ........................................................................................... 6-1
6.2 Data-Manager Parameters .............................................................................................. 6-1
6.3 File Status ....................................................................................................................... 6-3
6.4 Warnings and Errors ...................................................................................................... 6-4
6.5 Running Instructions ...................................................................................................... 6-5
6.6 ASAS Initialisation File ................................................................................................. 6-8
6.7 Extended Syntax in Data Files ....................................................................................... 6-9
6.7.1 IF/THEN/ELSE ....................................................................................................... 6-9
6.7.2 DATA REPLACEMENT...................................................................................... 6-12
6.7.3 The DEFINE Command ........................................................................................ 6-12
6.8 Secondary Data Files within ASAS-NL Data .............................................................. 6-13
6.8.1 Use of @filename command ................................................................................. 6-13
6.8.2 Notes about the @ Command ............................................................................... 6-14
6.9 Soft Halt Facility .......................................................................................................... 6-15
Appendix - A Element Description Sheets ............................................................................... A-1
A.1
Facilities Available for each Element Type ............................................................. A-1
A.2
Element Axes Systems ............................................................................................. A-8
A.2.1 Local Axes on Beam Elements ............................................................................. A-8
A.3
Beam Offsets .......................................................................................................... A-11
A.3.1 OFFS Command .................................................................................................. A-11
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
vi
ASAS (Non-Linear) User Manual
Contents
A.3.2 OFFG and OFSK Commands ............................................................................. A-12
A.3.3 OFCO Command................................................................................................. A-13
A.3.4 Finite Element Description Sheets ...................................................................... A-14
A.4
References ............................................................................................................ A-136
Appendix - B Material Models ................................................................................................. B-1
B.1 Linear Elasticity ............................................................................................................ B-1
B.1.1 Isotropic Material .................................................................................................. B-1
B.1.2 Anisotropic Material .............................................................................................. B-1
B.1.3 Orthotropic Material .............................................................................................. B-1
B.1.4 Laminated Material for Shell Elements ................................................................. B-2
B.1.5 Woven Material ..................................................................................................... B-4
B.2 Non-Linear Elasticity .................................................................................................... B-5
B.2.1 Hyperelastic Material ............................................................................................ B-5
B.3 Plasticity ........................................................................................................................ B-6
B.3.1 Yield Criteria ......................................................................................................... B-6
B.3.1.1 Von Mises ...................................................................................................... B-6
B.3.1.2 Tresca ............................................................................................................. B-6
B.3.1.3 Ivanov ............................................................................................................ B-6
B.3.1.4 Mohr-Coulomb .............................................................................................. B-7
B.3.1.5 Drucker-Prager .............................................................................................. B-8
B.3.1.6 Stress Resultant Plasticity for Beams ............................................................ B-8
B.3.1.7 Coulomb Friction ........................................................................................... B-9
B.3.1.8 Tension Cut-off .............................................................................................. B-9
B.3.1.9 Inelastic Spring .............................................................................................. B-9
B.3.2 Hardening Rules .................................................................................................. B-10
B.3.2.1 Isotropic ....................................................................................................... B-10
B.3.2.2 Kinematic ..................................................................................................... B-11
B.3.2.3 Combined ..................................................................................................... B-11
B.3.3 Equivalent Strain ................................................................................................. B-12
B.4 CREEP ........................................................................................................................ B-12
B.4.1 In-Built Creep Laws ............................................................................................ B-13
B.4.2 User Supplied Creep Laws .................................................................................. B-14
B.5 Composite Failure ....................................................................................................... B-16
B.5.1 Lamina Failure Criteria ....................................................................................... B-16
B.5.2 Laminate Failure Criteria .................................................................................... B-20
B.5.3 Failure Laws ........................................................................................................ B-22
B.5.3.1 In-Built Failure Law .................................................................................... B-22
B.5.3.2 User-Defined Failure Laws.......................................................................... B-24
B.6 User Material............................................................................................................... B-26
B.7 References ................................................................................................................... B-31
Appendix - C Solution Strategies in ASAS-NL ....................................................................... C-1
C.1 Introduction ................................................................................................................... C-1
C.2 Incremental - Iterative Procedures ................................................................................ C-3
C.2.1 Introduction ........................................................................................................... C-3
C.2.2 Basic Definitions ................................................................................................... C-7
C.2.3 Incrementation procedures .................................................................................... C-8
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
vii
ASAS (Non-Linear) User Manual
Contents
C.2.4 Iteration procedures ............................................................................................... C-9
C.2.4.1 Type of constraint surface ............................................................................. C-9
C.2.4.2 Iteration techniques ...................................................................................... C-11
C.2.5 Solution methods ................................................................................................. C-14
C.2.5.1 Euler-Cauchy method .................................................................................. C-14
C.2.5.2 Self-correcting Euler-Cauchy ...................................................................... C-15
C.2.5.3 Full incremental - iterative method.............................................................. C-15
C.2.6 Conclusions ......................................................................................................... C-16
C.3 Computation of Stresses.............................................................................................. C-17
C.3.1 Forward Euler Integration Scheme ...................................................................... C-17
C.3.2 Backward Euler Integration Scheme ................................................................... C-19
C.4 Convergence and Auto-Recovery ............................................................................... C-20
C.4.1 Convergence Check ............................................................................................. C-20
C.4.2 Auto-Recovery .................................................................................................... C-20
C.5 Eigenvalue Analysis .................................................................................................... C-21
C.5.1 Linear Pre-buckling Case .................................................................................... C-21
C.5.2 Non-linear Pre-buckling Case ............................................................................. C-21
C.5.3 Spectral Analysis ................................................................................................. C-22
C.5.4 Natural Frequency Analysis ................................................................................ C-23
C.6 Contact Analysis ......................................................................................................... C-23
C.6.1 Penalty Method .................................................................................................... C-23
C.6.2 Augmented Lagrangian Method .......................................................................... C-24
C.7 References ................................................................................................................... C-24
Appendix - D Restarts .............................................................................................................. D-1
D.1
Introduction .............................................................................................................. D-1
D.2
Initial Analysis ......................................................................................................... D-1
D.3
Restarted Jobs ........................................................................................................... D-2
D.4
Examples .................................................................................................................. D-3
Appendix - E Example Data Files ............................................................................................ E-1
E.1 Example 1: BM3D Plasticity Model (T0574) ............................................................... E-1
E.2 Example 2: TCS9 Geometric non-linearity (T0533) .................................................... E-3
E.3 Example 3: QUX4 Incompressible behaviour (T0540) ................................................ E-4
E.4 Example 4: QUS4 Elasto-plastic stiffened shell (T0553) ............................................. E-6
E.5 Example 6: QUS4 transient dynamics (T0591) .......................................................... E-12
Appendix - F List of Freedom Names .......................................................................................F-1
Appendix - G Isoparametric Elements ..................................................................................... G-1
G.1
Curvilinear Axes....................................................................................................... G-1
G.2
Integration Rules ...................................................................................................... G-1
Appendix - H ASAS/ASAS-NL Compatibility........................................................................ H-1
Appendix - I POSTNL General Post-Processor Interface Program .......................................... I-1
I.1 Introduction ......................................................................................................................... I-1
I.2 Usage .................................................................................................................................. I-1
I.3 FEMVIEW Interface........................................................................................................... I-2
I.3.1 Primary Nodal Variables ......................................................................................... I-4
I.3.2 Primary Element Based Variables ........................................................................... I-5
I.3.2.1 Rotation of Shell Element Based Variables ..................................................... I-5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
viii
ASAS (Non-Linear) User Manual
Contents
I.3.3 Secondary Element Based Variables ....................................................................... I-6
I.3.3.1 Laminated Composite Shells ........................................................................... I-6
I.3.3.2 Surface and Global Failure Indices .................................................................. I-7
I.3.3.3 Laminated Composite Bricks ........................................................................... I-7
I.4 PATRAN Interface ............................................................................................................. I-8
I.5 Printer Interface ................................................................................................................ I-10
I.6 Time Histories................................................................................................................... I-15
I.7 Rotation of Element Based Variables for Shells .............................................................. I-23
I.7.1 Introduction ............................................................................................................ I-23
I.7.2 Restrictions ............................................................................................................ I-23
I.7.3 The Plane Stress Transformation ........................................................................... I-23
I.7.4 Determination of the Rotational Angle, θ.............................................................. I-24
I.7.5 User Definition of New Local Axes Direction ...................................................... I-24
I.7.6 User Definition of Element Top and Bottom Surfaces .......................................... I-26
I.7.7 References .............................................................................................................. I-27
I.8 Fracture Mechanics Processing ........................................................................................ I-28
I.8.1 Introduction ............................................................................................................ I-28
I.8.2 Restrictions ............................................................................................................ I-28
I.8.3 Notes on the use of Fracture Parameters ............................................................... I-29
I.8.4 Format of Contour Definition File ......................................................................... I-29
I.8.5 Example ................................................................................................................. I-29
Appendix - J Creep Analysis ..................................................................................................... J-1
J.1Overview ............................................................................................................................. J-1
J.2Creep Solution Methods ..................................................................................................... J-2
J.3Convergence of Creep Solutions ........................................................................................ J-3
J.4Automatic Timestepping..................................................................................................... J-3
J.5Example Preliminary Data .................................................................................................. J-5
J.6Recommendations for Creep Analysis ............................................................................... J-5
J.7References ........................................................................................................................... J-6
Appendix - K Transient Dynamics Analysis ............................................................................ K-1
K.1
Overview .................................................................................................................. K-1
K.2
Time Integration Algorithm ..................................................................................... K-2
K.3
Automatic Timestepping .......................................................................................... K-3
K.4
References ................................................................................................................ K-9
Appendix - L References .......................................................................................................... L-1
Appendix - M Wave Loading On Offshore Jacket Structures ................................................. M-1
M.1
Introduction ............................................................................................................. M-1
M.2
Water Axes .............................................................................................................. M-1
M.3
Wave Theories ......................................................................................................... M-2
M.3.1 Conventional wave theories................................................................................. M-2
M.3.2 Shell New Wave .................................................................................................. M-2
M.3.3 Irregular Wave ..................................................................................................... M-3
M.4
Wave load data format ............................................................................................ M-5
M.5
WAVE LOAD Data ................................................................................................ M-6
M.6
Description of the Wave Load Data Block ............................................................. M-8
M.6.1 WAVE LOAD Data............................................................................................. M-8
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
ix
ASAS (Non-Linear) User Manual
M.6.2
M.6.3
M.6.4
M.6.5
M.6.6
M.6.7
M.6.8
M.6.9
M.6.10
M.6.11
M.6.12
M.6.13
M.6.14
M.6.15
M.6.16
M.6.17
M.6.18
M.6.19
M.6.20
M.6.21
M.6.22
M.6.23
M.6.24
M.6.25
M.6.26
M.6.27
M.6.28
M.6.29
M.6.30
M.6.31
M.6.32
M.6.33
M.6.34
M.6.35
M.6.36
M.6.37
M.6.38
M.6.39
M.6.40
M.6.41
M.6.42
M.6.43
M.6.44
M.6.45
M.6.46
M.6.47
Contents
AMAS Command ................................................................................................ M-9
BEAM Element Command................................................................................ M-10
Current BLOCKAGE Factor Command ........................................................... M-10
BUOYANCY Command ................................................................................... M-11
CURRENT Command ....................................................................................... M-12
DRAG Coefficients ........................................................................................... M-14
ELEVATION Command ................................................................................... M-15
END Command ................................................................................................. M-16
EXECUTE Command ..................................................................................... M-16
FREE Flooding Command .............................................................................. M-17
GRAVITY Command...................................................................................... M-18
GRID Wave Command ................................................................................... M-20
Marine GROWTH Command ......................................................................... M-27
HYDR Command ............................................................................................ M-28
Keulegan-Carpenter Number Tables ............................................................... M-32
Wave KINEMATICS Factor Command ......................................................... M-33
LFUN Data ...................................................................................................... M-34
MASS Inertia Coefficients .............................................................................. M-35
MOVE Command ............................................................................................ M-36
NANG Command ............................................................................................ M-37
NOBM Command............................................................................................ M-38
NOBO Command ............................................................................................ M-38
NOFR Command ............................................................................................. M-38
NOLO Command ............................................................................................ M-39
NOSW Command ............................................................................................ M-40
NOWI Command ............................................................................................. M-41
NOWL Command............................................................................................ M-42
OFFSET Command ......................................................................................... M-43
OUTPUT Control Command........................................................................... M-44
PEXT Command.............................................................................................. M-44
POINT Current Command............................................................................... M-45
PHASE Command ........................................................................................... M-47
PRINT Command ............................................................................................ M-49
Reynolds Number Tables ................................................................................ M-49
SLWT Command............................................................................................. M-51
SPECTRAL Command.................................................................................... M-52
Wave SPREADING Command ....................................................................... M-53
STOP Command .............................................................................................. M-54
TIDE Command .............................................................................................. M-54
TOLERANCE Command ................................................................................ M-56
UNITS Command ............................................................................................ M-56
VAXS Command ............................................................................................. M-57
VISCOSITY Command ................................................................................... M-58
VPOS Command ............................................................................................. M-58
WAVE Command............................................................................................ M-59
WIND Command ............................................................................................. M-60
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
x
ASAS (Non-Linear) User Manual
Contents
M.6.48 WPAR Command ............................................................................................ M-61
M.6.49 XMAS Data ..................................................................................................... M-63
M.6.50 ZONE Data ...................................................................................................... M-64
M.7
Valid Options Controlling Wave Load Calculation .............................................. M-65
Appendix - N Heat Analysis ..................................................................................................... N-1
N.1
Introduction .............................................................................................................. N-1
N.2
Heat Equations ......................................................................................................... N-1
N.3
Convection................................................................................................................ N-2
N.4
Radiation .................................................................................................................. N-2
N.5
Controlling a Heat Analysis ..................................................................................... N-2
N.6
Saving Heat Analysis Results................................................................................... N-3
N.7
Interfacing with Stress Analysis ............................................................................... N-4
Appendix - O Coupled Wind and Wave Load Analysis of Offshore Wind Turbine ............... O-1
O.1
Introduction .............................................................................................................. O-1
O.2
The Analysis ............................................................................................................. O-1
O.3
Data for FLXG job ................................................................................................... O-3
O.3.1 JOB Command ...................................................................................................... O-3
O.3.2 Generalized Mode Definition ................................................................................ O-3
O.4
Output from FLXG job............................................................................................. O-5
O.4.1 Generalized Matrix Files ....................................................................................... O-5
O.4.2 Generalized External Force File ............................................................................ O-5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
xi
ASAS (Non-Linear) User Manual
Introduction
1. Introduction
1.1
General Capabilities
ASAS-NL is a computer program for the static and dynamic analysis of engineering structures and components
which exhibit some form of non-linear response. It is designed for engineers to use, specifically for problems
involving plasticity, creep and large displacement effects, including buckling and gapping. For linear elastic
problems the parent program ASAS is usually more appropriate. The program is based on a finite element
formulation of the structural behaviour and uses an incremental procedure to represent the loading process and
response of the structure. A displacement formulation of the finite element method is used.
An extensive range of finite elements is provided for modelling both structures and continua. The material
models available include most popular theories of elasto-plastic behaviour and some specialist models for
failure. Large displacement effects may be taken into account where appropriate. Extensions to handle other
nonlinear effects have been allowed for in the program’s modular design, and are being developed.
ASAS-NL can treat a wide range of loadings. Loads may be presented as any combination of point forces or
moments, prescribed displacements, pressures, temperatures, body forces, centrifugal loads or angular
accelerations and may be applied incrementally or specified as a function of time.
The program is a further development of the ASAS family and, although a separate program, it is fully
compatible with other ASAS programs. Wherever appropriate the data input and output is ‘standard ASAS’.
The following ASAS programs interface with ASAS-NL through the interactive post-processing program,
POSTNL:
FEMGEN/FEMVIEW
Interactive graphical model building and results display.
In addition a number of proprietary general purpose graphics programs including PATRAN interface with
ASAS-NL to provide capabilities for model generation and results viewing.
ASAS-NL is written in FORTRAN and is readily transportable to differing computer types. The present version
is available on PC only.
ASAS-NL is thoroughly described in its documentation. This User Manual contains full instructions for using
the system, including choice of facilities, data preparation and running instructions.
Revisions of this User
Manual are circulated to all registered holders.
1.2
Using this Manual
This document is intended to serve both as a reference manual for the experienced ASAS-NL user and also as an
introduction to the program. In general the introductory and explanatory sections are contained in the first few
sections and the reference sections are placed at the end or in Appendices. The level of presentation and
background knowledge assumed of the user is adjusted to suit the complexity of the subject matter. No attempt
is made to cover the theory of finite elements or structural mechanics, but useful references are provided in
Appendix -L.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 1-1
ASAS (Non-Linear) User Manual
Introduction
Section 2 is an introduction to the types of analysis available. It contains brief descriptions of the program’s
various capabilities and also introduces terminology used in later sections.
Section 3 describes the modelling facilities that are contained in ASAS-NL. It includes information and advice
on the element and material types available and information on key features such as node numbering, local axis
systems, supports, loading and control of the program.
The data required to run the program is described in outline, in Section
4 The function of each data block type
is explained and the procedures for controlling the operations of the program are presented. This section is
essential reading for both new and experienced users.
Section 5 is intended as a reference section. It describes the format of each block of ASAS-NL data and gives
examples of their use.
In
Section 6 information relevant to specific machine installations is presented. Users should ensure that this
corresponds to their version. It contains running instructions and information for estimating size and cost
parameters together with any restrictions.
Various reference material is presented in Appendices.
Appendix -A is a key feature of the manual. It contains ‘element description sheets’, giving detailed
information about each element in the ASAS-NL library.
Appendix -B provides details of and reference to each material model available.
Appendix -C gives a description of the solution procedures used in ASAS-NL with an account of the control
options available to the user.
Appendix -D describes the Restart facility.
Appendix -E gives details of some example data files. A comprehensive series of test, verification and
educational input data files can be included with the computer programs.
Appendix -F gives a list of the names of the freedoms which may be present at a node.
Appendix -G explains the conventions for setting up local axes and the integration rules used for all
isoparametric elements.
Appendix -H lists necessary differences in data format between ASAS and ASAS-NL. These may impose
restrictions in modelling problems which are to run on both programs.
Appendix -I describes the interface program POSTNL required by various post-processors.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 1-2
ASAS (Non-Linear) User Manual
Introduction
Appendix -J gives additional instructions for creep analyses.
Appendix -K describes transient dynamic analysis.
Appendix -L contains a list of general references.
Appendix -M describes the wave loading capability in ASAS-NL.
Appendix - N describes heat analysis
Appendix - O describes coupled wind and wave load analysis of offshore wind turbines
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 1-3
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Introduction
Page 1-4
ASAS (Non-Linear) User Manual
2.
Types of Analysis Available
2.1
General
Types of Analysis Available
ASAS-NL is a general purpose computer program aimed at providing solutions to non-linear problems across
the broad field of structural mechanics. Therefore the facilities included in the program are subject to continual
enhancement as new problems arise and solution methods are improved. To accommodate this development to
the ‘state of the art’, the program has a highly modular structure communicating with a ‘data manager’ which is
tailored to the needs of non-linear analysis.
The analysis capabilities currently available include the following:
•
Static linear elastic
•
Static, non-linear incremental - STAT type
•
Transient, non-linear incremental - TRAN type
•
Eigenvalue extraction - buckling or natural frequency
•
General field
•
Piezo-resistivity - PIER type
•
Steady state heat - HEAT type
•
Transient heat - HTRA type
It should be noted that this categorisation influences the type of solution procedure which is employed by the
program and not the actual structural behaviour (thus for example a solution could be obtained to a linear elastic
problem using the non-linear incremental procedure - albeit inefficiently).
ASAS-NL solves the system of equations using the frontal solution technique. As well as an ordinary frontal
solver, an optimised frontal solution is also available that can greatly reduce the solution time and storage
requirements in medium to large problems.
2.1.1
Static Linear Elastic Solution
In general, a linear elastic problem is better tackled using the ASAS program. However, the linear elastic option
is included for applications where the model can be classified as small and/or where a linear elastic analysis is
the first tentative step in the design analysis before launching into a more expensive non-linear run. The
facilities available in ASAS-NL are generally the same as those in ASAS. The main differences are a somewhat
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 2-1
ASAS (Non-Linear) User Manual
Types of Analysis Available
reduced element library (see Section 3.1), treatment of a single loadcase at a time and the absence of the
substructuring facility. An important addition in ASAS-NL is the ability to handle generalised plane strain.
2.1.2
Static Non-Linear Incremental Solution
This category includes problems in which the non-linearity is due to any combination of the following:
•
large displacement effects
•
non-linear elastic material behaviour
•
plasticity
•
laminated composite failure behaviour
•
soil and rock-like material behaviour
•
non-linear boundary conditions (gaps and rigid surface contact)
The loading may be applied in a proportional or quite general non-proportional manner. In the latter case a
‘pseudo’ time scale is defined by the user to specify the sequence of loading.
Any given type of non-linear behaviour can be restricted to certain areas of the structural model, by use of
‘groups’ of elements and by use of different material identifiers.
The analysis procedure for these problems requires that the load is applied incrementally and the program then
provides several alternative methods for determining the structural response. These methods are a completely
flexible combination of various incremental-iterative procedures such as load or displacement incrementation
complemented by a selection of Newton-Raphson iteration techniques.
In the absence of other directives, the program automatically selects the Initial Stiffness iteration for all
increments. However experienced users can control the type of method or combination of methods, to be used
for each increment together with the order of non-linear theory required. A full explanation of the incremental
and iterative methods available is contained in Appendix -C.
2.1.3
Transient Non-Linear Incremental Solution
This category includes all problems where the material or structural response is a function of real time.
(a)
Creep Analysis
Creep is the generic term used in ASAS-NL to denote the time dependent material response associated with long
timescales. See Appendix -J for further details. Allowance has been made within the modular design of ASAS-
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 2-2
ASAS (Non-Linear) User Manual
Types of Analysis Available
NL for the more rapid time dependent material response associated with high velocity impact and metal forming
processes. These capabilities are planned for future development.
(b)
Non-Linear Transient Dynamic Analysis
Problems which require the inertia effects of the mass of the structure to be included come under the category of
transient dynamic analysis. Such an analysis is required where loading varies rapidly such as during blast from
an explosion or ground motion from an earthquake. In ASAS-NL the equations of motion are solved at discrete
points in time with the solution advancing in a stepwise manner. All the non-linear effects associated with a
static non-linear incremental solution (see Section 2.1.2) may be included in the analysis if required.
For transient dynamic analysis, the modelling of inertia (mass) is just as important as ensuring that the stiffness
characteristics are adequately represented. Three basic forms of mass matrix are available in ASAS-NL:
(i)
The program assembles the mass matrix from user specified lumped mass values at appropriate nodes to
produce a Direct Input Mass Matrix.
(ii)
The program assembles the mass matrix from the mass of each element lumped at its nodes (the Element
Lumped Mass Matrix).
(iii)
(The program assembles the mass matrix from the actual distribution of mass within each element (the
Element Consistent Mass Matrix).
These three forms can be mixed within a structure if required. The mass of selected elements can be omitted by
flagging the appropriate element topology commands. If no mass type is selected specifically, the type of
element mass matrix defaults to that given in Appendix -A.
2.1.4
Eigenvalue Extraction
In ASAS-NL, the two main applications of eigenvalue analysis are to provide solutions for stability and free
vibration problems.
The subspace iteration technique is employed to solve the eigenproblem which will
compute the lowest few eigenvalues requested by the user.
(a)
Stability Analysis
This type of analysis is used to determine the buckling loads and associated modes of the structures. The prebuckling behaviour can either be linear or non-linear. Full details concerning stability analysis are given in
Appendix C.5.1 and C.5.2.
(b)
Natural Frequency Analysis
This type of analysis provides the natural frequencies and associated vibration mode shapes of unloaded or preloaded structures.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 2-3
ASAS (Non-Linear) User Manual
Types of Analysis Available
In ASAS-NL, natural frequency analysis can be performed on free-free structures provided that a suitable shift is
specified.
Loading data need not be present for free vibration analysis but a warning message will be given. This facility
allows the user to determine natural frequencies of an unloaded structure.
Full explanation of natural frequency analysis can be found in Appendix C.5.4.
2.1.5
Steady State Heat Solution
This category provides solution to steady state heat transfer problems. The procedure is principally applied to
heat conductivity problems although secondary convective and radiative heat transfer effects may also be
included.
For this type of solution, non-linearity arises from the temperature dependency of heat transfer coefficients.
Their variations with temperature may be specified as temperature dependent material property data.
As in stress analysis, the heat input (cf loading) may be applied in a proportional or quite general nonproportional manner.
A selection of Newton-Raphson iteration techniques is available for non-linear solution as described in the static
non-linear stress analysis solution.
2.1.6
General Field Analysis
There are a wide range of engineering problems, eg electrical conductivity, ideal fluid flow and seepage through
a porous medium that are governed by Laplace’s equation. Field elements with a single degree of freedom at
each node are available for the solution of such problems.
2.1.7
Piezo-resistivity Analysis
A piezo-resistive material is one which experiences a change in electrical conductivity when the applied stress
field changes. ASAS-NL is capable of solving both the stress and the electrical field problem simultaneously.
THIS CAPABILITY IS CURRENTLY RESTRICTED AND IS NOT GENERALLY AVAILABLE.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 2-4
ASAS (Non-Linear) User Manual
Types of Analysis Available
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 2-5
Program Features
ASAS (Non-Linear) User Manual
3.
Program Features
3.1
Types of Element
The ASAS-NL library contains elements which are capable of modelling both continuum and structural forms.
The great majority are identical in their linear format to parent elements in ASAS, so that compatibility is
maintained. Specialisations are, however, introduced as required for non-linear applications.
Each type of element has a distinctive four character name, which indicates its form and number of nodes.
e.g. TCS8 - Thick Curved Shell with 8 nodes
A full description of each element type is provided in the element description sheets of Appendix -A.
Most element types are ‘isoparametric’ and have considerable versatility to model geometric and material
variations. However, excessive distortions from rectangular (or equilateral triangular) planform should be
avoided. Most element matrices are evaluated using numerical integration. The number of integration points in
the direction of the local curvilinear axes can be specified by the user, but the default values implemented in the
program are normally recommended.
The default integration rule generally corresponds to the ‘reduced
integration technique’. Appendix -G gives details of the various integration rules available, and an explanation
of local curvilinear axes.
In all elements, large displacement effects are taken into account by updating the geometry and using the
geometric stiffness matrix and non-linear geometrical relations. These relations are defined employing an
Updated Lagrangian formulation.
Elements may be placed together in ‘groups’. This is advantageous where it is required to vary, from group to
group, the type of behaviour modelled or the output printed. Certain elements must belong to their own groups
(see Appendix -A).
In the following sections elements are described according to their family.
3.1.1
Uniaxial Element
FLA2 - 2 node uniaxial constant stress element.
This element has some use as a tie/strut element, but its principal application is in association with other
elements, to represent boundary conditions and stiffeners.
3.1.2
Plane Stress/Strain Elements
These elements are essentially 2-D and are intended for problems in which a state of plane stress or plane strain
exists in the plane of the element.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-1
ASAS (Non-Linear) User Manual
TRM3
-
3 node isoparametric triangle
QUM4
-
4 node isoparametric quadrilateral
TRM6
-
6 node isoparametric triangle
QUM8
-
8 node isoparametric quadrilateral
Program Features
Unless specifically requested, the elements are plane stress elements lying in 3-D space with three degrees of
freedom per node. Special options convert them to plane strain, generalised (engineering) plane strain, or plane
stress forms with two degrees of freedom per node. In generalised plane strain, the strain normal to the plane is
everywhere uniform, but not zero. As a general rule, quadrilateral elements are to be preferred to triangles and
the higher order elements with mid-side nodes to the lower order ones.
3.1.3
Axi-symmetric Solid Elements
These elements are intended for the idealisation of 3-D solids with a rotational axis of symmetry, under
rotationally symmetric loading and support conditions
TRX3
-
3 node isoparametric triangular toroid
QUX4
-
4 node isoparametric quadrilateral toroid
TRX6
-
6 node isoparametric triangular toroid
QUX8
-
8 node isoparametric quadrilateral toroid
In general the higher order elements (QUX8 and TRX6) are better performers than the lower order ones and
quadrilaterals are to be preferred to triangles.
3.1.4
Three-Dimensional Solids
The brick family are applicable to general 3-D solids under arbitrary loading.
BRK6
-
6 node isoparametric pentahedron (wedge)
BRK8
-
8 node isoparametric hexahedron
BR15
-
15 node isoparametric pentahedron (wedge)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-2
ASAS (Non-Linear) User Manual
BR20
-
20 node isoparametric hexahedron
LB15
-
15 node isoparametric laminated pentahedron (wedge)
LB20
-
20 node isoparametric laminated hexahedron
Program Features
BR15 and BR20 are to be preferred in most situations to BRK6 and BRK8 due to their superior performance and
versatile shape.
3.1.5
Gap/Interface Elements
A family of gap/contact and interface elements are available to model interface problems in two and three
dimensions. Frictional forces can be included.
Gap elements are available to model node-to-node contact between two flexible structures.
GAP2 -can be used freely with the 2-D and 3-D elements but it is recommended that they interface with
the lower order elements.
GAPR-can be used to model tube-in-tube or external contact between two parallel tubes.
GAPX -is compatible with all the axisymmetric elements, but the lower order elements are to be
preferred.
Rigid surface interface elements are available to model contact between a structure and a rigid surface.
RGX3-rigid surface interface for use with lower order axisymmetric solid elements
RGX4-rigid surface interface for use with higher order axisymmetric solid elements
RG23-rigid surface interface for use with lower order 2-D plane elements
RG24-rigid surface interface for use with higher order 2-D plane elements
3.1.6
Plates, Shells and Beams
The plate and shell elements are isoparametric elements with six degrees of freedom per node. They are thick
curved elements with transverse shear flexibility. The interpolation for the in-plane stretching behaviour is quite
independent of the interpolation for bending. By using reduced integration they are in general satisfactory for
both thick and thin shells (say diameter- thickness ratios of up to 1000).
QUS4
-
4 node quadrilateral facet shell.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-3
ASAS (Non-Linear) User Manual
TCS6
-
6 node generally curved triangular shell
TCS8
-
8 node generally curved quadrilateral shell
TCS9
-
9 node generally curved quadrilateral shell
Program Features
Three elements are available to model stiffeners.
STF4
-
3 node isoparametric beam element with range of (closed) cross-sections
SST4
-
3 node isoparametric beam element with arbitrary open cross-section (no warping)
WST4
-
3 node isoparametric beam element with arbitrary open cross-section allowing warping
(7 degrees of freedom per node)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-4
ASAS (Non-Linear) User Manual
Program Features
Two two-noded engineering beams are available.
BEAM
-
2 node 3-D beam element, transmitting both axial forces and bending moments and
suitable for most 3-D frames includes rigid offsets
BM2D
-
2 node 2-D beam for plane frames subject to in-plane loading, allows for rigid offsets.
BM3D
-
2 node 3-D beam element, transmitting both axial forces and bending moments, suitable for
most 3-D frames, which allows for the effect of shear deformation, arbitrary local axes, and
rigid offsets.
TUBE
-
2 node 3-D beam element with hollow circular cross-section which allows for arbitrary
local axes and rigid offsets.
3.1.7
Spring/Dashpot Elements
These elements are linear or non-linear spring and/or dashpot elements with stiffness and/or damping in one
specific direction. This line of action can be fixed or varied with deformation.
3.1.8
SPR1
-
2 node spring/dashpot element with translational freedoms
SPR2
-
2 node spring/dashpot element with rotational freedoms
Linespring Elements
These elements are used to model surface flaws on a shell structure. Plasticity can be included.
LSP3
-
3 node linespring element for use with higher order shell elements on a symmetric
boundary
LSP6
3.1.9
-
6 node linespring element for use with higher order shell elements
Uniaxial Field Elements
These elements are 1-D field elements used to represent uniaxial conduction, etc.
FAT2
-
2 node uniaxial field elements
FAT3
-
3 node uniaxial field elements
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-5
ASAS (Non-Linear) User Manual
3.1.10
Program Features
Two Dimensional Plane Field Elements
These elements are used to represent plane or 2-D regions in a field analysis. No through-thickness variations of
the field variable is permitted.
TMT3
-
3 node triangular field element
QMT4
-
4 node quadrilateral field element
TMT6
-
6 node curved triangular field element
QMT8
-
8 node curved quadrilateral field element
3.1.11
Three Dimensional Solid Field Elements
These elements are used to represent 3-D continuum regions in a field analysis.
BRT6
-
6 node isoparametric wedge field element
BRT8
-
8 node isoparametric hexahedron field element
BT15
-
15 node isoparametric wedge field element
BT20
-
20 node isoparametric hexahedron field element
3.1.12
Axisymmetric Solid Field Elements
These elements are used to represent 3-D axisymmetric continuum regions in a field analysis.
3.2
TXT3
-
3 node isoparametric triangular field toroid
QXT4
-
4 node isoparametric quadrilateral field toroid
TXT6
-
6 node isoparametric triangular field toroid
QXT8
-
8 node isoparametric quadrilateral field toroid
Material Model Types
Several constitutive laws are available for material modelling. They are divided into groups of elasticity,
plasticity, creep and failure. In general all material models require elastic material data and usually data for a
plasticity, creep or composite failure model also. In addition, a user material interface is provided for users to
define their own constitutive behaviour for a material. Details of all material models are given in Appendix -B.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-6
ASAS (Non-Linear) User Manual
Program Features
Each material used in the analysis is identified by a number (the material integer) which is referenced by all
elements comprised of that material. The same material integer is used for all the properties of a single material
(i.e. for elastic, plastic and creep data).
All material properties may be temperature dependent. The relevant material values are specified at a set of
reference temperatures and the program interpolates between them for the material properties at any required
temperature.
3.2.1
Elasticity
Elasticity covers both linear elastic and non-linear elastic (temperature dependent or hyperelastic material)
models. For linear elasticity, the material can be either isotropic, orthotropic, woven, anisotropic or laminate.
For isotropic linear elastic material, the modulus of elasticity, Poissons ratio, coefficient of linear expansion and
density are generally required.
For orthotropic or woven material, the density, the three principal values of Young’s modulus, shear modulus,
Poisson’s ratio and expansion coefficient are required.
Anisotropy is defined by giving either the coefficients of the general material elasticity matrix (i.e. the stressstrain relation) or the coefficients of the compliance matrix (i.e. strain-stress relation), together with the
coefficients of linear expansion and density. The amount of information required for anisotropic material will
vary with the type of element for which it is being used. The requirements of each element type are detailed in
Appendix -A.
Laminate material is used to define composite shells and the density of the laminate may be provided. The layup
configuration and the materials used in the laminate are defined as geometric properties.
The hyperelastic material model implemented in ASAS-NL is a modified form of the Mooney-Rivlin model
which extends the original model to the compressible range. The Mooney-Rivlin model is associated with the
analysis of rubber-like materials which are almost incompressible with the bulk modulus a few orders of
magnitude larger than the shear modulus. The well known difficulties associated with this incompressibility for
finite element solutions are overcome in ASAS-NL by modifying the volumetric part of the strain-displacement
relationship. This involves a reduced order of pressure interpolation which is specified by the user as required.
The Mooney-Rivlin hyperelastic material model requires two constants, C10 and C01 to be specified by the user.
3.2.2
Plasticity
Plasticity is the generic term used in ASAS-NL to describe all time-independent non-reversible material
behaviour. It includes not only the classical plasticity theories applicable to most metals, but also some simple
theories to account for the behaviour of soils, rocks and concrete.
There are two requirements of any definition of plastic behaviour:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-7
ASAS (Non-Linear) User Manual
(i)
Program Features
A yield criterion to define the stress level at which plastic deformation first occurs and which also
provides the constitutive relationship between plastic strains and stresses. ASAS-NL has been developed
to allow separate specification of yield criterion and flow rule and hence wide generality. However, all
material models of the current version have an associative flow rule implemented and the more general
capability is not yet utilised.
(ii)
A hardening rule to define how the yield criterion is modified by subsequent plastic deformation.
3.2.2.1 Yield Criteria
The following yield criteria are available:
•
Von Mises
•
Tresca
•
Ivanov
•
Mohr-Coulomb
•
Drucker-Prager
•
Tension Cut
•
Beam Stress Resultant
•
Coulomb Friction
•
Inelastic Spring
Both von Mises and Tresca criteria are widely applied to the behaviour of metals, but experimental evidence
generally favours von Mises. The Tresca criterion is frequently used, on account of its simplicity, in analytical
solutions and is useful for validation purposes.
The Ivanov yield criterion is applicable only to plate and shell behaviour and thus is restricted to certain
elements. Yield is defined in terms of through thickness stress resultants (i.e. forces and moments per unit
width).
Both Mohr-Coulomb and Drucker-Prager criteria are applicable to soils and rock-like materials. Implicit in
these criteria is a dependence on the hydrostatic stress, which is a pre-requisite of any attempt to model soil
behaviour.
The tension cutcriterion is applicable to model concrete cracking. Failure is defined in terms of principal
stresses.
The beam stress resultant yield criterion is applicable only to the engineering beams. Yield is defined in terms of
stress resultants and the whole section is assumed to plastify instantaneously.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-8
ASAS (Non-Linear) User Manual
Program Features
The Coulomb friction criterion is only available for rigid surface elements (and implicitly to gap elements) to
model the interface behaviour.
The inelastic spring model is only applicable to the spring elements. This can be used to model the hysteretic
behaviour under cyclic loading.
3.2.2.2 Hardening Rules
Unless specifically requested, the program assumes that isotropic hardening (or softening) occurs.
This
corresponds to the yield surface expanding uniformly about the origin (for example a uniaxial model under
cyclic loading yields at the same value in both tension and compression and no Bauschinger effect is
reproduced). Isotropic hardening is usually satisfactory for problems where unloading does not occur and indeed
for cyclic loading of work hardened metals.
Kinematic hardening is available on request. The yield surface translates as a rigid surface upon plastic
deformation. With the Prager type the direction of travel is normal to the yield surface at the point concerned
and is applicable only to solids and axisymmetric solid elements. Ziegler type hardening is an attempt to
generalise Prager’s hypothesis to reduced stress spaces and results in the yield surface translating in the direction
of the stress vector. A combination of either kinematic forms with isotropic hardening is available by giving the
ratio of kinematic to isotropic hardening (see Appendix -B for further details).
The work hardening behaviour is defined by the material’s uniaxial stress-strain curve. This curve is specified
by a tabular representation of point values for varying temperatures. Linear interpolation between these point
values is used which effectively idealises the curve as a series of line segments and can be considered as
equivalent to specifying a series of slopes. A special case of this type of description gives a bi-linear work
hardening or perfectly plastic model if required.
In the absence of other directives then von Mises yield criteria and the associated Prandtl-Reuss flow equations
with isotropic hardening are assumed. The user then need take no further action.
3.2.3
Creep
Creep is the generic term used in ASAS-NL to describe all time dependent material behaviour. Creep and
plasticity models cannot be used concurrently in any one load step.
The creep material model requires the definition of a uniaxial creep strain rate and to extend this to multiple axes
the Mises potential function and associative flow rule are used. Four general ‘In-Built’ equations (“Laws”) are
available for the uniaxial creep strain rate and these optionally include strain or time hardening. The constants
for the equations are supplied by the user to match the material being modelled. If the required behaviour cannot
be defined by these then user-supplied subroutines may be added to the program to define the uniaxial rate as a
function of stress, strain, time and temperature.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-9
ASAS (Non-Linear) User Manual
Program Features
If supplying a creep subroutine users should note that many commonly used primary creep laws yield an infinite
creep rate at zero time which can cause numerical problems in the program. This can be avoided by suitable
adjustment of the creep law for times close to zero, or by providing a small offset to the time axis.
It is also important to ensure that any implied system of units in the creep law is consistent with the units being
used in the analysis.
3.2.4
Failure
Failure material models are used in ASAS-NL to describe the material failure behaviour of composite laminates.
Failure material properties may be specified to define the strength properties of a lamina, the strength properties
of the whole laminate, or, the parameters required for in-built or user defined failure laws.
3.2.5
Field
Field material properties are used in ASAS-NL to describe the ‘material’ properties for the field elements. The
actual type of properties will depend on the field problem being analysed. For example, if the electrical field
problem is being analysed, the properties will relate to the electrical conductivities.
3.2.6
Piezo-Resistivity
Piezo-resistivity material properties are used in ASAS-NL to describe the properties of a piezo-resistive material
for the coupled stress/electrical conduction problem.
3.2.7
Heat Convection
This type of material is used in ASAS-NL to model general non-linear convective heat transfer in a heat
analysis.
3.2.8
Heat Radiation
This type of material is used in ASAS-NL to model radiant heat transfer in a heat analysis.
3.3
Loading
Within ASAS-NL the word ‘LOAD’ signifies any externally imposed influence and includes prescribed
displacements and temperatures. Any number of different load types may be combined together and their
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-10
ASAS (Non-Linear) User Manual
Program Features
proportions may vary over the load history (i.e. the loading can be ‘non-proportional’). Only one loadcase can
be analysed in a single analysis.
The individual load types are listed in the following sections.
3.3.1
Nodal Loads
A nodal load is a force or moment associated with a freedom at a node. Loads may be applied in skew directions
by use of skew systems (see Section 3.6).
3.3.2
Prescribed Displacements
Prescribed displacements may be imposed on any nodal freedoms, in skew directions if required. The user first
specifies which freedoms are to be prescribed and then quotes displacement values for them. The nodal
reactions associated with each prescribed freedom are calculated automatically by the program.
3.3.3
Pressure Loads
A constant or spatially varying pressure distribution may be applied to any set of element faces. The distribution
is defined by the pressure values at the nodes on the faces. The default direction in which the pressure acts
depends on the element type and is described for each element in Appendix -A. Pressure can also be applied in
a specific direction.
For large displacement problems the pressure load is of non-conservative (follower) character. If required, this
however can be changed by the user to conservative load type (see Section 5.1 GROU/PROB/TITL command).
3.3.4
Distributed Loads
Distributed loads and intermediate point loads can be applied to some types of element as described in
Apprendix A
3.3.5
Temperature Loads
The effect of thermal straining due to a given temperature distribution can be determined. The distribution can
be defined at the nodes or on elements. Temperature loads are calculated from the difference between the
supplied nodal temperatures and a pre-specified reference temperature. (The latter is taken as zero unless
specified otherwise - see Section 4.3.4.) The required nodal temperatures can either be specified directly or
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-11
ASAS (Non-Linear) User Manual
Program Features
obtained from ASASHEAT using the HOTRAN program. (For details of the latter see the ASASHEAT User
Manual).
On higher order elements, with mid-side nodes, only corner node temperatures are required. The program will
over-ride, with interpolated values, any supplied temperatures for mid-side nodes.
Temperature fields which are discontinuous across element boundaries, can either be applied by using Groups
with nodal temperatures or element temperatures.
For problems with temperature dependent material data, material properties are evaluated at the supplied nodal
temperatures and the reference temperature is not used.
3.3.6
Face Temperature
The effect due to a difference of temperature through the thickness of a shell element can be determined. The
program requires the temperatures of both faces at some or all of the nodes. Alternatively, the face temperature
values on some or all of the elements can be specified.
On higher order elements, with mid-side nodes, only corner node temperatures are required. The program will
over-ride, with interpolated values, any supplied temperatures for mid-side nodes.
Temperature fields which are discontinuous across element boundaries, can be applied by using Groups.
For problems with temperature dependent material data, material properties are evaluated at the mid- surface
temperatures (i.e. average of top and bottom surfaces) and the reference temperature is not used.
3.3.7
Body Forces
Self weight, or the effect of uniform acceleration fields, are provided by this load type. The user specifies the
components of acceleration along each of the three global axes, and the body forces are automatically
determined for these acceleration components for all elements in the model. A density value must be specified
for all materials. The units of density and acceleration must be consistent with the units used in the remainder of
the data (see Section 3.11).
3.3.8
Centrifugal Loads
Centrifugal loading is available for most elements. It is applied by specifying the centre of rotation, together
with the angular velocity about each of the three global axes. A density value is required for all materials. The
units of density and angular velocity must be consistent with the units used in the remainder of the data (see
Section 3.11).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-12
ASAS (Non-Linear) User Manual
3.3.9
Program Features
Angular Accelerations
Angular acceleration loading is available for most elements. It is applied by specifying the centre of rotation
together with the values of angular acceleration and/or velocity about each of the three global axes. A density
value is required for all materials. The units of density, angular acceleration and velocity must be consistent
with the units used in the remainder of the data (see Section 3.11).
3.3.10
Nodal Fluxes
A nodal flux is a flux associated with freedom T at a node. This load type applies to field analysis only.
3.3.11
Prescribed Field Variables
A prescribed field variable may be imposed on the nodal freedom in a field analysis. The user first specifies
which freedoms are to be prescribed and then quotes values for them. The nodal reacted fluxes associated with
each prescribed freedom are calculated automatically by the program.
3.3.12
Flux Densities
A constant or spatially varying flux density distribution may be applied to any set of element faces or volumes.
The distribution is defined by the flux density values at the nodes on the faces or elements.
3.3.13
Wave Load
The loading due to wave, wind and current on fixed offshore structures may be included with this load type. The
envionmental loads are only applied to BEAM, BM3D and TUBE elements.
3.3.14
Tank Loads
If a floating structure has internal tanks that are filled with fluid, the combination of gravity and any motion of
the vessel will cause pressure loads on the walls of those tanks. By specifying the tank geometries together with
the internal fluid levels and densities, ASAS(NL) can automatically calculate the pressure loads on the tank
walls.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-13
ASAS (Non-Linear) User Manual
3.3.15
Program Features
Load History
The load history (or load sequence in time independent problems) and the corresponding response of the model
is defined by reference to a ‘pseudo-time’ axis. For other than creep or dynamic analyses pseudo-times have no
physical meaning; their values are used only to sequence the application of load and identify the increments.
Unless directed otherwise the program assumes a load history corresponding to a single application of a
proportionately increasing load.
More complex load histories may be specified in one of two ways. Firstly, the complete spatial load distribution
can be defined explicitly at each required pseudo-time. Proportional loading is implied between each load state.
This is usually the most convenient way when there are relatively few such load sets. Alternatively, a load
history may be specified by supplying a set of ‘load functions’ to define a few reference load states. The
functions define the proportion of each of the reference load’s components to be applied at any pseudo-time.
This allows quite general application of non-proportional loading.
For problems with cyclic loading, there is provision to repeat automatically a given load history any number of
times.
3.4
Node Numbers and Coordinates
Each node in the finite element idealisation must be given a unique positive integer number, so that an element
can be identified unambiguously by the node numbers on its boundaries. The shape and orientation of an
element is determined by the coordinates of these nodes.
If the structure has N nodes, the node number need not necessarily be within the range 1 to N; gaps in the
numbering are allowed and are often helpful. The gaps should preferably be small (eg. less than N).
The geometry of the elements and of the structural model is defined by the coordinates of the nodes. In general,
the coordinates must be supplied for all nodes on the structure. However, for elements with straight edges the
coordinates of any mid-side nodes can be calculated by the program.
The coordinates of a node or group of nodes may be defined in any convenient rectangular cartesian, cylindrical
polar or spherical polar coordinate system. An idealisation may use several of these coordinate systems. The
only exception is an axisymmetric idealisation where the cylindrical polar coordinates which are implicit in the
element must be input as a cartesian system.
The relationship of coordinate local axes or skew systems to the global system is given by the direction cosines
of their axes relative to the global axes. Each direction cosine gives the projection of a unit vector along the
skew axis on to the global axis. Skew systems must be right-handed and orthogonal.
It is only necessary to specify two of the axes; the third is computed automatically. If X’, Y’, Z’ represent the
skew axes, and X, Y, Z the global axes, ASAS-NL requires the six direction cosines:
X’X, X’Y, X’Z, Y’X, Y’Y, Y’Z
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-14
ASAS (Non-Linear) User Manual
Program Features
where, for example X’X is the projection on to the global X axis of a unit vector along the skew X’ axis. For a
2-D system within the X-Y plane, both X’Z and Y’Z will be zero.
As an alternative to specifying the direction cosines of the local axis system with respect to the global axis
system, a set of three node numbers may be used to identify the skew system, with ASAS-NL automatically
calculating the direction cosines (see Section 5.2.7.2).
3.5
Element Numbering
The program numbers elements automatically in the order in which they are first defined (the “input element
number”). Alternatively users can number each element explicitly (“user element number”). The user element
number (which defaults to the input element number if it is not given) is used as an identifier to specify the
group structure, integration rules and order of output.
Elements are defined by their constituent node numbers. The starting node and order of numbering (clockwise
or counter-clockwise) determines the direction of the local curvilinear axes. (See Appendix -G).
The program reorders the elements internally (the “system element number”) in an attempt to keep the maximum
frontwidth as small as possible. It allocates system element numbers on the basis of least node number order.
Elements are then assembled into the front of this order. Special options may be used, however, to suppress this
reordering and to use either the user or input element order within the solution process. (See MYEL and INEL
options)
If no attention has been paid to the node number sequence, which will effect the order of system element
numbering, the frontwidth optimiser can be invoked, using the PASS command, to reduce the incore frontwidth.
Five different methods are available in the program, namely CUTHILL-MCKEE, KING, LEVY, PINA and
SLOAN. CUTHILL-MCKEE is basically an algorithm for out-of-core bandwidth reduction but it may also be
used to optimise the incore frontwidth effectively. The others, however, are all methods for incore frontwidth
optimisation but, apart from SLOAN, they do take significantly more time to do the optimising (typically an
order of magnitude or more per pass compared with CUTHILL-MCKEE). This increase can be offset by use of
the user defined START node facility to reduce the number of passes attempted. The revised system element
ordering is carried out internally without renumbering the nodes and therefore its operation is transparent to the
user. Since the element ordering will be changed when using the frontwidth optimiser, the user or input element
order options should not be specified.
3.6
Global and Local Axis Systems
Regardless of the system(s) used to define coordinates, the displacement freedoms within ASAS-NL are usually
referred to the global axis system. This is a right-handed rectangular cartesian (X,Y,Z) system, except for the
axisymmetric elements, which use a cylindrical polar system (R,Θ,Z). In some cases the global axis system is
replaced for selected nodes or elements by a local axis system. There are three broad types of these: coordinate
local axes, element local axes and nodal local axes. The latter are known as ‘skew systems’.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-15
ASAS (Non-Linear) User Manual
3.6.1
Program Features
Coordinate Local Axes
Coordinate local axes are used to define the positions of nodes in space. Any required combination of cartesian,
cylindrical polar or spherical polar systems may be used; all of them are transformed to the global system within
the program. For each local system, the user provides the origin and the direction cosines relative to the global
system. Coordinates may, of course, be entered directly in the global system if required.
3.6.2
Element Local Axes
Many types of element have their own local axes. These are used as the reference frame for stress and strain
results and also, in certain elements, for the geometric properties. The direction of the element local axes is
defined by the order and location of the nodes on the elements and in large displacement analyses will vary
throughout the analysis. Full details are given in the relevant element description sheets in Appendix -A.
3.6.3
Skew Systems
Skew systems, otherwise known as nodal local axes, can be used for three purposes:
(i)
To specify suppressions, prescribed displacements or constrained freedoms (see Section 3.7) in directions
other than those of the global axis system. All output of displacements and reactions is related to this new
axis system. Only one such skew system is permitted at a node.
(ii)
To specify nodal loads in a direction other than the reference system, where the reference system is either
the global system or the global system as modified by a skew system defined in (i). For example, if a
node is skewed to allow a skew suppression, and a nodal load is required in the global direction, then a
further skew system is required to ‘re-skew’ the load back to the global system. Nodal loads applied with
a skew system are transformed to their components in the reference system described above. The axis
system at the node is not altered and hence any number of skew systems may be applied at a node to
accommodate various skewed nodal loads.
Each skew system is defined by a unique integer number - the skew integer. The same skew system may
be referred to in several places in the data.
The relationship of coordinate local axes or skew systems to the global system is given by the direction
cosines of their axes relative to the global axes. Each direction cosine gives the projection of a unit vector
along the skew axis onto the global axis. Skew systems must be right-handed and orthogonal. See
Section 5.2.7.1.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-16
Program Features
ASAS (Non-Linear) User Manual
It is only necessary to specify two of the axes: the third is computed automatically. If X’, Y’, Z’
represent the skew axes and X,Y,Z the global axes, ASAS-NL requires the six direction cosines:
X’X, X’Y, X’Z, Y’X, Y’Y, Y’Z
where, for example, X’X is the projection onto the global X axis of a unit vector along the skew X’ axis.
For a two-dimensional system within the X-Y plane, both X’Z and Y’Z will be zero.
A skew system may also be defined in terms of 3 points whose coordinates are defined in the coordinate
data. See Section 5.2.7.2.
(iii)
To specify the direction of the data supplied for anisotropic material properties. Anisotropic material
properties normally align with the element local axis system or the global axis system. By specifying a
skew integer on the material property data line it is possible to input material data in an alternative
direction. See Appendix B.1 for further details.
3.7
Structural Suppressions and Constraints
The movement of a node in any direction may be restrained by applying ‘suppressions’, or given a value by
applying ‘prescribed displacements’. These may be applied to any freedom existing at the node and may be
related to the global axis system or to a skew system defined for the purpose. (The freedoms at a node are
determined by the elements meeting at the node.) ASAS-NL automatically calculates the reactions associated
with such restraints. A freedom may also be made to depend linearly on any number of other freedoms by
means of ‘constraint equations’.
For static analysis, it is essential to ensure that there are sufficient restraints on the idealised model to prevent
any possibility of it behaving as a mechanism. In particular, the model or any part of it,should be prevented
from moving or rotating as a rigid body.
3.8
3.8.1
Solution Procedures
Non-Linear Static Solution Procedures
The non-linear static solution procedures available in ASAS-NL are conventional incremental ones, with
iterative correction within the increment. The user has wide ranging capabilities to control the nature and size of
the increment, and to vary the frequency of updating of the stiffness matrix, the required number of iterations,
convergence criteria and restart procedures to be invoked in the event of non-convergence.
The solution procedure commences by incrementing one of the following quantities (chosen by the user)
Generalised Load
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-17
ASAS (Non-Linear) User Manual
Program Features
Single Displacement Component
Displacement Vector Length (“arc-length” method)
External Work Measure
and then holding a value of the selected quantity constant throughout the iteration process.
The above procedures may be freely combined with any of the following iteration techniques
Standard Newton Raphson
Modified Newton Raphson
Initial Stiffness.
In all cases the iteration process can be accelerated by employing
Secant-Newton
or
Line Search
techniques.
The Load Incrementation procedure is most suitable for cases of non-proportional loading. The other procedures
are useful for problems involving multi-valued load-displacement relationships such as ‘snap-through’.
Solution procedures usually can be changed during the course of an analysis. In addition analyses may be restarted from previous load increments using a different solution strategy if required.
Appendix -C describes the inter-relationship of the different methods.
The size of increment, which may be either load or displacement, is normally determined by the user. However,
in problems with proportional loading, the program can automatically determine initial plastic yield (or scale to a
user defined level).
Convergence is, by default, assessed against residual forces. Displacements, element strains, stresses or total
work may also be used.
Computation of stresses adopts the Forward Euler Integration Scheme by default and sub-incremental
procedures for plastic stress redistribution may be used in conjunction with any solution procedure upon request.
For von Mises yield criterion, Backward Euler integration scheme may also be used.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-18
ASAS (Non-Linear) User Manual
3.8.2
Program Features
Non-Linear Transient Solution Procedures
Non-linear transient solution procedures are used in ASAS-NL to solve creep (time-dependent material
response) problems, structural dynamics problems and transient thermal problems. These types of problems use
a finite difference in time where the solution is advanced in a stepwise fashion using finite increments of time
(time steps). Two distinct types of solution procedures are available; implicit and explicit schemes. The implicit
scheme has the advantages of unconditional stability and allows larger timesteps compared to the alternative
explicit scheme. The iterative nature of the implicit scheme ensures, in general, greater accuracy but at a much
computational cost. In structural dynamics the two schemes may be combined in a single analysis to take of the
benefits of both schemes. In addition to defining the list of solution times manually, automatic timestepping
procedures are also available for both types of transient analyses. Further details concerning creep analysis may
be found in Appendix -J. Further details concerning structural dynamics analysis may be found in Appendix -K.
Further details concerning transient thermal analysis may be found in Appendix N.
3.8.3
Contact Analysis Solution Procedures
By default, the penalty method is adopted to solve problems involving gap and rigid surface elements. For rigid
surface contact, the augmented Lagrangian method may be used upon request. Further details for these two
methods are given in Appendix C.6.
3.8.4
Fracture Mechanics Solution Procedures
Depending on the nature of an analysis, fracture mechanics analysis may be performed in one of the following
ways:
(i)
Surface flaws on shell structures - use linespring elements and perform the analysis using any of the nonlinear static solution procedures
(ii)
Cracks on 2-D planar or axisymmetric structures - perform the analysis as usual and save the appropriate
results on the post-processing file for POSTNL to evaluate the fracture mechanics parameters (e.g. Jintegral) (see Appendix I.8)
3.9
Program Organisation
ASAS-NL makes extensive use of files and it is helpful to classify these as either internal or external files.
INTERNAL files are used for intermediate storage within a program and are deleted upon successful completion
of the program.
EXTERNAL files are permanent and are used for transporting information between the
programs and between successive restarts. The user need not normally concern himself with internal files, but
some understanding of the external file organisation is required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-19
ASAS (Non-Linear) User Manual
Program Features
When a restart is attempted information describing the current state of the analysis is required. Thus ASAS-NL
allows the user to archive (or save) all relevant information at the end of any increment. This information is
stored on two labelled external backing files. One file, called the STIFFNESS MATRIX ARCHIVE FILE (or
stiffness file) contains all the element stiffness matrices for the model. The other file, the DATA-MANAGER
ARCHIVE FILE (sometimes abbreviated to archive file) contains all other necessary information such as model
description, control parameters, load history, stresses and displacements. When the information is written to the
archive files, an integer number known as the CHECKPOINT number is used to identify the position of the
archived information on the backing file for that load increment and is printed in the output file when the
archiving has been accomplished. The two backing files are checkpointed separately.
When a restart is attempted, the internal file structure is re-created from the archived backing files using the
checkpoint number supplied by the user in the restart data.
Distinction is made between ‘OLD’ and ‘NEW’ files in ASAS-NL to distinguish between the two pairs of files
used in a restarted analysis.
Backing files created by ASAS-NL (as output) are referred to as ‘NEW’
(Newarchive and Newstiffness) whilst backing files read by ASAS-NL (as input in restarts for instance) are
referred to as ‘OLD’ (Oldarchive and Oldstiffness). For example, the data manager archive file named, say
NLARCHIVE, by the user is understood to be the newarchive file when created but the oldarchive file when
read by ASAS-NL when the restart is attempted.
ASAS-NL also makes full use of the ASAS file system. All the runs associated with a particular analysis, i.e.
the initial run and any restarts and post-processing runs, must be under a common project name. This name is
used to set up a project index file (the 10 file) which stores the details of every run carried out in this project.
The ASAS backing files created during a run are controlled by the structure name specified. A unique structure
name must be assigned for each run within the same project.
3.10 Post-Processing
A post-processing program called POSTNL is available to provide an interface for transferring ASAS-NL results
to a number of graphical display programs and to perform certain additional post-processing calculations. The
information saved on the post-processing file is specified by the POST or RESU command in the preliminary
data.
In addition, post-processing of ASAS-NL results may also be carried out using standard ASAS post-processors
such as BEAMST, AXL and AMC. As before, the POST/RESU Command in the preliminary data is required to
specify the information to be saved on the ASAS database. The increment number where results are saved will
be recognised as the user load case number by the ASAS post-processors.
3.11 Data Units
The user is free to choose any system of units for his data, provided that the units employed form a consistent
system so that all data are defined using the same units of force and length. It is also possible to define explicitly
the units for the analysis. These can be locally overridden or changed within each data block if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-20
Program Features
ASAS (Non-Linear) User Manual
The basic global units to be employed are defined in the Preliminary data using the UNITS command (see
Section 5.1.42) where the units of force, length and, where appropriate, temperature are supplied. (Time is
assumed to be in seconds). These basic units will be utilised as the default input and results units.
In order to facilitate the utilisation of different units for the various types of data, a units command can be used
within the main body of the data to locally override the basic units defined in the Preliminary data. This facility
enables each data block to have one or more different sets of data units which may or may not be the same as the
global definitions.
The following example shows a simple structure where the basic global units are Newtons and Metres but the
geometric properties have been supplied in both millimetres and inches.
Defined units
Derived units
SYSTEM DATA AREA 5000000
PROJECT ASAS
STRUCTURE ASAS
JOB STAT
TITLE *EXAMPLE
SOLV 1.0
OPTIONS GOON END
UNITS
N
M
END
COOR
CART
1
0.0 0.0 0.0
2
10.0 0.0 0.0
3
20.0 0.0 0.0
END
ELEM
MATP 1
BEAM 1
2
1
BEAM 2
3
2
END
GEOM
UNITS
MM
1 BEAM 108.0 90.0 90.0 25.5
UNITS
INCHES
2 BEAM
12.0
5.0
5.0
3.2
END
MATE
1
2.0E11 0.3
0.0
0.0
END
..
.
Newtons Metres Kg
Centigrade (default)
Newtons Millimetres
Kgx10-3
Newtons Inches. See note 3 below
Newtons Metres
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Kg
Page 3-21
ASAS (Non-Linear) User Manual
Program Features
Notes
1.
The units defined in the Preliminary data must be given for both force and length. The temperature unit is
optional and defaults to centigrade. The mass unit is a derived quantity consistent with the units of length
and force specified.
2.
Locally defined units will be reset at the end of each data block or sub data block (see Section 5.1.42).
Thus in the example above the units for the MATE data are reset to the global terms Newtons and metres
automatically.
3.
In the second units definition in the GEOM data, the force and length units do not form a consistent set
and so a mass unit cannot be derived. This is acceptable to the program provided that the data being
defined do not require a mass or density input. Thus units of Newtons and inches would be unacceptable
in the MATE data where the density is specified. Table 3.1 provides a list of unit definitions which
permit the calculation of a consistent mass unit.
4.
Where mass data has to be supplied, the input can be simplified by locally choosing the appropriate units
of force and length to provide a consistent unit of mass of either 1kg (using Newtons and metres) or 1lb
(using Poundals and feet).
If units are employed, the cross checks and results will, by default, be printed in the basic global units defined in
the Preliminary data and any data defined using local unit definitions will be factored appropriately.
Where the UNITS command is not used, the user must ensure that all data utilise a consistent system of units
throughout. Three examples of consistent sets are shown below.
1.
SI Units :
Force in Newtons, length in metres, mass in kilograms, time in seconds, acceleration
in metres/sec2
2.
Imperial Units :
Force in pounds, length in feet, mass in slugs, time in seconds, acceleration in
feet/sec2
3.
Imperial Units :
Force in poundals, length in feet, mass in pounds, time in seconds, acceleration in
feet/sec2
For any other set of units, the unit of consistent mass will be a multiple of the basic unit of mass because it is a
derived unit. The consistent unit of mass is obtained by dividing the unit of force by the acceleration due to
gravity, which itself has units of length divided by time squared. A change in the unit of length, for example
from feet to inches or metres to millimetres, requires a corresponding change to the unit of mass used for
calculating the density.
A list of sets of consistent units is given in Table 3.1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-22
Program Features
ASAS (Non-Linear) User Manual
Unit of force
Newton
Unit of
Typical value
length
of E for steel
metre
2.1x10
11
7
Newton
cm
2.1x10
Newton
mm
Kilopond
G
9.81
Consistent
unit of mass
1Kg
Density (mass/unit volume)
Steel
Concrete
7850
2400
-5
2.40x10-5
981
100Kg
7.85x10
2.1x105
9810
1000Kg
7.85x10-9
2.40x10-9
metre
2.14x1010
9.81
9.81Kg
800
245
Kilopond
cm
2.14x106
981
981Kg
8.00x10-6
2.45x10-6
Kilopond
mm
2.14x104
9810
9810Kg
8.00x10-10
2.45x10-10
KNewton
metre
2.1x108
9.81
103Kg
7.85
2.40
KNewton
cm
2.1x104
981
105Kg
7.85x10-8
2.40x10-8
KNewton
mm
2.1x102
9810
106Kg
7.85x10-12
2.40x10-12
Tonne (f)
metre
2.14x107
9.81
9.81x103Kg
0.800
0.245
Tonne (f)
cm
2.14x103
981
9.81x105Kg
8.00x10-9
2.45x10-9
Tonne (f)
mm
2.14x101
9810
9.81x106Kg
8.00x10-13
2.45x10-13
Poundal
foot
1.39x1011
32.2
1lb
491
150
8
Poundal
inch
9.66x10
Pound (f)
foot
4.32x1011
-2
7.23x10-3
386
12lbs
2.37x10
32.2
32.2lbs
15.2
4.66
(1 slug)
386
386lbs
7.35x10-4
2.25x10-4
4.32x106
32.2
3.22x104lbs
1.52x10-2
4.66x10-3
inch
3.0x104
386
3.86x105lbs
7.35x10-7
2.25x10-7
Ton (f)
foot
1.93x106
32.2
7.21x104lbs
6.81x10-3
2.08x10-3
Ton (f)
inch
1.34x104
386
8.66x105lbs
3.28x10-7
1.0x10-7
Pound (f)
inch
3.0x10
Kip
foot
Kip
7
Table 3.1 Examples of Consistent Sets of Units
1 Kip = 1000 pounds force
1 Kilopond = 1 Kilogram force
All times are in seconds
Assumed specific gravity of steel = 7.85
Assumed specific gravity of concrete = 2.4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 3-23
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Program Features
Page 3-24
ASAS (Non-Linear) User Manual
4.
Data Preparation
4.1
General
4.1.1
Data Preparation
Data
Data for ASAS-NL is prepared as a series of ‘data blocks’, each specifying a particular feature of the problem.
The data blocks are grouped into a number of sections such as structural description, boundary conditions,
loading, etc. These data blocks are shown in Table 4.1.
The various sections must be entered in order, but within each section the order of the data blocks can be varied,
although the user is advised to adopt the order shown. The sections for structural description, boundary
conditions, loading, additional mass and initial conditions collectively define the finite element idealisation. The
Preliminary data controls the solution of the problem including the type of material and structural behaviour that
is sought.
The Preliminary data is compulsory and all the data blocks of the structural description section must be present
except for the geometric properties and skew systems which are not always needed.
At least one data block from the boundary conditions section and one from the loading section must be present
for static analysis. For natural frequency analysis loading is optional. Other sections are optional.
In a restarted analysis only the Preliminary data, suppressions, displaced freedoms, loading and additional mass
can be changed. Initial conditions have no relevance.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-1
ASAS (Non-Linear) User Manual
Data Preparation
Data Block Contents
Section
Preliminary Data
Control Parameters.......... ....................................................................... 5.1
Structural Description - Shape and Properties of the Model
Coordinates ..................... .................................................................... 5.2.2
Element Topology ........... .................................................................... 5.2.3
Material Properties .......... .................................................................... 5.2.4
Geometric Properties ...... .................................................................... 5.2.5
Section Information ............................................................................. 5.2.6
Skew System ................... .................................................................... 5.2.7
Boundary Conditions - Restraints on the Model
Suppressions ................... .................................................................... 5.3.3
Displaced Freedoms ........ .................................................................... 5.3.4
Constraint Equations ....... .................................................................... 5.3.5
Rigid Constraints ............ .................................................................... 5.3.6
Loading Applied to the Model
Nodal Loads .................... .................................................................... 5.4.3
Prescribed Displacements .................................................................... 5.4.4
Pressure Loads ................ .................................................................... 5.4.5
Distributed Loads ............ .................................................................... 5.4.6
Temperature Loads ......... .................................................................... 5.4.7
Face Temperatures .......... .................................................................... 5.4.8
Body Forces .................... .................................................................... 5.4.9
Centrifugal Loads............ .................................................................. 5.4.10
Angular Acceleration ...... .................................................................. 5.4.11
Nodal Flux ...................... .................................................................. 5.4.12
Prescribed Field Variable ................................................................... 5.4.13
Flux Density .................... .................................................................. 5.4.14
Wave Load ...................... .................................................................. 5.4.15
Tank Loads ..................... .................................................................. 5.4.16
Load Functions................ .................................................................. 5.4.17
Additional Mass
Lumped Mass Values ...... ....................................................................... 5.5
Initial Conditions
Residual Initial Stresses
................................................................... 5.6.2
Stiffener Residual Initial Stresses ........................................................ 5.6.3
Initial Conditions for Transient Dynamic Analysis ............................. 5.6.4
End of File
STOP Command ............. ....................................................................... 5.7
Table 4.1 Data Blocks for ASAS-NL Data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-2
ASAS (Non-Linear) User Manual
4.1.2
Data Preparation
Data Formats
4.1.2.1 General Principles
The input data for ASAS-NL are specified according to syntax diagrams similar to that shown below. The
conventions adopted are described in the following pages. Detailed descriptions for each of the data blocks can
be found in Section 5
HEADER
KEYWORD
(alpha)
/integer/
KEYWORD1
real
//integer//
KEYWORD2
integer
KEYWORD3
real
END
Each data block commences with a compulsory header line and terminates with an END command which delimit
the information from the other data. The sequence of the input data follows the vertical line down the left hand
side of the page. If a data block can be omitted, this will be indicated as shown below.
HEADER
END
Within each data block, each horizontal branch represents a possible input instruction. Input instructions are
composed of keywords (shown in upper case), numerical values or alphanumerics (shown in lower case
characters), and special symbols. Each item in the list is separated from each other by a comma or one or more
blank spaces.
Numerical values have to be given in one of two forms:
(i)
If an integer is specified a decimal point must not be supplied.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-3
ASAS (Non-Linear) User Manual
(ii)
Data Preparation
If a real is specified the decimal point may be omitted if the value is a whole number.
Exponential formats may be utilised where real numbers are required.
for example
0.004
4.0E-3
4.0D-3
are equivalent
similarly
410.0
410
4.10E2
are the same.
Alphanumerics are any non-numeric strings which may include the letters A-Z, numbers 0-9, and the characters :
. , +
- and /. The letters A-Z may be supplied in either upper or lower case but no distinction is made
between the upper and lower case form. Hence “A” is assumed identical with “a”, “B” with “b” and so on.
For example
CASE
are all permissible alphanumeric strings
STR1
END
3mm
also
COMB
are all identical strings
Comb
comb
Alphanumeric strings must not include any special symbols (see below).
If certain lines are optional, these are shown by an arrow which bypasses the line(s)
real
integer
In order to build up a data block, a line or series of lines may be repeated until the complete set has been defined.
These are shown by an arrow which loops back.
HEADER
real
integer
END
Some data lines require an integer or real list to be input whose length is variable. This is shown by a horizontal
arrow around the list variable.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-4
ASAS (Non-Linear) User Manual
real
Data Preparation
integer
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-5
ASAS (Non-Linear) User Manual
Data Preparation
Where one or more possible alternative items may appear in the list, these are shown by separate branches for
each
KEYWORD1
integer
integer
KEYWORD2
KEYWORD3
real
An optional item in a line will be enclosed in brackets e.g.
KEYWORD
(alpha)
integer
The relevant data block description in Section 5 will detail the default value adopted if the item is omitted.
An input line must not be longer than 80 characters. Certain input instructions may extend onto continuation
lines. Where this is allowable, the syntax diagram line is shown ending with an arrow (see Section 4.1.3).
KEYWORD
4.1.3
integer
Special Symbols
The following is a list of characters which have a special significance to the ASAS-NL input.
*
An asterisk is used to define the beginning of a comment, whatever follows on the line will not be
interpreted. It may appear anywhere on the line, any preceding data will be processed as normal. For
example
’
(i)
*
(ii)
X Y RZ 1 16 24 27 *support conditions at ground level*
THIS IS A COMMENT FOR THE WHOLE LINE
single quotes are used to enclose some text strings which could contain otherwise inadmissible characters.
The quotes are placed at each end of the string. They may also be used to provide in-line comments
between data items on a given line. For example
BM3D
’NODES’
1
2
’GEOM PROP’
5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-6
ASAS (Non-Linear) User Manual
,
Data Preparation
A comma or a blank will act as a delimiter between items in the line. For example
5, 10, 15 is the same as 5
10
15
Note that two commas together signify that an item has been omitted. This may be permissible for
certain data blocks. For example
5,, 15
Unless otherwise stated in the section describing the data block omitted numerical values are zero.
:
A colon at the start of the line signifies that the line is a continuation from the previous line.
For example
is the same as
5
:
10
:
15
5
10
15
Note that this facility is only available in certain data blocks. See the appropriate detailed description of
each data block for details.
@
A command @filename may appear anywhere in a data file. When such a command is encountered, the
input of data switches to the file filename and data continues to be read from that file until either the endof-file is reached or an @ command is encountered in the secondary file.
When the end of the secondary file is reached, that file is closed and input switches back to the previous
data file. If, however, an @ command is found in the secondary file, input switches to yet another file.
This process can continue until a maximum of 5 secondary files are open simultaneously.
For example
@prelim.dat
@section1.dat
@section2.dat
@load.dat
section1.dat might then contain the lines
@coor.dat
@elem.dat
@mate.dat
@geom.dat
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-7
ASAS (Non-Linear) User Manual
Data Preparation
finally
coor.dat contains the coordinate data
elem.dat contains the element data
etc
4.2
Data Generation Facilities
4.2.1
Repeat Facilities
Lists of regular data can often be shortened by use of a repeat facility. A block of one or more lines of data may
be identified by a delimiter character(/) and terminated by a repeat command (RP). The repeat command
contains information on how many times the set of lines of data is to be generated and how the data is to be
incremented for each generation. The general form is:
/
/
KEYWORD
real
/integer/
RP
nrep
incr
: delimiter character to identify the start of the data to be generated. It must be on a line of its
own
KEYWORD
: items not enclosed within two slashes will be repeated without any increment for generated
real
/integer/
:
data
: indicates the data in the line which may be generated using the repeat facility. The slashes
must not appear in the actual data
RP
: command word to identify the end of the data to be generated
nrep
: number of times the set of lines is to be generated, including the original data line(s)
incr
: the increment to be added to the data items each time the block is generated
For example, suppose the data format is specified as
KEYWORD
/integer/
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-8
ASAS (Non-Linear) User Manual
Data Preparation
It is required to generate integers 1,6,11,16,21,26,31,36,41,46. If the keyword is ALL the data could be
ALL
1
6
11
16
21
26
31
36
41
46
or
ALL
1
ALL
ALL
6
11
.
.
.
ALL
46
Using the repeat facility, the following examples all produce the same identical data
/
ALL
RP
10
5
or
/
ALL
1
6
RP
5
10
or
/
4.2.2
ALL
1
ALL
RP
6
5
10
Re-Repeat Facilities
The repeat facility can be extended to include a double repeat whereby data which has been expanded by use of
the RP command may be repeated again with different increment values. The general form is
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-9
ASAS (Non-Linear) User Manual
Data Preparation
//
/
KEYWORD
real
//integer//
RP
nrep
incr1
RRP
nrrep
incr2
//
: identifies the start of the data to be re-repeated. It must precede a / line
/
: identifies the start of the data to be repeated
KEYWORD
: items not enclosed within two slashes will be repeated without any increment for generated
real
//integer//
:
data
: an item enclosed by // characters indicates data which can be modified using the re-repeat or
repeat facility. The slashes must not appear in the actual data
RP
: identifies the end of the data to be generated with the repeat facility
nrep
: number of times the block of data is to be generated, including the original data line(s)
incr1
: the increment to be added to the data items for the second and subsequent generated blocks.
(The first block corresponds to the original data)
RRP
: identifies the end of the data to be generated with the re-repeat facility
nrrep
: the number of times the expanded data from the repeat block is to be further generated,
including the original repeat block
incr2
: the increment to be added to each of the expanded data items for the second and subsequent regenerated blocks. (The first block corresponds to the expanded data items)
For example, taking the previous example, if the data syntax was specified as
KEYWORD
integer
then the data could be
//
/
ALL
1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-10
ASAS (Non-Linear) User Manual
RP
RRP
5
2
Data Preparation
generates 1,11,21,31,41
generates 6,16,26,36,46
10
5
Note, the order of the numbers generated by this example in Section 4.2.1 using RP and in Section 4.2.2 using
RP and RRP is different. This may be important in a few cases where the order of the data supplied matters, for
example, the generation of user element numbers.
4.2.3
List Generation in the Preliminary Data Section
Many of the commands in the Preliminary data require a list of integer data items following the keyword. This
list can be created in a number of ways.
4.2.3.1 A Simple List
A simple list of integers can be written in free format with each number separated by a space or comma up to
column 80.
Example:
1
6
11
16
17
18
1, 6, 11, 16, 17, 18
4.2.3.2 Generating a List with a Topological Variable
By use of ’topological variables’, a list of integers can be generated. This is very valuable for generating lists of
regular numbers. It is not so useful for irregular lists.
GENERATING A LIST OF NUMBERS USING ONE MODIFIER
The most basic form of topological variable has the form (L)(N,M1). This is used to generate a list of L numbers
at equal intervals. The first pair of brackets encloses the number L. The second pair of brackets encloses two
integers, separated by a comma. The first of these integers, N, is the start value and the second integer, M1, is
the increment for modifying the start value. Thus, the numbers N, N+M1, N+2M1, N+3M1 .......N+(L-1)M1 will
be generated.
Example:
(4) (3, 5)
This example will generate data for the four nodes 3, 8, 13, 18.
GENERATING A LIST OF NUMBERS USING TWO MODIFIERS
A more general form of the topological variables is as follows:
(L)(N,M1,M2)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-11
ASAS (Non-Linear) User Manual
Data Preparation
This is used to generate a list of numbers at unequal intervals. Its application is similar to the topological variable
with a single modifier. The second modifier M2 is used to change the value of M1 every time the latter is used.
Modifiers may be positive or negative. The rules are as follows:
(a)
The first number generated is the basic number N.
(b)
The second number generated is N+M1.
(c)
M1 is now modified by M2.
(d)
The next number generated is the previous number modified by the new M1.
(e)
Stages (c) and (d) are repeated until L numbers are generated.
Examples:
(i)
The topological (5) (7,3,12) variable will create a list 7, 10, 25, 52, 91 by expanding in the following way:
First number generated:
7
Second number generated:
7+3
10
10+15
25
25+27
52
New M1 = 3 + 12 = 15
Third number generated:
New M1 = 15 + 12 = 27
Fourth number generated:
New M1 = 27 + 12 = 39
Fifth number generated:
52+39
(ii)
(4) (25,2,-6) generates 25,27,23,13
(iii)
(4) (2,0,3)
(iv)
(4) (25,2,-6)
91
generates 2,2,5,11
(3) (2,3,3)
generates 25,27,23,13,2,5,11
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-12
ASAS (Non-Linear) User Manual
4.3
4.3.1
Data Preparation
Description of Each Data Block
The Preliminary Data
4.3.1.1 General
The Preliminary data is the first block of ASAS-NL data and consists of all the information required to control
the execution of the analysis. It can be divided into two sections, depending on whether the data applies to the
problem as a whole (Problem section) or whether it is specific to a given group (Group section). Commands for
the Problem section appear first and are then followed by Group section commands for each group in turn.
Groups are defined by their constituent elements, if none are explicitly given then the program treats all elements
as being in Group 1.
Collectively the Preliminary data fulfils the following functions
•
System control (see Section 4.3.1.2)
This includes commands for naming and controlling backing files and setting the data area size. These
commands only appear in the Problem section.
•
Solution algorithm definition (see Section 4.3.1.3)
These commands determine the solution method to be used and control its performance (e.g.
convergence) and again can only appear in the Problem section.
•
Model behaviour (see Section 4.3.1.4)
Commands in this category control the type of structural and material behaviour that is to be modelled.
This can vary from group to group.
•
Output control (see Section 4.3.1.5)
This includes not only the control of printed results and diagnostic monitoring, which can vary from
group to group, but also the saving of results on file for subsequent post-processing.
4.3.1.2 System Control
Commands in this category establish values of certain parameters controlling internal data storage and
workspace, and also control the use of backing files.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-13
ASAS (Non-Linear) User Manual
Data Preparation
The data area (freestore) required may be specified using the SYSTEM command. Its value is dependent on the
size of problem; guidelines are given in Section 6
The data-manager parameters are automatically set by the program, but may be re-set using the SYSPAR
command. Normally this will only be necessary for unusual jobs.
External files may be named and controlled by the data given with the PROJECT, STRUCTURE,
NEWSTRUCTURE, FILE, SAVE and, (in restarted jobs) JOB commands. Although the program has defaults
built in, it is recommended that, in all but the simplest of jobs, file names and status should be explicitly given.
Names of the files created by ASAS-NL are defined using FILE commands (except for the old data manager
archive file required in restart jobs, which is given with the JOB command). In addition, depending on the file
type, directives may also be required to define the file status (i.e. whether it is to be a ‘new’ file or whether an
existing one, and in the latter case whether information is to be appended or overwritten). These directives are
given using SAVE and FILE commands.
The ASAS backing file names are controlled by the PROJECT, STRUCTURE and NEWSTRUCTURE
(restarted jobs only) commands. These provide identification of the model for use by ASAS postprocessing
programs. As additional security, a label is attached to all external files. This label can be specified using the
PROJECT command. Subsequent restart jobs making use of the files must then have the same PROJECT
command.
4.3.1.3 Solution Algorithm
The solution procedure is controlled by information using the following commands.
1.
Either STAT using the JOB command, specifying the request for a nonlinear static incremental solution
or TRAN using the JOB command, specifying the request for a transient solution procedure, i.e. including
creep or dynamic effects.
or HEAT using the JOB command, specifying the request for a steady state heat solution procedure.
2.
Either SOLVE or RESTART commands specifying the times (Pseudo or real times) at which a solution is
to be performed. The SOLVE command is used for initial analyses; the RESTART command whenever
an analysis is restarted. SOLVE/RESTART are mandatory for JOB type TRAN involving creep
or SOLUTION or SRESTART commands specifying the number, size and nature of incremental steps at
which a solution is to be performed. SOLUTION is used for initial analysis, SRESTART for restarts.
Note that SOLUTION/SRESTART are not available with JOB type TRAN involving creep.
SOLUTION/SRESTART should be used for structural dynamics problems employing an automatic
timestepping procedure.
Full details about the above methods are given in Appendix -C and Appendix -K.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-14
ASAS (Non-Linear) User Manual
3.
Data Preparation
UPDATE command specifying the frequency of reformation of the global stiffness matrix (UPDA STIF),
the global mass matrix (UPDA MASS) and updating loads and geometry (UPDA GEOM). Using these
commands, a range of Newton-Raphson type iteration techniques are available.
The iteration can be accelerated with Secant Newton or Line Search techniques by using options SECN or
LINS respectively using the OPTION command.
Two methods of stress recovery are available. The default method is the Forward Euler integration
scheme. Sub-incremental procedures for plastic stress redistribution compatible with this scheme can be
requested by specifying the number of sub-increments using the PARAMETER command.
The
alternative is the Backward Euler integration scheme, requested by option BAKE using the OPTIONS
command. Note that the Backward Euler integration scheme is only available with von Mises yield
criterion.
In case of diverging iteration an auto-recovery facility is available by specifying option AUTO using the
OPTION command.
In problems with proportional loading, an analysis may be scaled to first yield using the SCALE
command. The analysis must then be restarted.
4.
CONVERGENCE command. The program will normally iterate until convergence is achieved. The
required convergence criteria are defined using this command. If not given, appropriate default values
are used.
5.
ITERATION command. The maximum number of iterations attempted within a load step is set by
default to 10. The ITERATION command provides a means of modifying this. If convergence is not
achieved within this number then the analysis will terminate unless the option OVIT is given using the
OPTIONS command. In this latter case out of balance residual forces are carried over to the next load
increment and the program continues. Directive NRES with the GROUP or PROBLEM/TITLE
command will set the out of balance forces to zero at the start of a new increment.
6.
EIGN command specifies the times at which an eigenvalue analysis is to be performed. The type of
eigenvalue analysis and the control parameters are defined using the SPIT command.
4.3.1.4 Model Behaviour
The material or structural behaviour is defined for each group as required. Each group is defined using a
GROUP command containing four character directives which, together with the directive using the JOB
command, determines the behaviour of the group. (If no group is explicitly given, then the PROBLEM/TITLE
command serves the same purpose). Thus, for example, static large deflection elasto-plastic shell behaviour is
specified by directives LARG and PLAS using the GROUP command, together with STAT using the JOB
command. (Note that the actual solution is determined also by the commands discussed in Section 4.3.1.3
above.)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-15
ASAS (Non-Linear) User Manual
Data Preparation
Each GROUP command is followed by an ELGROUP command defining the elements within the group. There
is provision to vary the integration rule used in each element using the INTEGRATION command. There is also
provision for elements to be ‘put-to-sleep’ and ‘woken-up’ using the SLEEP and WAKE commands.
4.3.1.5 Output Control
A range of commands are required to control output, depending on the type (e.g. results, data echoes,
diagnostics) and whether it is to be printed or saved on file for subsequent post-processing.
In the absence of any explicit directives, the program will print ‘standard’ output consisting of an echo of the
input data, expanded data lists, problem parameter summaries and the convergence details for each load
increment followed by the tail sheet. NO DISPLACEMENT, VELOCITY, ACCELERATION, STRESS OR
STRAIN RELATED QUANTITIES ARE PRINTED UNLESS ASKED FOR.
The printing of displacements, velocities, accelerations, stresses and strains and associated quantities is
controlled by OUTPUT and BLOCK commands. The stress and strain related output depends on the element
type (see Appendix A). The axis system (local or global) to which it refers can be controlled for some elements
by directives specified using the GROUP command.
The printing of data lists and echoing of input data can be controlled by options using the OPTIONS command.
The Preliminary data can also be interspersed with COMMENT and TEXT commands.
Diagnostic monitoring of the two constituent programs is controlled using PRENL and MONITOR commands.
Archiving of results to file for post-processing or viewing is controlled using the POST or RESU command. No
results will be saved unless POST/RESU Command is specified and hence its usage is highly recommended.
Details of output are given in Section 4.4.
4.3.2
Structural Description Data - see Section 5.2
The Structural Description data defines the shape and physical properties of the idealisation. The following data
blocks are involved:
(a)
Coordinates Data (see Section 5.2.2)
This data defines the positions of the nodes.
Coordinates may be given in rectangular cartesian,
cylindrical polar or spherical polar coordinate systems or in any combination of these. ASAS-NL
transforms all these local coordinates into a global rectangular cartesian system. If a list of coordinates is
requested, they are printed in the global system.
(b)
Element Topology Data (see Section 5.2.3)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-16
ASAS (Non-Linear) User Manual
Data Preparation
This data defines the location of each of the elements by reference to its node numbers. It also defines the
material properties associated with the element by reference to a material property integer.
Most
elements must have their nodes listed in a given sequence. For details, see the element description sheets
in Appendix A.
Each element topology line contains an integer number which refers to the Geometric Property Data
(except for brick and axisymmetric solid elements). Each line also contains a flag which indicates
whether the element mass matrix is to be lumped, consistent or not used at all. If it is left blank in a
natural frequency analysis, the mass matrix for the element will default to the type indicated in Appendix
A.
The user may also assign a unique ‘element number’ to each element. This ‘user element number’
controls the order in which the results are printed and is also referred to by several commands in the
Preliminary data. The numbers are also used to reference elements for post-processing. If numbers are
not given by the user, the program numbers elements automatically in the order in which they first
appear.
(c)
Material Properties Data (see Section 5.2.4)
This data defines the material properties which are referred to by the material property integers in the
Element Topology Data.
For each material sufficient data must be provided to fully define the behaviour and solution required.
All materials require elastic data. If PLAS or CREP appears with the PROBLEM, TITLE or appropriate
GROUP commands in the Preliminary data then data for a plastic (failure) or creep model respectively
are also required.
If the material is temperature dependent, the data for each type of behaviour (i.e. Elastic and Plastic) is
repeated in turn for a set of reference temperatures. The program interpolates linearly for data at
intermediate temperatures.
(d)
Geometric Properties Data (see Section 5.2.5)
This data defines the geometric properties of the element, such as thickness and cross-sectional area.
Solid elements such as the brick family have no geometric properties.
For selected beam elements e.g. BEAM, BM2D, BM3D and TUBE, the properties may optionally be
input using section definitions which provide additional information with regard to shape and physical
dimensions (see Sections 5.2.6).
(e)
Section Data (see Section 5.2.6)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-17
ASAS (Non-Linear) User Manual
Data Preparation
This data is used as an alternative means to define properties for beam element types BM2D, BM3D,
BEAM and TUBE. In order to generate the flexural properties for the structural analysis, the section
shape and dimensions are supplied and the program automatically calculates the required geometric
properties. If required, user defined flexural properties may also be supplied which will override those
calculated from the section dimensions.
The section type and dimensions are stored so that the post-processor, BEAMST, can automatically
calculate extreme fibre stresses without additional information.
(f)
Skew Systems Data (see Section 5.2.7)
This data defines the relationship between the global axis system and any local axis system required at a
node. Each skew system can be defined either in terms of direction cosines or by 3 node points.
4.3.3
Boundary Condition Data - see Section 5.3
The Boundary Condition data defines how the idealisation is restrained or constrained.
(a)
Suppression Data (see Section 5.3.3)
This data lists all the freedoms which are to be suppressed. If a freedom is suppressed in a direction other
than parallel to the global axis, then Skew Systems Data is also required (see Section 3.6.3).
(b)
Prescribed Freedom Data (see Section 5.3.4)
All freedoms which are to be given a prescribed value of displacement, velocity or acceleration are listed
in this data. Freedoms may be prescribed in skew directions by reference to a skew system. The actual
values of displacements, velocities or accelerations to be applied are listed separately, in the Prescribed
Displacement, Velocities and Accelerations Data of Loading Data.
(c)
Constraint Equations Data (see Section 5.3.5)
This data defines any required linear dependence between freedoms. The dependent freedom on the left
hand side of the constraint equation may be skewed by reference to a skew system.
The linear
dependence must be meaningful; it is not valid for example, to have a suppressed freedom on the left side
of a constraint equation.
(d)
Rigid Constraint Data (see Section 5.3.6)
This data block defines rigid connections between freedoms. A selection of rigid ‘elements’ is available
comprising rigid links, 2-D and 3-D rigid beams, rigid link systems and rigid beam systems. Systems are
also available to connect shell elements to brick elements.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-18
ASAS (Non-Linear) User Manual
Data Preparation
The first node specified must be the independent node. The dependent freedoms may be skewed by
reference to a skew system.
(e)
Freedom Release Data (see Section 5.3.2)
This data block defines freedoms which are to be disconnected on specified elements at specified nodes.
A released freedom may be skewed by reference to a skew system. The user element number and node
number is then given to describe each freedom to be released.
The facility is only available for beam elements with release provided in the beam local axis system. This
may be used to model pin joints and sliding connections.
If any of the freedoms specified in this data are referenced in any other Boundary Condition Data then the
Freedom Release Data block must be the first data block specified in the Boundary Condition Data.
4.3.4
Loading Data - see Section 5.4
The Loading data defines the loading history applied to the model.
Load histories may be defined in one of three ways (see Section 3.3.15):
•
Proportional Loading - Section 4.3.4.1
•
Load Functions - Section 4.3.4.2
•
Specific Pseudo Times - Section 4.3.4.3
The three methods of defining load history cannot be mixed. The load history defined with Loading data may be
cycled using the LOCYCLE command in the Preliminary data.
4.3.4.1 Proportional Loading
To specify proportional loading:
•
Define a single load set containing as many load types (e.g. pressure, nodal temperatures) as necessary
•
Leave the Pseudo Time blank on the SET data line
•
A Load Function Data block is not required
•
All nodal temperatures are taken as the reference temperature TREFLD (default 0.0) at zero pseudo
time.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-19
ASAS (Non-Linear) User Manual
Data Preparation
The loads so defined are factored by a multiplier equal to the corresponding pseudo time to give the value at
each load step.
4.3.4.2 Load Functions
To use load functions:
•
For each load function, define a load set containing as many load types as necessary that describe the
load distribution. Each load set references a load function
•
Leave the Pseudo Time blank on the SET data line
•
Define load functions in the Load Function Data
Each load function is a tabulated table of pseudo times and factors giving the proportion of the load to be applied
at that pseudo time. Proportional loading is assumed between tabulated values. Load set without a load function
defined is assumed to have proportional loading.
4.3.4.3 Pseudo Times
To use pseudo times:
•
For each time on the pseudo time axis that the total load distribution is known, define a load set of
(possibly many) load types describing the load state
•
The Pseudo Time for the load set is given on the SET data line
•
A Load Function Data block must not be present
•
All loads not defined within a particular load set are taken as zero at that pseudo time
•
All nodal temperatures are taken as the reference temperature TREFLD (default 0.0) at pseudo time
TIMBEG (default 0.0). All other loads are taken to be zero at pseudo time TIMBEG
•
TREFLD and TIMBEG may be redefined using the PARAMETER command in the Preliminary data
•
All temperatures explicitly defined within a load set at pseudo time TIMBEG are interpreted as a set
of user-supplied reference temperatures unless a solution is attempted at time TIMBEG in which case
the constant reference temperature TREFLD is assumed for all nodes. This facility allows the
reference temperature to be varied throughout the structure.
Proportional loading is assumed between load sets.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-20
ASAS (Non-Linear) User Manual
4.3.5
Data Preparation
Additional Mass Data - see Section 5.5
The Additional Mass data defines the direct mass input values.
This data lists the freedoms and associated lumped mass (inertia) values which are to be added to the finite
element model. With this ADDED MASS facility the mass matrix so described can augment the finite element
mass. Each lumped mass must only be associated with the existing freedoms present on the elements generated
by the element topology data.
Apart from natural frequency or transient dynamics analyses, only x, y, z masses are allowed; all others are
ignored.
The added mass data specified are usually included in all relevant calculations (i.e. load when body loading
applied and mass when inertia required). It is also possible to account for their effects selectively, enabling
greater modelling flexibility.
4.3.6
Initial Conditions Data - see Section 5.6
The Initial Conditions Data defines an initial (residual) stress state. This should be self-equilibrating; if it is not,
the ‘out of balance’ forces will be redistributed within the first load increment, but convergence may be poor.
The Initial Conditions Data also allows for the definition of initial displacements and/or velocities at the start of
a transient dynamic analysis. Care should be taken that any initial conditions so specified are compatible with
any prescribed displacements/velocities/accelerations.
4.4
Description of Output
The output file from ASAS-NL contains listings of checked and unchecked data and cross-reference tables
describing the model as well as results of the non-linear analysis. In addition, two journal files may be produced
from each run.
4.4.1
Data Input Echo and Checking
The following are produced during data input and checking stages:
PRELIMINARY DATA ECHO
A complete listing of the Preliminary data as supplied by the user is given.
PROGRAM CONTROL PARAMETERS
A complete listing of Program Control Parameters is given.
These, in general, are controlled using the
PARAMETER command in the Preliminary data, but default values are supplied automatically by the program.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-21
ASAS (Non-Linear) User Manual
Data Preparation
Typical program parameters are the reference temperature for temperature loads and whether a sub-incremental
analysis has been requested.
INPUT DATA ECHO
A complete echo of the rest of the input data as supplied by the user is given.
CHECKED DATA
A listing of all data describing the model after being checked is given. Error and Warning messages, as
appropriate, are printed. This section contains expanded lists of coordinates, material properties, geometric
properties, suppressions, constraints and load tables for each load set. This is followed by listings of checked
residual stresses and results from further temperature checking if appropriate. Cross-reference tables giving
group structure, integration rules and nodes are also given.
4.4.2
Analysis Results
The amount of output produced depends on the results requested by the user in the Preliminary data. The order
of the load increments is dictated by the order of the solution times as given using the SOLVE command.
Output for each increment will be as follows:
STIFFNESS REFORMATION
A message is given if the stiffness matrices of elements in any group are reformed in any iteration during any
incremental step.
GEOMETRY REFORMATION
A message is given if the geometry is reformed in any iteration during any incremental step.
MASS REFORMATION
A message is given if the mass is reformed at any incremental step.
CONVERGENCE MONITORING
The incremental and total values of the convergence criterion are given for each iteration. This allows the rate of
convergence to be monitored.
ARCHIVING
Checkpoint numbers on the data-manager archive file and element stiffness matrix file are given if the user
specifically requests an archive at this load step using the SAVE command. The checkpoint number for the
Data-Manager archive file is required in the Preliminary data when a restart is being attempted. An archive is
always made following the final load increment if a SAVE command is present and the checkpoint number is
then found on the Data-Manager Tail Sheet.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-22
ASAS (Non-Linear) User Manual
Data Preparation
In addition, messages about information saved on the file for post-processing and plotting by ancillary program
are also given.
OUTPUT
Displacements and Reactions, if requested, are given first. By default maximum values of displacements and
summed reactions are printed for all increments for a linear or nonlinear static analysis. For a transient dynamics
analysis, maximum values of velocities and accelerations are additionally output. If requested the program also
prints values of displacements (velocities, accelerations) and reactions at all or selected nodes for all selected
increments.
Reactions include forces arising from application of prescribed displacements and constraint
equations.
Other than displacements (velocities, accelerations) and reactions, the output depends on the type of analysis and
the elements used. In the most general case, current stress, current total strain, elastic, inelastic and creep strain,
current yield stress and yield strain, equivalent stress, equivalent strain, equivalent plastic strain and work may
be requested for any element and any load increment. For shell and beam elements stress resultants at the
centroidal surface sample points are available. If no directives are given then no stress and strains will be
printed.
All stress and strain related quantities are computed and output at element integration points (see Appendix -G)
referred to either global or element local axes. The choice of axis systems can be varied, if required, from group
to group, but cannot be changed during the analysis.
In addition to stress and strain quantities, the material ‘status’ of an integration point is also printed under the
column INDR/STATUS according to the following convention:
All relevant elements except gaps and rigid surfaces
E
-
0
-
elastic
U
-
1
-
elastic unloading (or reloading) following yield
P
-
2
-
yielded and loading
C
-
3
-
Cracking
F
-
4
-
fibre failure for composite analysis
M
-
5
-
matrix failure for composite analysis
L
-
6
-
lamina failure for composite analysis
S
-
7
-
transverse shear/normal stress failure for composite analysis
MS
-
8
-
M and S modes failure for composite analysis
Rigid surface or gap elements
1
-
no contact
2
-
stick
3
-
slide in Y direction
4
-
slide in Z direction
5
-
slide in both Y and Z directions
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-23
ASAS (Non-Linear) User Manual
Data Preparation
Maximum values of displacements and largest equivalent stress, equivalent total strain, equivalent plastic strain
and equivalent creep strain, where appropriate, are also given.
4.4.3
Analysis Summary
The following information is given at the end of a run:
DATA MANAGER TAIL SHEET
A complete listing of system control parameters is given. These, in general, are controlled using the SYSTEM
and SYSPAR commands in the Preliminary data. The information may be used to monitor the efficiency of the
analysis. This information is intended only for the experienced user. The checkpoint number of the datamanager file for a default archive on the last load increment is also given.
FILE STATUS
The status and disposition of all backing files accessed and created is given. The status is NEW for a virgin file
or OLD for an existing one. The disposition is OPEN, CLSE (closed) or DEL (deleted). DEL files have been
successfully deleted and CLSE files closed and saved.
MAIN RUN PARAMETERS
Listings of the main program parameters such as number of nodes and elements in the model are given.
Solution characteristics such as number of accumulated iterations and maximum frontwidth are also given.
4.4.4
Journal Files
Two journal files are printed during an ASAS-NL run. The first file, called pnamJF (pnam is the project name),
contains a summary of the run information of all the runs in the project. The second file, called INCRJF,
contains condensed information about the main analysis, enabling the user to monitor interactively the
incremental iterative solution process. File INCRJF is normally deleted at the end of the analysis but it may be
saved using option SAVJ.
4.4.5
ASASNL Output Markers
Certain values which are helpful for either the assessment or control of the analysis are periodically output by
ASASNL. To help find them using text editors, they are marked by a character string **nnnnnnnn, in columns 1
to 10, where nnnnnnnn is an indicative keyword.
Keyword
Description
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-24
ASAS (Non-Linear) User Manual
Data Preparation
ACCL
Summary information about acceleration technique used
ADJUST
Adjusted value of next step size
AUCR
Automatic creep timestepping. Summary information for automatically selected solution
times
AUGMENT
Augmentation of Lagrangian multipliers required
CHANGE
Gives number of sampling points (INDR) to have changed state for increment
CONV
Convergence performance parameters
CURRENT
Current value of step size
DETK
Stiffness determinant and number of negative stiffness and constraint pivots
DISP
Start of displacement output
DMTAIL
Data Manager tail sheet
DPCOM
Constant Increment of Displacement Component - iteration performance parameters
DPVEC
Constant Increment of Displacement Vector - iteration performance parameters
DPVECL
Constant Increment of Displacement Vector, Linearised version - iteration performance
parameters
DUMP
Solution state saved for possible future restart or post-processing
EIGN
Start of eigenvalue output
ELEM
Start of element based output
ERROR
Error flag
EXWRK
Constant Increment of External Work Measure - iteration performance parameters
EXWRKL
Constant Increment of External Work Measure, Linearised version - iteration performance
parameters
FREQ
No natural frequency analysis performed due to non +ve definite stiffness matrix
FILES
Active files summary
FINISH
Abnormal exit path following error
GEOM
Geometry reformed
INCRnnnn
Start of increment nnnn and pseudo time (Always 1.0 for SOLU)
LEVEL
Load/displacement level exceeds preset value, job terminating
LINS
Line Search performance information
MASS
Mass reformed
MAXP
Gives highest PLASTIC strain and position for increment
MAXS
Gives highest STRESS and position for increment
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 4-25
ASAS (Non-Linear) User Manual
MAXT
Gives highest TOTAL strain and position for increment
PERT
Perturbation introduced
POST
Post-processing identifier saved to porthole file
SECN
Secant-Newton performance information
STIFF
Stiffness reformed
SUMM
Summary information for this increment
TRACE
Start of subroutine trace back
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Data Preparation
Page 4-26
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Data Preparation
Page 4-27
ASAS (Non-Linear) User Manual
5.
Data Formats
Data Formats
ASAS-NL data is organised into a series of data blocks, each containing a particular type of data. This chapter
describes each data block individually. The layout of each block is explained, and some examples are given.
The user need only refer to the sections describing the data blocks required for his current analysis.
Each block, except the Preliminary data, begins with a block header line. This header line defines the type of
data which follows. The final line in each block must be an END, written on a line on its own. The final line in
the data file must be a STOP, written on a line on its own.
The data blocks described in this chapter are:
Preliminary Data ..... ................ ................ ................ Section 5.1
Structural Data ........ ................ ................ ................ Section 5.2
Boundary Condition Data ......... ................ ................ Section 5.3
Loading Data .......... ................ ................ ................ Section 5.4
Additional Mass Data .............. ................ ................ Section 5.5
Initial Conditions Data ............. ................ ................ Section 5.6
STOP Data .............. ................ ................ ................ Section 5.7
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-1
ASAS (Non-Linear) User Manual
5.1
Preliminary Data
The Preliminary Data
The preliminary data is the first block of ASAS-NL data. It defines the:
•
memory size to be used for data handling
•
job type (eg whether statics or dynamics)
•
identity of the project
•
structure or component to be processed within that project
•
options which will affect the course of the run
•
amount of printing produced
•
files saved for further processing
All commands are identified by a unique command word at the start of the line. The first 4 characters of each
command word are mandatory, others are optional. Free format is used, with ‘topological variables’ (see Section
4.2.3) used as an optional shorthand method for generating lists of required numbers.
The majority of commands are optional and can be placed in any order. However, the following are mandatory
and must be supplied in the order given.
JOB
PROBLEM or TITLE
One of SOLVE or RESTART, SOLUTION, SRESTART or SCALE
END
Table 5.1 lists all possible commands in the preliminary data section. Mandatory commands are shown in bold.
An asterisk against optional commands signifies that defaults are implied, details of which are given below:
SYSTEM
PROJ
STRUCTURE
NEWSTRUCTURE
SYSP
CONV
FILE
INTE
ITER
PARA
PINO
SAVE
SPIT
UPDA
WEIG
Data area 1000000
Default project title is ‘ASAS-NL ARCHIVE FILE’ and project name is ASNL
Default name is ASNL
Default name is ASNN
The various default values are given in Section 6, Table 6.1.
Residual convergence with Euclidean norm and tolerance 0.001.
The various default file names are given in Section 6, Table 6.1.
Use default integration rules.
Limit of 10 iterations for each load increment.
Various default values. See the PARAMETER command for details.
The default pressure interpolation order is that implied by the particular element
displacement variation.
Archive data manager and global stiffness matrix for last increment only.
Various default values. See the SPIT command for details.
Reform stiffness matrix on first iteration of first increment only.
The default values are unity for all freedom types.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-2
ASAS (Non-Linear) User Manual
Preliminary Data
The preliminary data commands fall into two sections, referred to as the problem and group sections. The
problem section includes all the commands following the PROBLEM command up to the first occurrence of the
GROUP command. All subsequent commands fall into the group section. The group section allows elements
to be assigned to a particular group. The division of the finite element model into groups of elements is strongly
recommended as many of the post-processing options in POSTNL are group related. Some elements, such as the
bar element FLA2, have to be assigned to a separate group (or groups) if the model includes other element types.
Table 5.1 indicates which section each command should appear in. The preliminary data commands invoke
procedures (eg frontwidth optimisation) and sets parameters (eg the subspace iteration convergence tolerance)
which are global in nature. Commands allowed within the group section control procedures and parameters that
may be assigned to groups of elements, eg output of stresses and strains.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-3
Preliminary Data
ASAS (Non-Linear) User Manual
Name
SYSTEM
PROJECT
STRUCTURE
NEWSTRUCTURE
SYSPAR
Description
*
*
*
*
*
Section
Sets size of data area
Sets project name and title
Sets structure name
Sets new structure name
Sets system parameters
Category
O
O
O
O
O
JOB
PROBLEM
TITLE
Titles output
P
P
SOLVE
RESTART
SOLUTION
SRESTART
SCALE
Solution times
Restart times
Special solution control
Special solution restart
Controls scaling of loads
P
P
P
P
P
O
Comments in data
Sets convergence criteria
Replaces ELGROUP for coupled
analysis
Eigenvalue solution
Backing file names
Group Titles
Elements in group
Skip elements in group
PG
PG
G
O
O
O
P
P
G
G
G
M
O
O
O
O
Hydrodynamic database name
P
O
Integration rules
Iteration limits
Controls cyclic loading
Diagnostic monitoring in ASASNL
Controlling options
Controls output
Controls output
P
P
P
P
P
PG
PG
O
O
O
O
O
O
O
Sets problem parameters
Invokes frontwidth optimiser
Sets starting vectors
Defines pressure interpolation order
Post-processing requirements
P
P
P
P
P
O
O
O
O
O
Archive times
Set eigenvalue soln. parameters
Controls temporal integration for
transient analysis
Printed comments in output
P
P
O
O
P
P
O
O
Defines global analysis units
Controls solution procedure
Weighting factors for convergence
Sets wake up time for elements
Sets sleep time for elements
Signifies end of Preliminary Data
P
PG
P
P
P
O
O
O
O
O
M
COMMENT
CONVERGENCE
EGEN
EIGN
FILE
GROUP
ELGROUP
SKIP
*
*
HYDR
INTEGRATION
ITERATION
LOCYCLE
MONITOR
OPTION
OUTPUT
BLOCK
*
*
PARAMETER
PASS
START
PINO
POST
RESU
SAVE
SPIT
TEMPORAL
*
*
*
*
TEXT
UNITS
UPDATE
WEIGHTS
WAKE
SLEEP
END
*
*
M
M
M
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Comments
Must be the
first section
One only,
must follow JOB
One only,
must follow
PROB or TITL
for eigenvalues
recommended
must follow GROUP
only use with
ELGROUP
mandatory for
accessing hydrodynamic
data
must follow OUTput
must have PASS
recommended,
one only
recommended
last command
Page 5-4
Preliminary Data
ASAS (Non-Linear) User Manual
Note
P PG O -
Problem Section
Problem and Group Section
Optional
G M * -
Group Section
Mandatory
Default available
Table 5.1 Preliminary Data Commands
5.1.1
AQWA Command
This command defines the name of the AQWA hydrodynamic database files. The command (or HYDR) is
mandatory if linkage to the hydrodynamic database is required, e.g. import of AQWA RAOs via the load
function type RAOS.
AQWA
aqwaid
(istr)
Parameters
AQWA
: Command keyword
aqwaid
: name of the AQWA model to be processed. This is the name associated with the .RES file
generated by AQWA-LINE. (Alphanumeric, up to 32 characters)
istr
: identification number of the structure in the hydrodynamic model. If omitted defaults to 1.
(Integer)
Notes
1.
If the file name contains space, the specified name must be embedded in double quotes (“).
5.1.2
BLOCK Command
This command defines the type of output to be printed under control of the OUTPUT command(s). Optional
BLOCK
blocno
ident
(ndelno)
Parameters
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-5
Preliminary Data
ASAS (Non-Linear) User Manual
BLOCK
: command keyword
blocno
: identifying number of block
ident
: output identifier, one or more of the following:
DISP
displacements (problem section)
STRS
stresses
STRN
INST
total strains
inelastic strains
ELAS
SRES
elastic strains
stress resultants (beam and shell elements only)
CRSN
creep strains
ESTR
SSTR
end segment smoothed stresses
all segments smoothed stresses
for WST4 and SST4 elements
SSRE
smoothed stress resultants
ORIG origin of yield locus (for kinematic hardening)
ndelno
: user defined list of nodes (for displacement only) or element numbers (for stresses or strains)
given in topological format. If blank defaults to all nodes or elements (in group)
Notes
1.
2.
3.
5.1.3
If GROUPS are used, then all commands controlling output (i.e. OUTPUT, BLOCK) must
appear in the GROUP section other than commands controlling displacement output which
always appear in the PROBLEM section.
BLOCK commands should immediately follow the parent OUTPUT command(s).
For a transient analysis including inertia effects, if DISP is specified, then velocities and
accelerations are also output.
COMMENT Command
Any number of these commands may be used anywhere in the Preliminary data. They are not included in the
descriptive text block. Optional
COMMENT
alpha
Parameters
COMMENT
: command keyword
alpha
: any alphanumeric comment
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-6
Preliminary Data
ASAS (Non-Linear) User Manual
Note
COMMENT commands may only be used in the preliminary data. For comment lines in the main body of the
data, use an asterisk at the start of the comment.
5.1.4
CONVERGENCE Command
This command defines the convergence criteria. Optional
CONVERGE
nmtype
refvar
tol
Parameters
CONVERGE : command keyword
nmtype
refvar
: type of norm, one of the following:
ABSN
absolute norm
EUCN
euclidean norm (Default)
MAXN
maximum value
SCAL
scaled using diagonal stiffness terms
: reference variable, one of the following:
DISP
tol
displacement Increments
RESF
residual forces (Default)
STRN
STRS
strain
stress
: tolerance value for convergence, default is 0.001. (Real)
Notes
1.
For creep analysis, a reference variable may be chosen by the program according to the form of the
solution. For details, see Appendix -J.
2.
STRN and STRS Convergence Criteria are not available for shells using Ivanov yield criterion or
engineering beams, ie BM2D, BM3D and TUBE.
Examples
The default convergence criterion
CONV
EUCN
RESF
0.001
Convergence criterion based on displacements
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-7
Preliminary Data
ASAS (Non-Linear) User Manual
CONV
5.1.5
EUCN
DISP
1.0
EGEN Command
This command defines the elements to be generated in a group and must follow immediately its parent GROUP
command. The command is only used in coupled analysis in place of ELGROUP command for the automatic
generation of field elements.
EGEN
grpno
elincr
Parameters
EGEN
: compulsory keyword
grpno
: group number from which the elements are generated
elincr
: user element number increment with respect to corresponding element in group grpno
Notes
1.
The topology of elements specified in EGEN will be generated automatically by the program, and should
2.
not be given explicitly in the ELEM data.
Automatically generated field elements will have material property integer (1000+IMAT) and geometric
property integer (1000+IGEOM) assigned. IMAT and IGEOM are the material property integer and
geometric property integer respectively of the parent displacement element.
5.1.6
EIGN Command
This command invokes an eigenvalue analysis. Compulsory for eigenvalue analysis.
ALL
EIGN
ptinc1
SELP
(ptinc2)
Parameters
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-8
Preliminary Data
ASAS (Non-Linear) User Manual
EIGN
: command keyword
ptinc1
: list of pseudo times (Real) or increments (Integer) at which an eigen solution is to be
attempted.
These must occur with the preceding SOLVE, SOLUTION, RESTART,
SRESTART or SCALE commands
SELP
: keyword (optional but required for perturbation analysis)
ptinc2
: selected pseudo time (Real) or increment (Integer) for inclusion of perturbation load vector
(default is the first pseudo time or increment on the list)
Notes
1.
The type of eigenvalue analysis is determined by the matrix specified with the SPIT command, together
with other control information.
2.
The pseudo times must be in ascending order.
3.
Pseudo times are required for SOLVE problems: increment numbers are required for special solution
problems, e.g. ARCL.
4.
To achieve results similar to a frequency analysis with ASAS (Linear), use EIGN 0.0 in a static job
solving at time 0.0 (assuming that at time 0.0 the loading is zero). Note that if a frequency analysis is
performed with loading, then natural frequencies may change due to load stiffening and other non-linear
effects.
5.1.7
ELGROUP Command - (Group Section Only)
This command defines the elements in a group and must follow immediately its parent GROUP command. It is
valid only in conjunction with a GROUP command. If no group is defined, then all elements are assumed to be
in group 1. Conversely, if groups are used, then every element must be explicitly assigned to one or other group.
Optional
ELGROUP
elno
Parameters
ELGROUP
: command keyword
elno
: list of element numbers given in topological format. (Integer)
Note
1.
Gaps and FLA2 elements must always belong to their own group and must not be mixed with other
element types.
2.
The SKIP command can be used to switch off some elements defined in the ELGROUP command. The
order of ELGROUP and SKIP commands within a group is not important.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-9
Preliminary Data
ASAS (Non-Linear) User Manual
Examples
Assign elements 1 to 10 to group 3
GROU
3
*
BEAM
ELEMENTS
ELGR
1
2
3
5
4
6
7
8
9
10
Alternative method using topological format
ELGR
5.1.8
(10)
(1,1)
END Command
This must be the last command in the preliminary data. Compulsory
END
Parameter
END
5.1.9
: command keyword
FILE Command
Defines names and attributes of files. Recommended
FILE
ftype
NEW
(APPEND)
OLD
OVER
fname
Parameters
FILE
: command keyword
ftype
: keyword to identify file type, one of the following:
ARCH
new archive file
NSTF
new stiffness file
OSTF
POST
old stiffness file
post-processor file
MODL
‘PATRAN’ or ‘FEMVIEW’ formatted model file
NEW should be given on SAVE command
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-10
Preliminary Data
ASAS (Non-Linear) User Manual
fname
: filename of up to 12 characters (including extension)
NEW
: keyword to denote file is new
OLD
: keyword to denote file already exists
APPEND
: keyword required to append new information to end of file (default)
OVER
: keyword required if new information is to overwrite existing information
Notes
1.
The old archive file, if required, is defined with the JOB command.
2.
3.
The default values for existing files is given in Section 6
Keywords APPEND and OVER are applicable to file types POST and MODL only. Leave blank for
4.
ARCH, NSTF and OSTF.
If the old stiffness file is omitted in a restart, the required filename will be retrieved from information
stored in the old archive file.
Example
Naming the porthole file for post-processing with POSTNL
FILE
5.1.10
POST
CRANEPST
GROUP Command - (Group Section Only)
A Group is a subset of elements in the structural model, all of which have the same non-linear behaviour. This
behaviour can vary between Groups. The Group command defines the behaviour by means of directives. In
some cases it is possible to define the same directives at Group and Problem level, in which case the lower level
Group definition applies. Optional
The Group command must be followed immediately by the ELGR command.
GROUP
grpno
(direct)
(*
title)
Parameters
GROUP
: command keyword
grpno
: identifying number of the group. (Integer, 1-9999)
direct
: 4 character directives defining structural and material model. May be one or more of the
following:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-11
Preliminary Data
ASAS (Non-Linear) User Manual
PLAS
take plasticity effects into account
LARG
include large displacement effects in the calculation of strains and geometric
stiffness matrices.
This directive should be accompanied by the command
UPDATE GEOM (see UPDATE command)
CONL
use conservative pressure loading - i.e. calculate pressure loads using original
geometry throughout.
Only applicable with UPDATE GEOM (see UPDATE
command)
NRES
do not carry forward residuals into next increment
FLNS
form natural stiffness (i.e. Young’s modulus*Area) for FLA2 and FAT2 elements
CREP
creep analysis
NREC
(only use with the GROUP command). The stresses will not be recovered nor
element stiffnesses be reformed for elements in the group
EXPL
*
user explicit temporal integration scheme for transient analysis
: character to indicate the following text (up to and including column 80) forms a title for this
group
title
: any alphanumeric group title. It must be preceded by an asterisk (*). The title is used in the
output from ASASNL to describe the group
Notes
1.
If no directives are given, linear elastic behaviour is assumed with the default implicit temporal
2.
integration scheme for transient analysis.
Gaps and FLA2/FAT2 elements must always belong to their own group and must not be mixed with other
element types. In general, it is strongly recommended that each group defined comprises only one
element type to facilitate post-processing of the analysis results.
5.1.11
HYDR Command
This command defines the name and details of the file containing the hydrodynamic information. The command
is mandatory if linkage to the hydrodynamic data is required, e.g. import of RAOs via the load function type
RAOS.
HYDR
AQWA
aqwaid
(istr)
NRAO
filename
(wfform)
(wdform)
(raoform)
(rotform)
Parameters
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-12
Preliminary Data
ASAS (Non-Linear) User Manual
HYDR
AQWA
aqwaid
istr
NRAO
filename
wfform
wdform
raoform
rotform
command keyword
keyword to signify that hydrodynamic data is obtained from AQWA
name of the AQWA model to be processed. This is the name associated with the .RES file
generated by AQWA-LINE. (Alphanumeric, up to 32 characters)
identification number of the structure in the hydrodynamic model. If omitted defaults to 1.
(Integer)
keyword to signify that hydrodynamic data is obtained from a neutral RAO data file
name of the neutral RAO file. (Alphanumeric, up to 32 characters)
format of wave frequency data, one of the following:
FREQ
frequency in rad/s (Default)
PERD
period in s
HRTZ
frequency in Hz
format of wave direction data, one of the following:
XPOS
positive X direction is 0° (Default)
XNEG
negative X direction is 0°
format of RAO data, one of the following:
AP
amplitude and phase angles (Default)
RI
real and imaginary parts
format of rotational units in RAO data, one of the following:
DEG
degrees (Default)
RAD
radians
Notes
1.
The format of the neutral file is described as follows:
Frequency/Period value
Direction value
X (surge)
X (surge)
RX (roll)
RX (roll)
Y (sway)
RY (pitch)
Y (sway)
RY (pitch)
Z (heave)
RZ (yaw)
Z (heave)
RZ (yaw)
The 6 numbers representing the RAO are in pairs of Amplitude and Phase or Real and Imaginary.
The data lines are repeated for each wave frequency and direction.
2.
Maximum number of wave frequencies allowed is 50. Maximum number of wave directions allowed is 40.
3.
Wave directions are assumed to be in degrees and in the range -100 to +180.
4.
The rotational units specified apply to all phase and rotational RAO values.
5.
If the file name contains space, the specified name must be embedded in double quotes (“).
6.
A positive phase angle is considered as lagging.
Example
Example of a neutral RAO data file with data supplied at 2 frequencies 0.34907 rad/s and 0.36960 rad/s and 5
directions 0°, 45°, 90°, 135°, and 180°.
0.34907
0.00
0.6997
0.0000
88.98
0.31
0.0000
0.1507
-104.31
88.35
2.0823
0.0000
13.11
46.90
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-13
Preliminary Data
ASAS (Non-Linear) User Manual
0.34907
45.00
0.5048
0.0874
0.34907
90.00
0.0000
0.1382
0.34907
135.00
0.5048
0.0874
0.34907
180.00
0.6997
0.0000
0.36960
0.00
0.6585
0.0000
0.36960
45.00
0.4780
0.0630
0.36960
90.00
0.0000
0.1047
0.36960
135.00
0.4780
0.0630
0.36960
180.00
0.6585
0.0000
5.1.12
89.01
-91.84
0.5046
0.0954
89.02
88.15
2.0826
0.0000
13.09
-134.89
123.22
-91.64
0.6994
0.0000
88.98
23.57
2.0823
0.0000
13.11
-94.99
-90.99
-91.84
0.5046
0.0954
89.02
-91.85
2.0826
0.0000
13.09
-47.76
-91.02
162.66
0.0000
0.1507
87.73
-91.65
2.0823
0.0000
13.11
146.91
88.53
-159.88
0.0000
0.1134
-177.96
87.68
3.0661
0.0000
36.08
-152.22
88.59
-92.74
0.4779
0.0682
88.60
87.26
3.0668
0.0000
36.06
-62.60
104.89
-92.32
0.6583
0.0000
88.53
19.68
3.0661
0.0000
36.08
-42.51
-91.41
-92.74
0.4779
0.0682
88.60
-92.74
3.0668
0.0000
36.06
-120.04
-91.47
-35.18
0.0000
0.1134
91.21
-92.32
3.0661
0.0000
36.08
-24.82
INTEGRATION Rule Command
This command defines the integration rules to be used by specified elements. If not present the default rule is
used. Optional
INTEGRATION
intx
inty
intz
(elno)
Parameters
INTEGRATION : command keyword
intx
: integration order or rule number in element local directions. All three numbers must be
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-14
Preliminary Data
ASAS (Non-Linear) User Manual
inty
intz
given. (Integer)
elno
: list of element numbers in topological format. (Integer)
If blank, defaults to all elements (in group)
Notes
1.
See Appendix -G for default integration rules for each element type.
2.
3.
intz should be 1 for 2-D elements.
If zero is specified for any rule number then that rule number is set at the default value.
4.
If an invalid integration rule is specified for an element then that element’s default values will be used.
5.
If more than one set of integration rules is specified for any given element then the final set will be used.
Examples
Allow for five layers through the thickness for QUS4 shell element numbers 1 to 25 in a plasticity analysis.
INTE
1
1
5
(25)
(1,1)
Similar example but for TCS8 shell elements
INTE
5.1.13
2
2
5
(25)
(1,1)
ITERATION Command
This command specifies the maximum number of iterations to be performed within a load increment. Optional
ptminc
ITERATION
n
TO
END
Parameters
ITERATION : command keyword
n
: maximum number of iterations in every increment up to and including the solution time/
increment ptminc, if specified. (Integer)
TO
: keyword
ptminc
: solution pseudo-time/time (Real) or increment (Integer) up to which this specification of n is to
apply
END
: keyword indicating that n applies for all solutions times/increments to the end of the analysis
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-15
Preliminary Data
ASAS (Non-Linear) User Manual
Notes
1.
If no ITERATION command is present a maximum of 10 iterations are assumed for each increment.
2.
The run will terminate if convergence is not achieved within the specified number of iterations, unless
3.
option OVIT (OVerride ITeration limit) is specified in the OPTION command.
If a solution is performed at a pseudo-time/time/increment greater than the last pseudotime/time/increment specified with an ITERATION command, then the maximum number of iterations
performed will be that specified on the last ITERATION command. To revert to the default, specify
ITERATION 10 TO END as the last ITERATION command.
Example
Allow up to 20 iterations to time 5.0, 15 iterations from time 5.0 to 7.0 and revert to default for all remaining
times
ITER
20
TO
5.0
ITER
15
TO
7.0
ITER
10
TO
END
5.1.14
JOB Command
Defines analysis type and for restart jobs the old archive file name and required checkpoint number on the old
archive file. Compulsory
(NEW)
JOB
STAT
(OLD)
TRAN
(REPL)
PIER
oldarch
(nchkpt)
HEAT
HTRA
Parameters
JOB
: command keyword
NEW
: optional keyword indicating that this run will create a new project data base
OLD
: optional keyword indicating that this run will add to an existing project data base
REPL
: optional keyword indicating that this run will replace a previous run of the same structure on
the project database
STAT
: keyword indicating static analysis
TRAN
: keyword indicating a transient analysis, ie including creep or inertia effects
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-16
ASAS (Non-Linear) User Manual
Preliminary Data
PIER
: keyword indicating a piezo-restivity analysis
HEAT
: keyword indicating a steady state heat analysis
HTRA
: keyword indicating a transient heat analysis
oldarch
: old archive file name up to 8 characters. This is only required for restarts
(nchkpt)
: number of the required restart checkpoint on the old archive file (brackets must appear). If
omitted the highest checkpoint on the old archive file is taken. This is only required for
restarts. (Integer)
Notes
The default project status is OLD for a restart job and NEW otherwise
1.
5.1.15
LOCYCLE Load Cycle Command
This command defines cyclic loading. Optional
LOCYCLE
ptime1
ptime2
Parameters
LOCYCLE
: command keyword
ptime1
: pseudo time for start of cycle - T1. (Real)
ptime2
: pseudo time at finish of cycle - T2. (Real)
Notes
1.
The starting and finishing times, T1 and T2 respectively, refer to the first cycle. Cyclic loading, period T2
minus T1, follows.
2.
T1 need not necessarily be the first time specified with the SOLVE command but T1 minus T0 must be
less than T2 minus T1.
3.
The load cycle times and the parameters TREFLD and TIMBEG cannot be redefined in a restart. This
means that if the loads are redefined on restart they must lie within the load cycle range of the initial run.
5.1.16
MONITOR Command
This command controls diagnostic monitoring in ASASNL. Optional and not normally required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-17
Preliminary Data
ASAS (Non-Linear) User Manual
(i)
For the main analysis stage.
MONITOR
stage
subkey
Parameters
MONITOR
: command keyword
stage
: stage identifier, one of the following:
subkey
INIT
initialisation stage
LOAD
STIF
load generation
stiffness
REDU
reduction
SOLV
UPDT
solve
update
STRE
UPD1
stress recovery
update 1
UPD2
update 2
SCAL
MASS
scaling to first yield
mass generation
EIGN
SPIT
eigenvalue extraction
eigenvalue extraction
OUTP
PORT
output
post-processing output file
AUTM
automatic timestepping
AUGM
ALL
augmented Lagrangian
monitoring on all stages
: names of subroutines and/or keywords to be monitored. Keywords (set throughout the stage)
may be one or more of the following:
ALL
monitor all subroutines in stage
STOPnn
abort program run at start of this stage in increment nn, where nn is zero filled
and right justified
CLAIM
monitor dynamic storage allocator
TOTAL
print contents of freestore area on CLEAR
COMMON print common block contents at start of stage
EXTEND
set extended logging mode for subroutine tracing package
BRIEF
set compact logging mode for subroutine tracing package
DTAILS
print length and type of each record in Data Manager tail section
DTAILL
print length, type and contents of each record in Data Manager tail section
VPUTS
print length and type of each VPUTI or VPUTR
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-18
Preliminary Data
ASAS (Non-Linear) User Manual
VPUTL
print length, type and contents of each VPUTI or VPUTR
VGETS
print length and type of each VGETI or VGETLR
VGETL
print length, type and contents of each VGETI or VGETR
MODMAN monitor data manager page file in Data Manager tail section
PCHAIN
call subroutine PCHAIN in stage header
PUSAGE
monitor page usage in the stage
PUFULL
as for PUSAGE but with more information
OVROFF
switch off overflow check
DISKFL
monitor status of disc files
ROTAWS includes rotations in the initial configuration in the stress recovery stage when an
element wakes up so that they will not cause straining (rotations not included by
default) usage MONI STRE ROTAWS
TEMPWS assumes that there is no sudden change of temperature when an element wakes up
in the load generation stage (by default newly activated elements are set to the
reference temperature)
usage MONI LOAD TEMPWS
Note
Several MONITOR commands can be used to monitor different stages with different subkey values if required.
(ii)
For all other stages:
FULL
ALL
READ
MONITOR
WRITE
BRIEF
file
INDEX
FREESTORE
SYOP
option
v alue
FLAG
SENTRY
Parameters
MONITOR
: keyword
FULL
: print the contents of the file transfers on reading and writing
READ
: print the contents of the file transfers on reading only. Print the header only (not contents)
on writing
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-19
Preliminary Data
ASAS (Non-Linear) User Manual
WRITE
: print the contents of the file transfers on writing only. Print the header only (not contents)
on reading
BRIEF
: print the headers for the file transfers but not the contents on reading and writing
ALL
: monitor all ASAS logical files
file
: list of ASAS logical file numbers to be monitors
INDEX
: monitor the ASAS Project Index file
FREESTORE
: monitor the allocation of space in the Data Area
SYOP
: the ASAS program has a number of system monitoring options which can be switched on
FLAG
using this command
option
: the number of the system option
value
: the value assigned to the system option
SENTRY
: monitor the entry into each Fortran subroutine
Notes
1.
Specific information relating to these monitoring features can be found in the ASAS Programmer’s
Manual.
2.
3.
Many of these features produce large amount of formatted output.
Several MONITOR commands can be used in the same run.
Example
MONITOR BRIEF 13 15 3
MONITOR FREESTORE
5.1.17
NEWSTRUCTURE Command
To define the new structure name to be associated with the results created by a restarted run. Required by
restarted jobs only but highly recommended.
NEWSTRUCTURE
nsname
Parameters
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-20
ASAS (Non-Linear) User Manual
NEWSTRUCTURE
nsname
:
Preliminary Data
keyword
: structure name to be associated with the results being created by the current restarted run in
order to identify these results from others in the project. nsname must be unique for this
project (alphanumeric, 4 characters).
Notes
1.
If the NEWSTRUCTURE command is omitted then nsname defaults to the name ASNN. However,
since the structure name must be unique within a project, the default must not be assumed more than once
2.
if the project contains a series of restarts.
A STRUCTURE command is normally required in conjunction with NEWSTRUCTURE to define the
name of the existing structure
5.1.18
OPTION Command
This command defines options applicable to the problem. Optional
OPTION
option
Parameters
OPTION
: command keyword
option
: 4-character keyword to identify option. May be one or more of the following:
APIW
complete wave load to the requirements of API RP2A (See Appendix M.7)
APIC
vary current profile using non-linear stretching as recommended in the API RP2A
Code of Practice. Default when APIW is selected (See Appendix M.7)
AUCR
automatic timestepping for creep (see Appendix -J)
AUTO
automatic restart of increment with reduced size (see MXAUTO and STEPRF
with PARAMETER command) when solution is not available, divergence or
slow convergence. Used only with SOLUTION command. Not applicable for
creep
BAKE
backward Euler method for plasticity (see Appendix C.3)
BODY
check for sensible density values
BRIG
rigorous buoyancy load calculation (See Appendix M.7)
CCOG
calculate centre of gravity of the model
CCON
print the constraint equations input data
CCOO
print the coordinate input data
CDIR
print the direct mass input data
CDIS
print the displaced freedoms input data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-21
ASAS (Non-Linear) User Manual
Preliminary Data
CELE
print the element topology input data
CGEO
print the geometric property input data
CLOA
print the load input data
CLST
solve constraint equations last. Note that this method cannot remove local
singularities. High speed frontal solver only
CMAT
print the material property input data
CONV
Include convective acceleration terms when APIW is operative. Default for non
COOR
print coordinate data
CORE
write element stiffnesses etc. to data manager instead of backing files
CSKE
print the skew systems input data
APIW analyses (See Appendix M.7)
CSUP
print the suppressions input data
DDEC
delete the decomposed stiffness disc file before an eigenvalue analysis
DATA
perform a data check run only
DIRE
print the direct mass input data
DTRS
initial conditions supplied in a transient dynamic restart to the previous solution
ELAX
print offset and local axes information for each beam and tube element in the
structure
ELEM
print the element topology data
EPSN
engineering plane strain model for membranes
FCRO
print full summary for automatically selected creep solution times (summary is
short by default)
FDMS
print a list of freedoms at each node
FEMV
produce ‘FEMVIEW’ analysis model file (see note)
FIXD
read data input in fixed format
FNUM
print a list of freedom numbers (I.e position of freedom in solution vector)
FSOL
instruct the program to use the ordinary frontal solver
GAUS
print out stress sampling points for elements with stress output
GEOM
print the geometric property data
GLST
global stress output (see Appendix -A for valid element types)
GOON
continue with solution even when warnings present in data
HYDR
print detailed elemental hydrodynamic information (see Appendix M.7)
IEST
use initial elastic stiffness for first iteration when there is residual stress input
INEL
use input element order for solution order
LINS
use line search procedure (cannot be used with CONSIT with the SOLUTION
command)
LOWE
convert all higher order element types to lower order ones in steady state heat
analysis. When used, the geometric properties data must refer to the lower order
element types only
MATE
print the material properties data
MCON
vary current profile to maintain mass conservation. This is not recommended for
use with API analyses (See Appendix M.7)
MYEL
use user element order for solution order
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-22
ASAS (Non-Linear) User Manual
Preliminary Data
NODL
print only selected expanded data (“No Data List”)
NOKC
no centrifugal stiffness to be included in tangent stiffness matrix
NOKP
no pressure load stiffness to be included in tangent stiffness matrix
NOPF
no porthole file created for post-processing using POSTNL
NOPG
suppress page throws in output
NORE
no resultants calculated for applied loads during data checking
OVIT
override iteration limit (i.e. continue to next load increment when iteration limit
exceeded)
PATN
produce ‘PATRAN’ neutral file for analysis model (see note)
PLSN
plane strain model for membrane elements
PRNO
print only selected input data
RELC
vary current profile such that the velocities are not at absolute depths, but relative
depths (See Appendix M.7)
RVOF
switch off relative velocity formulation in Morison’s equation for wave load
calculation (See Appendix M.7)
SAVJ
save journal file INCRJF
SECN
use Secant-Newton acceleration (SOLVE solution procedure only)
SKEW
print the skew systems data
SURF
use temperature at node 1 to determine material properties. Only apply to FAT2
elements with FLNS option (see GROUP or PROBLEM commands)
TRAP
trapezoidal rule used for through thickness integration for shells
TWOD
convert plane stress membranes and FLA2 to 2-D forms
VEXT
no modification to current profile in the presence of wave, simple extrapolation is
used above still water level. Default for non-APIW analyses. (See Appendix
M.7)
VISC
use viscoplastic creep solution method (See Appendix -J). Not available for
creep law LAW4.
Note
FEMV and PATN are mutually exclusive options.
5.1.19
OUTPUT Command
This command defines the points in time at which results are to be output.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-23
Preliminary Data
ASAS (Non-Linear) User Manual
OUTPUT
blocno
TGEN
stime
timei
ntime
IGEN
incst
iinc
nincs
ALL
INCR
incno
TIME
ptime
Parameters
OUTPUT
: command keyword
blocno
: number of the block controlled by this command. A BLOC command is then required.
(Integer)
TGEN
: keyword indicating that a list of times is to be generated
stime
: start time for list of generated times. (Real)
timei
: time increment to be added to start time for list of generated times. (Real, ≥ 0.0)
ntime
: total number of generated times, including start time. (Integer, > 0)
IGEN
: keyword indicating that a list of increments is to be generated
incst
: start increment for list of generated increments. (Integer)
iinc
: increment to be added to start increment for list of generated increments. (Integer, > 0)
nincs
: total number of generated increments, including start increment. (Integer, > 0)
ALL
: keyword indicating that output is required at all times/ increments
INCR
: keyword indicating that a list of increment numbers are supplied
incno
: increment number for which results are to be output. (Integer)
TIME
: keyword indicating that a list of pseudo-times are supplied
ptime
: pseudo-time for which results are to be output. (Real)
Notes
1.
If GROUPS are used, then all commands controlling output (i.e. OUTPUT, BLOCK) must appear in the
GROUP section other than commands controlling DISPlacement output which always appear in the
PROBLEM section.
2.
INCR or IGEN may only be used with SOLUTION solution method.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-24
Preliminary Data
ASAS (Non-Linear) User Manual
3.
4.
TIME or TGEN may only be used with SOLVE solution method.
If the list of pseudo times/increments at which output is required is too long for one line, specify further
5.
OUTPUT commands with the same block number.
If a time or increment is re-specified with a subsequent OUTPUT command the output identifiers with
the associated BLOCK command(s) are overwritten.
5.1.20
PARAMETER Command
This command enables the values of certain problem parameters to be set. Optional
PARAMETER
ident
pv al
Parameters
PARAMETER : command keyword
ident
: alphanumeric identifier. See table below.
pval
: value of parameter ident. See table below. (Real or Integer)
Identifier
Definition and value
SUBINC
Number of plasticity subincrements (default 1) (see Appendix C.3). (Integer)
SUBTOL
Plasticity strain tolerance used to calculate a number of plasticity subincrements (see Appendix C.3). (Real)
MXSUBI
Limit for number of plasticity subincrements (default 20). (Integer)
TREFLD
Reference temperature for temperature loads. (Real)
TAZERO
Absolute zero temperature for radiation calculations. (Real)
GAPSTF
Gap stiffness factor (default 1.0E3). (Real)
GAPSMA
Gap residual stiffness factor (default 1.0E-8) See GAP element description
sheets (Appendix -A). (Real)
TIMBEG
Pseudo time corresponding to zero load state (default 0.0). (Real)
DRILF
Stiffness multiplier for fictitious local RZ stiffness for shells (default 1.0E08). (Real)
PENFUN
Penalty function multiplier for fictitious local RZ stiffness for shells (used in
conjunction with FLATOL) (default 1.0). (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-25
ASAS (Non-Linear) User Manual
FLATOL
Preliminary Data
Shell flatness threshold to activate penalty function control of local RZ
stiffness (largest angle between opposite diagonal normals in degrees)
(default 90.0). (Real)
SHEARL
Shear locking reduction factor for TCS and TSD elements (default 19.2).
(Real)
LNMULT
Line search multiplier for control parameter adjustment. (Real)
EIGCNV
Subspace iteration convergence tolerance (default 1.0E-05). (Real)
MXAUTO
Limit for number of repeated AUTO restarts for special solution methods
(default 3). (Integer)
FINCMX
Maximum step increasing actor for special solution methods. (default 1.5 for
LOAD, 10.0 for ARCL, TARCL and CONSIT). (Real)
TINCMX
Maximum timestep for special solution method LOAD. (Real)
TINCMN
Minimum timestep for special solution methods LOAD. (Real)
KSIGNL
Number of consecutive step increasing signal before actual increase is made
for special solution method LOAD (default 2). (Integer)
STEPRF
Step reduction factor in auto-restart for special solution methods (default
0.5). (Real)
SCONLO
Solution diagonal decay ratio - warning threshold (default 1.0E5). (Real)
SCONHI
Solution diagonal decay ratio - abort threshold (default 1.0E12). (Real)
SERCH1
Line search tolerance for interpolation (default 1.0). (Real)
SERCH2
Line search tolerance for extrapolation (default 0.7). (Real)
SERCL1
Lower limit for line search factor (default 0.01). (Real)
SERCL2
Upper limit for line search factor (default 10.0). (Real)
FACLSP
Line spring factor (default 0.4). (Real)
MXAUGM
Maximum number of Lagrangian augmentations (default 0). (Integer)
GAPCVG
Penetration tolerance for Lagrangian augmentations (default 0.001). (Real)
TANCVG
Tangential relative displacement tolerance at stick positions for Lagrangian
augmentation (default 0.001). (Real)
Notes
1.
2.
SUBINC and SUBTOL are mutually exclusive.
TREFLD and TIMBEG cannot be redefined on a restart.
3.
Some identifiers may be specified in both the PARAMETER and TEMPORAL command. If an
identifier is defined more than once, the last definition will be assumed.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-26
Preliminary Data
ASAS (Non-Linear) User Manual
5.1.21
PASS Command
This command invokes the frontwidth optimisation facility. Optional
PASS
(method)
(npass)
Parameters
PASS
: command keyword
method
: optional word; KING, LEVY, PINA, or SLOAN, to indicate method of optimising. If blank,
CUTHILL-MCKEE is assumed. However, when the optimised frontal solver is adopted, the
default method is SLOAN.
npass
: number of attempts to reduce the frontwidth. If blank, defaults to 2 for SLOAN and 10 for
other methods. (Integer)
Note
1.
The frontwidth optimiser assumes that all elements with the same node number are connected together
according to data given in element topology data. In the situation where elements contain an auxiliary
node (SST4, STF4, and WST4), it is advisable to assign a unique node number to each auxiliary node so
that the final outcome of the optimisation process will not be affected.
2.
Two passes are always performed with SLOAN unless npass is explicitly set to 1.
3.
The SLOAN method is only available with the optimised frontal solver.
5.1.22
PINO Pressure Interpolation Order Command
The PINO command defines the pressure interpolation order to be used by specified elements. To avoid
numerical problems with incompressible or nearly incompressible materials, this command may be used to
specify a different (lower) interpolation order for the volumetric strain. If the PINO command is not present the
normal displacement formulation is used. Optional
PINO
inpr
(elno)
Parameters
PINO
: command keyword
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-27
Preliminary Data
ASAS (Non-Linear) User Manual
inpr
: pressure interpolation order. (Integer)
elno
: list of element numbers in topological format. (Integer)
If blank, defaults to all elements (in group)
Notes
1.
2.
This command is recommended for use with the hyperelastic material model
The recommended pressure interpolation orders and the associated element types are given below:
Interpolation
Elements
order
1
BRK6
BRK8
BR15
BR20
QUM4
QUM8
TRM3
TRM6
QUX4
QUX8
TRX3
TRX6
3
QUM8
TRM6
QUX8
TRX6
4
BR15
BR20
Example
A rubber membrane with a mesh of 100 high order membrane elements (QUM8’s and TRM6’s)
PINO 3 (100) (1,1)
5.1.23
PROBLEM and TITLE Command
This command is mandatory and must immediately follow the JOB command.
PROBLEM
(direct)
(*
title)
TITLE
Parameters
PROBLEM
: command keyword
TITLE
: command keyword
direct
: 4 character directives defining structural and material model to be used. May be one or more
of the following:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-28
Preliminary Data
ASAS (Non-Linear) User Manual
GLST
compute stresses/strains in global axis system
LOST
compute stresses/strains in local axis system
PLAS
take plasticity effects into account
LARG
include large displacement effects in the calculation of strains and geometric
stiffness matrices.
This directive should be accompanied by the command
UPDATE GEOM (see UPDATE command)
CONL
use conservative pressure loading - i.e. calculate pressure loads using original
geometry throughout.
NRES
Only applicable with UPDATE GEOM (see UPDATE
command)
do not carry forward residuals into next increment.
FLNS
form natural stiffness (i.e. Young’s modulus*Area) for FLA2 and FAT2 elements
CREP
EXPL
creep analysis
use explicit temporal integration scheme for transient analysis
*
: character to indicate the following text forms the title
title
: any alphanumeric title of up to 60 characters including blanks. It must be preceded by an
asterisk (*). This title will be printed at the top of each page of ASASNL output
Notes
1.
If no directives are given linear elastic behaviour is assumed with the default implicit temporal integration
2.
scheme for transient analysis and stresses are computed in the element default axis system.
This is a global switch and will set these directives for all groups regardless of what is put on the GROUP
commands. You can, however, add other directives with the GROUP commands.
3.
4.
The first six characters of the title are used for the problem name.
The PROBLEM command and TITLE command are identical and interchangeable.
5.1.24
PROJECT Command
To define a name and title for the project. Optional but project name is recommended.
PROJECT
(pname)
(*
title)
Parameters
PROJECT
: command keyword
pname
: project name for current run (Alphanumeric, 4 characters, first character must be alphabetic). If
pname is omitted, then pname defaults to the name ASNL
*
: character to indicate following text forms the project title.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-29
Preliminary Data
ASAS (Non-Linear) User Manual
title
: any alphanumeric title of up to 60 characters including blanks. It must be preceded by an
asterisk (*). The default project title is ‘ASAS-NL ARCHIVE FILE’
Notes
1.
All runs with the same project name access the same ASAS data base and hence this must be the same in
all restarts. A project data base consists of one project file (with a file name consisting of the 4 characters
of pname with the number 10 appended) which acts as an index to other files created under this project,
2.
together with those other files.
The title is used by the program as an identifier for the archive files saved. Subsequent jobs requiring to
use those files must have the same identifying title (in addition to the correct file names with the FILE
command).
5.1.25
RESTART Command
This command is used in restarted runs in place of the SOLVE command. It defines times at which a solution is
to be attempted. It must follow the PROBLEM or TITLE command. Compulsory
TGEN
stime
timei
ntime
RESTART
time
Parameters
RESTART
: command keyword
TGEN
: keyword indicating that a list of times is to be generated
stime
: start time for list of generated times. (Real)
timei
: time increment to be added to start time for list of generated times. (Real, ≥ 0.0)
ntime
: total number of generated times, including start time. (Integer, >0)
time
: time for solution. (Real)
Notes
1.
All times must be non-negative.
2.
The first time, time1, must correspond with the time on the restart file for the chosen checkpoint and
agree within 3 decimal places. The checkpoint number is defined using the JOB command.
3.
No solution is attempted at time, time1.
4.
Solution times may be continued using subsequent RESTART commands.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-30
ASAS (Non-Linear) User Manual
5.
6.
Preliminary Data
All solution times specified must be greater than or equal to zero. (In general they must be greater than or
equal to TIMBEG, the zero load start time.)
The list must also be in ascending order i.e. time (i+1) ≥ time(i).
If load functions are used, then all solution times specified must be greater than, or equal to the first
pseudo time specified with each load function.
7.
8.
On a restart, only the preliminary data, suppressions, displaced freedoms, loading and additional mass can
be changed. Material property data may also be changed but only if the analysis type has been changed
from the initial run.
If temperature data is redefined on restart, the number of load sets must be the same as on the initial run.
5.1.26
RESU (or POST) Commands
This command defines the points and the information to be saved for post-processing with POSTNL, on the file
specified on a corresponding FILE command. It also defines the points where information is to be saved on the
ASAS database. Recommended
Parameters
RESU
: command keyword
POST
: command keyword (same meaning as RESU)
outid
: output identifier, one or more of the following:
DISP
displacements (temperatures for heat)
VELO
velocities (temperature rates for heat)
ACCN
accelerations
REAC
reactions (reactive nodal heat for heat)
STRS
stresses (fluxes for heat)
STRN
total strain (field for heat)
INST
inelastic strains
ELAS
elastic strains
SRES
stress resultants
WORK
element mechanical work (NOT saved to ASAS database)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-31
ASAS (Non-Linear) User Manual
Preliminary Data
TEMP
temperatures (NOT saved to ASAS database)
EIGN
mode shapes
CRSN
SUMR
creep strains
output summary of maximum displacements, velocities, accelerations, summed
reactions and solution control information (only summed reactions saved to ASAS
database)
TGEN
: keyword indicating that a list of times is to be generated
stime
: start time for list of generated times. (Real)
timei
: time increment to be added to start time for list of generated times. (Real, ≥ 0.0)
ntime
: total number of generated times, including start time. (Integer, > 0)
IGEN
: keyword indicating that a list of increments is to be generated
incst
: start increment for list of generated increments. (Integer)
iinc
: increment to be added to start increment for list of generated increments. (Integer, > 0)
nincs
: total number of generated increments, including start increment. (Integer, > 0)
ALL
: keyword indicating that information is to be stored for all increments
INCR
: keyword indicating that a list of increment numbers is supplied
incno
: increment number for which results are to be stored. (Integer)
TIME
: keyword indicating that a list of times is supplied
time
: time for which results are to be stored. (Real)
Notes
1.
SRES must be saved if layer stresses/strains or failure indices are required to be recovered in POSTNL
2.
for an elastic laminated shell analysis.
DISP, STRS, STRN, ELAS and INST (if plasticity) must be saved if fracture mechanics processing is
required in POSTNL. For creep fracture, CRSN must also be saved in addition and results from at least
two increments must be available.
3.
INCR or IGEN may only be used with SOLUTION solution method.
4.
5.
TIME or TGEN may only be used with SOLVE solution method.
Information written to the ASAS database consists of two parts. The first part is equivalent to the
specification of SAVE LOCO FILES in ASAS. Data which will only be generated for ASAS
compatible element types, are written to the “35 file”. The second part concerns with saving of results.
This information is written to the “45 file”.
6.
If post-processing using POSTNL is not required, option NOPF can be used to supress the generation of
porthole file. Data will always be written to the ASAS database
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-32
Preliminary Data
ASAS (Non-Linear) User Manual
7.
POST/RESU command alone will cause saving of DISP, STRS and SUMR in all increments/times. In
addition, the SURFACE FAILURE results will be saved to the ASAS database in a job involving
plasticity or failure.
If the results database is to be used in any post-processing run then a RESU command must be included
8.
in the initial ASAS run to initialise the database.
9.
The last POST/RESU command at a time overrides all the previous specifications.
5.1.27
SAVE Command
This command defines points at which run information is stored on the stiffness and data manager archive files.
File names are defined on appropriate FILE commands. Optional
STEP
ninc
NEW
SAVE
ALL
OLD
(ROLL
nsol)
ptminc
Parameters
SAVE
: command keyword
NEW
: keyword to indicate that new files are to be created
OLD
: keyword to indicate that existing files are to be used - information is appended to the old files
(except that a restarted run from an intermediate checkpoint will override previously dumped
information for higher checkpoints)
STEP
: keyword to indicate that information is to be stored every ‘ninc’ increments
ninc
: see above. (Integer)
ROLL
: keyword to indicate that a rotating set of ‘nsol’ solutions will be stored on the archive file
nsol
: see above. (Integer)
ALL
: keyword to indicate that information is to be stored after all load increments
ptminc
: pseudo time (Real) or increment (Integer) for which restart information is to be stored
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-33
Preliminary Data
ASAS (Non-Linear) User Manual
Notes
1.
If OLD then there should not be any FILE commands referring to new stiffness and archive files.
2.
Information is saved on the stiffness archive file only if stiffnesses have been updated since the previous
3.
checkpoint.
Information is always saved on both files on the last increment of a successful analysis.
4.
ROLL should not be used to hold less than 3 increments.
5.1.28
SCALING Command
Controls scaling of applied loads for proportional loading to a factor times yield stress on first load increment.
See Note.
SCALE
ident
v al
Parameters
SCALE
: command keyword
ident
: an alphanumeric identifier. If no identifier is specified, then applied loads are scaled until first
yield is reached. Allowable identifiers are as follows:
RPROP
Reference proportion for scaling.
The reference value for scaling is this
proportion multiplied by the yield stress. The default value is one.
SCALIM
This specifies a ceiling value to the load factor. If omitted no limiting value is
enforced.
val
: value for selected identifier. (Real)
Note
This command is an alternative to the SOLVE command. The job terminates after scaling to the value given
and can be restarted as requested. No SAVE command is required.
5.1.29
SKIP Command - (Group Section Only)
This command defines the elements to be skipped from a group. It is valid only in conjunction with an
ELGROUP command.
Optional
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-34
Preliminary Data
ASAS (Non-Linear) User Manual
elno
SKIP
Parameters
SKIP
: command keyword
elno
: list of element numbers given in topological format. (Integer)
Notes
The order of ELGROUP and SKIP Commands within a group is not important.
Example
Assign elements 1, 2, 4, 6, 9, 10 to group 3
5.1.30
GROU
3
*
ELGR
(10)
(1,1)
SKIP
3
5
SKIP
(2)
(7,1)
BEAM
ELEMENTS
SLEEP Command
This command defines the elements which will become inactive (sleep) during part of the analysis. Optional
ptime
SLEEP
elno
incno
Parameters
SLEEP
: command keyword
ptime
: pseudo time at which element sleeps (SOLVE). (Real)
incno
: increment number at which element sleeps (SOLUTION). (Integer)
elno
: list of element numbers in topological format. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-35
Preliminary Data
ASAS (Non-Linear) User Manual
Notes
1.
The same element number cannot be specified more than once in the entire list of SLEEP commands.
This means that an element cannot sleep more than once during a run.
2.
The element is put to sleep before the solution for the specified time/increment number is obtained. Thus
the element is inactive for the time/increment number specified and for all times/increment numbers
thereafter. It is important to note that global mass, damping and stiffness matrices are not updated unless
specifically requested. Appropriate UPDATE commands should be specified at the time/increment
3.
number specified with the SLEEP command.
If the pseudo time specified is within the lower and upper limits of solution times given on the SOLVE
(or RESTART) commands, then it must coincide with one of the solution times.
4.
If both WAKE and SLEEP times/increment numbers are present for an element, the wake
time/increment has to be before the sleep time/increment number.
5.
The list of element numbers specified with the WAKE/SLEEP commands cannot be changed during any
subsequent restart analysis.
6.
Care should be taken using the WAKE/SLEEP commands when load type NODAL LO has been
specified. Internally, ASAS-NL attaches all nodal loads to the element with the highest system element
number which references the freedom to which the nodal load is applied. When an element which has
nodal loads attached in this manner is woken up or put to sleep, the nodal load is also woken up or put to
sleep, as are all element loads.
5.1.31
SOLUTION Command
Defines automatic load (or time) stepping procedure for static and transient dynamics analysis in a virgin run
(used instead of SOLVE command). If used this command must immediately follow the PROBLEM or TITLE
commands. For restarted runs, the SOLUTION command is replaced by the SRESTART command. Note that
SOLUTION (and SRESTART) cannot be used for creep analysis. Instead, the creep automatic timestepping
procedure is activated by specifying AUCR in the OPTION command together with SOLVE (or RESTART)
SOLUTION
method
ninc
direct
v al
Parameters
SOLUTION:
method
command keyword
: special solution method name (Alphanumeric). Valid methods are:
LOAD
Constant load control. This method is applicable to static analysis with any load
history types. It is not suitable for predicting limit point or snap behaviour.
ARCL
Cylindrical arc-length control (i.e. constant displacement vector increment
(DPVEC)). Constraint on the step size has quadratic form, thus no distinction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-36
Preliminary Data
ASAS (Non-Linear) User Manual
between the positive and negative path direction is available.
This method is
applicable to static analysis with proportional loading only. It can deal with limit
point or snap behaviour.
TARCL
Linearised cylindrical arc-length control.
This method is applicable to static
analysis with proportional loading only.
It can deal with limit point or snap
behaviour.
CONSIT
Constant displacement component increment (DPCOM) control. Constraint on the
step size has linear form, thus positive and negative value of an increment is
recognised. This method is applicable to static analysis with proportional loading
only. It can deal with limit point or snap behaviour.
DOMFRQ
Dominant frequency control. This method is applied to transient dynamics analysis
using implicit time integration only.
MAXFRQ
Maximum frequency control. This method is applied to transient dynamics analysis
using explicit time integration only
ninc:
maximum number of increments to be attempted.
direct:
alphanumeric directive. See table below
val:
value(s) associated with the directive. (Integer, Real or Character, see table below)
Below are the directives for use with the SOLUTION and SRESTART commands.
(A)
For method LOAD
Identifier Definition and value
FIRTIM
The first solution pseudo-time. (Real, ≥last solution time)
FIRTIN
The initial pseudo-time increment. (Real, >0.0)
MAXTIM The maximum solution time. (Real, ≥last solution time)
ITERD
Desired number of iterations per increment. If set to zero step size adjustment is
independent of number of iterations (default 4). (Integer, ≥0)
Notes
1
FIRTIM and/or FIRTIN must be specified. If FIRTIM is omitted, the first solution time is assumed to
be the last solution time in the previous run (or 0.0 for a new run). Conversely, if FIRTIN is omitted,
the initial time step size is taken as the difference between FIRTIM and the last solution time (or 0.0
for a new run). If both are specified, the first solution time will be FIRTIM while the next step (i.e. the
second step) will have a step size of FIRTIN.
2
Additonal control parameters are available in the PARA commands.
These include FINCMX,
TINCMN, TINCMX, KSIGNL, STEPRF and MXAUTO.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-37
Preliminary Data
ASAS (Non-Linear) User Manual
3
The automatic load procedure may not be effective when there is a sudden change of loading from the
previous increments. If difficulty arises, a restart should be carried out with the load stepping control
parameters re-defined.
4
The run terminates when either the maximum number of increments or the maximum solution time is
reached. In the latter case, the last solution will always be attempted at time MAXTIM.
5
Further details are given in Appendix C.
(B)
For methods ARCL, TARCL and CONSIT
Identifier
WORKC
Definition and value
Adopts constant external work increment control in conjunction with ARCL or
CONSIT. May not be used on first restart following standard solution procedure.
Switch tolerance. If set to zero this procedure is used in all increments. (Real)
AUTO
Automatic selection of displacement component to be controlled. Used with CONSIT
only.
Size of incremental displacement. (Real)
INITPR
Defines initial step size. Used with ARCL and TARCL only.
Initial proportion of reference load. (Real)
INCDIS
Defines initial step size.
Mandatory with CONSIT and optional for ARCL and
TARCL. Three parameters to follow:
Nominated node. (Integer)
Nominated freedom name. (Alphanumeric)
Initial incremental displacement of nominated freedom. (Real)
ITERD
Desired number of iterations per increment. If set to zero step size adjustment is
independent of number of iterations (default 4). (Integer, ≥0)
MAXIPR
Maximum incremental proportion of reference load. used with CONSIT only. (Real)
MAXLOD
Terminates the run when this proportion of reference load is exceeded. (Real)
MAXDIS
Terminates the run when total displacement of the specified freedom is exceeded. Three
parameters to follow:
Nominated node. (Integer)
Nominated freedom name. (Alphanumeric)
Maximum displacement of nominated freedom. (Real)
CONDIR
Controls loading direction. Used on restarts with ARCL and TARCL only..
Controlling parameter taking value +1.0 or -1.0. (Real)
Notes
1
INITPR or INCDIS must be specified when ARCL or TARCL is used.
2
Additional control parameters are available in the PARA commands.
3
These procedures can only be applied to static analysis with proportional loading.
4
For analysis containing a dead load set (i.e. non-proportional part) and a live load set (i.e. proportional
part), the dead loads may be applied in a SOLVE run followed by restart using the special solution
procedure for the live loads.
In this case, only the proportional load data is required in the
SRESTART run.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-38
Preliminary Data
ASAS (Non-Linear) User Manual
For methods DOMFRQ and MAXFRQ
(C)
Identifier
Definition and value
FIRTIM
The first solution time. (Real, ≥last solution time)
FIRTIN
The initial timestep size. (Real, >0.0)
MAXTIM
The maximum solution time. (Real, ≥last solution time)
ITERD
Desired number of iterations per increment. if set to zero step size adjustment is
independent of number of iterations (default 4). (Integer, ≥0)
Notes
FIRTIM and/or FIRTIN must be specified. If FIRTIM is omitted, the first solution time is assumed to
1
be the last solution time in the previous run (or 0.0 for a new run). This setting is useful for
determining the consistent initial accelerations from given initial conditions and/or initial loading.
Conversely, if FIRTIN is omitted, the initial time step size is taken as the difference between FIRTIM
and the last solution time (or 0.0 for a new run). If both are specified, the first solution time will be
FIRTIM while the next step (i.e. the second step) will have a step size of FIRTIN.
2
Additional control parameters are available in the PARA and TEMP commands.
3
Further details are given in Appendix K.
5.1.32
SOLVE Command
This command invokes the classical solution method (incremental Newton-Raphson) and defines points at which
a solution is to be attempted for a virgin run. It must follow either the PROBLEM/TITLE command. In
restarted runs it is replaced by the RESTART command.
TGEN
stime
timei
ntime
SOLVE
time
Parameters
SOLVE
: command keyword
TGEN
: keyword indicating that a list of times is to be generated
stime
: start time for list of generated times. (Real)
timei
: time increment to be added to start time for list of generated times. (Real, ≥ 0.0)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-39
Preliminary Data
ASAS (Non-Linear) User Manual
ntime
: total number of generated times, including start time. (Integer, > 0)
time
: time at which a solution is to be attempted. Times must be non-negative. (Real)
Notes
1.
List of times may be continued using subsequent SOLVE commands.
2.
The solution method activated by the SOLVE command can be used for static problems of proportional
or non-proportional loading. The latter is defined by explicitly specifying load history. Otherwise
proportional loading is assumed with the load multiplier equal to the time at each solution point.
3.
4.
This solution method is compulsory for creep analysis.
All solution times specified must be greater than or equal to zero. (In general they must be greater than or
equal to TIMBEG, the zero load start time.)
The list must also be in ascending order i.e. time(i+1) ≥ time(i).
5.
If load functions are used for solution times specified outside the pseudo times specified with each load
function, extrapolation will be used.
5.1.33
SPIT Command
This command sets the parameters for the Subspace Iteration Eigen Solution. If present it must be accompanied
by an EIGN command. Optional and only for Eigen Solution.
KGEOM
SPIT
UNITM
ident
v al
MASS
Parameters
SPIT
: command keyword
KGEOM
: keyword to indicate that the current small displacement stiffness Ko and the geometric stiffness
KG matrices are to be used for a buckling analysis
UNITM
: keyword to indicate that the current small displacement stiffness Ko and the unit I matrices are
to be used for a spectral analysis
MASS
: keyword to indicate that the current tangential stiffness KT and the mass M matrices are to be
used for a natural frequency analysis
ident
: alphanumeric identifier. See table below
val
: value associated with the specified identifier. (Integer and Real)
Identifier
Definition and value
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-40
Preliminary Data
ASAS (Non-Linear) User Manual
NORME
Eigenvector normalisation. (Integer)
0 Maximum component is 1.0 (default)
1 Euclidean norm is 1.0
SCOPE
Scope of solution. (Integer)
0 Eigenvalues and modes (default)
1 Eigenvalues only
NHIGHF
Number of eigenvalues required. (Integer)
1≤NHIGHF≤NSUBSP
NSUBSP
(default to 1)
Number of eigenvalues to iterate over (size of subspace). If omitted then
default value is calculated automatically by the program. (Integer)
0≤NSUBSP≤NFREE, where NFREE is the number of free freedoms.
LMSPIT
Maximum number of iterations in eigenvalue solution (default 45) (Integer)
EIGCNV
Convergence tolerance in eigenvalue solution (default 0.00001). (Real)
SELMOD
Number of mode selected for perturbation.
1<SELMOD<NHIGHF (default 1). (Integer)
PERTMG
Relative magnitude of perturbation (default 0.005). (Real)
STURM
Sturm sequence check flag. (Integer)
SHIFT
0 =
no check (default)
1 =
check required
Eigenvalue shift (default 0.0). (Real)
The shift should be specified in eigenvalue units for buckling problems.
The shift should be specified in frequency units (Hz) for natural frequency
problems
STARTV
Method for forming the Starting Vectors
0
=
Vectors generated based on the stiffness to mass ratio (default)
1
=
Use last calculated eigenvectors as starting vectors
Notes
1.
To obtain the KG matrix for SST4/WST4 elements the LARG directive must be specified with the
GROUP or PROBLEM/TITLE commands.
2.
3.
See Appendix C.5 for further details concerning eigenvalue analysis.
Load stiffness will only be ignored if CONL is specified with the GROUP or PROBLEM/TITLE
4.
commands.
A shift must be applied if there are not enough suppressions in the model to remove all the rigid body
motions. Eigenvalue analysis of a free structure is allowed for UNITM and MASS provided no loading is
applied. The structure must have adequate suppressions for KGEOM.
5.
NHIGHF and NSUBSP will be reset if their specified values are outside the allowable bounds.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-41
Preliminary Data
ASAS (Non-Linear) User Manual
6.
The eigenvalues of a shifted problem are arranged in ascending order of their distance from the shift
origin. The eigenvalues of the original problem, which are reported in the output file, will be given in the
same order.
The sturm sequence check implemented assumes that the lowest modes have been computed and the
7.
eigenvalues are monotonially increasing. It should not be applied to problems where these conditions are
not satisfied. One such example is when a shift is applied to determine the higher modes directly.
The use of last calculated eigenvectors as starting vectors is only allowed in a restart analysis if the
8.
subspace size NSUBSP remains unchanged between runs.
5.1.34
SRESTART Special Solution Restart Command
Defines special solution options for restart run. (Used instead of RESTART command and must follow the
PROBLEM or TITLE command.)
SRESTART
FROM
incno
method
ninc
direct
v al
Parameters
SRESTART : command keyword
FROM
: keyword
incno
: increment number of increment immediately before start. (Integer)
method
: special solution method name. See SOLUTION command for valid names.
ninc
: maximum number of increments to be attempted.
direct
: alphanumeric directive The directives used vary according to the special solution option
selected. See the table detailed with the SOLUTION command, and below.
val
: value(s) associated with the directive. (Integer, Real or Character)
The directive below is for use with SRESTART command only.
Identifier
Definition and value
STEP
Defines directly step size. Used with ARCL only.
Length of incremental displacement vector. Is used as an alternative to
INITPR or INCDIS. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-42
ASAS (Non-Linear) User Manual
Preliminary Data
Notes
1.
The loading information will not be correctly transferred to the ASAS database if the restart adopts a
variable load solution procedure (e.g. ARCL) while the initial run adopts a fixed load procedure (SOLV
or SOLU LOAD). This may affect the results of code checking using BEAMST.
5.1.35
START Command
This command defines the list of starting node numbers for any renumbering attempt specified with the PASS
command. This command must only be used in conjunction with the PASS command and need not be present.
If absent the renumbering will commence from a point chosen by the program. (A maximum of 3 START
commands can be provided and each one can consist of up to 10 nodes). Optional
START
nodeno
Parameters
START
: command keyword
nodeno
: node number with which to start any renumbering attempt. A maximum of 10 node numbers
may be specified. (Integer)
Notes
1
Up to 3 starting vectors may be specified.
2
Number of passes will be equal to number of starting vectors if START is used.
3
START will have no effect on the Sloan method and, thus, is not required when adopting this method.
5.1.36
STRUCTURE Command
To define the structure name for a new run or an existing model name for a restarted run. Optional but
recommended.
STRUCTURE
sname
Parameters
STRUCTURE :
keyword
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-43
Preliminary Data
ASAS (Non-Linear) User Manual
sname
: structure name. The name must be unique from all other structure names in this project.
(Alphanumeric, 4 characters, the first character must be alphabetic)
Notes
1.
sname is used as a prefix for all ASAS backing files created during a new run. The four characters are
appended with two digits to create each individual file. In a restarted job, this defines an existing
structure from which the current run is based upon.
2.
If the STRUCTURE command is omitted then the project name pname is used in place of sname
Example
STRUCTURE
5.1.37
SHIP
SYSPAR Command
This command, if present, must precede the JOB command. It allows the values of certain system parameters to
be reset. Optional
SYSPAR
ident
v al
Parameters
SYSPAR
: command keyword
ident
: alphanumeric identifier. See table below
val
: value associated with the specified identifier. (Integer or Logical)
Identifier
Definition and value
LPGSIZ
Data manager page size. (Integer, must not exceed 16383)
MINPAG
Minimum number of incore pages reserved for data manager. (Integer)
LTPAGE
Maximum length of page directory. (Integer, must not exceed 65535)
LMJIA
Length of archive file major index. (Integer, must not exceed 16383)
MANREC
Default length of subindex. (Integer)
IPERM
1 = use permanent files; 0 = use temporary files. (Integer)
NOPAG
Block multiplier for LENTRK (length solution backing files). (Integer)
SINDEC
.TRUE. if reduced stiffness to be archived (if .FALSE., this file will be
reformed by decomposing the stiffness file on restarts) (Logical)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-44
Preliminary Data
ASAS (Non-Linear) User Manual
LEVSYS
System abort level. (Integer)
MXCONS
The maximum of MXCONS and NCONEQ constraint equations will be
allowed for restarts. (Integer.)
NCONEQ is the number of constraint
equations in the initial run.
OPENFL
Default number of keys with which an internal ASAS file is opened (integer)
Notes
1.
See Table 6.1 for default values and Section 6.2 for the significance of some of the system parameter.
2.
3.
In a restart, new constraint equations can be added but cannot contain a constant term.
LPGSIZ and LMJIA must be the same and the program will ensure this if either is specified.
5.1.38
SYSTEM Command
To define the amount of data space to be allocated during the run. Optional.
SMALL
(MEDIUM)
SYSTEM
DATA
AREA
memory
(initm)
LARGE
Parameters
SYSTEM
: command keyword
SMALL
: keyword indicating data manager page size
MEDIUM
: keyword indicating data manager page size (default size)
LARGE
: keyword indicating data manager page size
DATA
: keyword
AREA
: compulsory keyword
memory
: amount of memory (in 4 byte words) to be used by this run. A minimum of 1000000 is
assumed. (Integer)
initm
: initial memory reserved. Not normally used. (Integer)
Note
See Table 6.1 for optional page sizes.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-45
Preliminary Data
ASAS (Non-Linear) User Manual
5.1.39
TEMPORAL Command
This command allows the user to vary the temporal integration scheme used for transient analysis and the
parameters associated with automatic timestepping.
TEMPORAL
ident
v al
Parameters
TEMPORAL
:
command keyword
ident
: alphanumeric identifier. See table below.
val
: value of identifier. See table below.
Identifier
Definition and value
TALPHA
Temporal integration scheme coefficient (default 0.0). (Real)
TBETA
Temporal integration scheme coefficient (default 0.5). (Real)
TGAMMA
Temporal integration scheme coefficient (default 0.25). (Real)
VALPHA
Creep integration weighting factor. Any value between 0.0 and 1.0 may be
used. (Default 0.0). (Real)
DCSTMX
Autocreep control parameter (use with OPTION AUCR only). Maximum
incremental creep strain. (Real)
DCESMX
Autocreep control parameter (use with OPTION AUCR only). Maximum
ratio of incremental creep strain to total strain. (Real)
DSIGMX
Autocreep control parameter (use with OPTION AUCR only). Maximum
ratio of incremental stress to total stress. (Real)
TINCMX
Automatic timestepping control parameter for creep and transient dynamics.
Maximum timestep. (Real)
TINCMN
Automatic timestepping control parameter for creep and transient dynamics.
Minimum timestep. (Real)
FINCMX
Automatic timestepping control parameter for creep and transient dynamics.
Maximum ratio of new timestep to previous timestep. (Real)
FIRSTP
Autocreep control parameter (use with OPTION AUCR only).
First
timestep for this solution or restart. (Real)
MXINCS
Autocreep control parameter (use with OPTION AUCR only). Maximum
number of timesteps for this solution or restart. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-46
ASAS (Non-Linear) User Manual
TFACLO
Preliminary Data
Automatic timestepping control parameter for transient dynamics. Lower
limit on ξ for no change in timestep. (Real)
TFACHI
Automatic timestepping control parameter for transient dynamics. Upper
limit on ξ for no change in timestep. (Real)
TFACRJ
Automatic timestepping control parameter for transient dynamics. Limit on ξ
below which the current solution will be rejected. (Real)
FRAPRD
Automatic timestepping control parameter for transient dynamics. Desired
fraction of the characteristic period for determining the timestep. (Real)
KSIGNL
Automatic timestepping control parameter for transient dynamics. Number
of consecutive timestep increasing signal before an actual increase is made.
(Integer)
IPDICT
Predictor type for transient dynamics. (Integer)
1. Predictor acceleration equals to 0.0. (Default)
2. Predictor displacement equals to displacement at end of last step. Note
that this must not be used in explicit analysis or when TBETA=0.0.
HGAMMA
Temporal integration scheme parameter for transient heat (default 1.0).
(Real)
Notes
1.
2.
See Appendix -J for full details concerning the individual parameters for creep analysis.
See Appendix -K for full details concerning the individual parameters for transient dynamic analysis.
3.
4.
See Appendix N for full details concerning the individual parameters for transient heat analysis
Some identifiers may be specified in both the PARAMETER and TEMPORAL commands. If an
identifier is defined more than once, the last definition will be assumed.
5.1.40
TEXT Command
To define a line of text to be printed once only at the beginning of the output. Several TEXT lines may be
defined to give a fuller description of the current analysis on the printed output.
Optional
TEXT
text
Parameters
TEXT
:
command keyword
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-47
ASAS (Non-Linear) User Manual
text
:
Preliminary Data
this line of text will be printed once, at the beginning of the output. (Alphanumeric, up to 75
characters)
Example
TEXT
THIS EXAMPLE OF THE TEXT
TEXT
COMMAND IS SPREAD
TEXT
OVER THREE LINES
5.1.41
TITLE Command
See PROBLEM Command for full details of this command.
5.1.42
UNITS Command
Recommended.
This command allows the user to define the units to be employed in the analysis and the default units for the
input data. The defined unit set will appear on each page of the printout as part of the page header. If this
command is omitted then no units information will be reported and the units of all data supplied must be
consistent (see Section 3.11).
If the UNITS command is employed, facilities exist to locally modify the input data units within each main data
block. See Sections 5.2.1, 5.3.1, 5.4.1, 5.5.1 and 5.6.1 for further details.
5.1.42.1 Global UNITS Definition
This specifies the units to be employed for the analysis and provides the default units for input and printed
output.
UNITS
unitnm
Parameters
UNITS
: keyword
unitnm
: name of unit to be utilised (see below)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-48
Preliminary Data
ASAS (Non-Linear) User Manual
The units of force and length must be supplied. Temperature is optional and defaults to centigrade. A time unit
of seconds is assumed. A default angular unit of radians is used for results reporting. The default input angular
unit varies according to the data block and must not be specified on the basic UNITS command.
Restriction
The program calculates a consistent unit of MASS based upon the length and force units supplied. The
permitted combinations of force and length are given in Table 3.1.
Valid unit names
Length unit
Force unit
Temperature unit
METRE(S),
CENTIMETRE(S),
M
CM
MILLIMETRE(S),
MM
MICROMETRE(S)
NANOMETRE(S)
MICM
NANM
FOOT, FEET,
INCH, INCHES,
FT
IN
NEWTON(S)
KILONEWTON(S)
MEGANEWTON(S)
N
KN
MN
TONNEFORCE(S)
TNEF
POUNDAL(S)
POUNDFORCE,
PDL
LBF
KIP(S)
TONFORCE(S)
KIP
TONF
KGFORCE(S)
KGF
CENTIGRADE,
FAHRENHEIT,
C
F
Example
1.
Input data units and results units to be in units of Kips and feet
UNITS KIPS FEET
The derived consistent unit of mass will be 3.22x104 lbs.
Please also refer to Example 1 of Section 5.1.19.1 of the ASAS user manual.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-49
Preliminary Data
ASAS (Non-Linear) User Manual
5.1.43
UPDATE Command
These commands determine the type of solution procedure, by controlling the frequency with which the stiffness
and mass matrices are reformed and the structure geometry updated. If no update commands are specified, the
program defaults to the initial (elastic) stiffness procedure.
GEOM
UPDATE
MASS
STIF
(ELAS)
INCR
ALL
ITER
ptminc
KT1
KT2
KT0
Parameters
UPDATE : command keyword
GEOM
: keyword to update the structure coordinates each iteration
MASS
: keyword to reform the mass matrix to account for changes in geometry
STIF
: keyword to reform the stiffness matrix to account for changes in stress/strain level and/or
geometry
ELAS
: keyword to reform stiffness using elastic material properties
INCR
: keyword to reform matrix on first iteration only
ITER
: keyword to reform matrix on every iteration
KTO
: keyword to reform stiffness matrix on first iteration of first increment only (default)
KT1
: keyword to reform stiffness matrix on first iteration
KT2
: keyword to reform stiffness matrix on second iteration
ALL
: keyword to perform update specified for all increments
ptminc
: pseudo time/time (Real) or increment number (Integer) at which update is to be performed
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-50
Preliminary Data
ASAS (Non-Linear) User Manual
Notes
1.
Except for cases when the nonlinearity is low, updating of the geometry and the stiffness matrix should be
combined with the directive LARG with the PROBLEM/GROUP command.
2.
For the case of pressure loading, the current geometry is always used to calculate the equivalent nodal
loads. Therefore, using UPDATE GEOM will result in non-conservative pressure loading.
3.
If OPTION VISC is set (for viscoplastic creep solution) the stiffness matrix is automatically updated at
each iteration.
5.1.44
WAKE Command
This command defines the elements which will become active (wake up) during part of the analysis. Optional
ptime
elno
WAKE
incno
Parameters
WAKE
: command keyword
ptime
: pseudo time at which element wakes up (SOLVE). (Real)
incno
: increment number at which element wakes up (SOLUTION). (Integer)
elno
: list of element numbers in topological format. (Integer)
Notes
1.
The same element number cannot be specified more than once in the entire list of WAKE commands.
2.
This means that an element cannot wake up more than once during a run.
The element is woken up after the solution for the specified time/increment number has been obtained,
including any eigensolution requested. Thus, the element is effectively active from the time/increment
number following the time/increment number specified with the WAKE command. It is important to
note that global mass, damping and stiffness matrices are not updated unless specifically requested.
Appropriate UPDATE commands should be specified for the time/increment number when the element
becomes active, i.e. at the time/increment number following the time/increment number specified with the
3.
WAKE command.
If the pseudo time specified is within the lower and upper limits of solution times given on the SOLVE
4.
(or RESTART) commands, then it must coincide with one of the solution times.
If both WAKE and SLEEP times/increment numbers are present for an element, the wake time
increment number has to be before the sleep time/increment number.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-51
Preliminary Data
ASAS (Non-Linear) User Manual
5.
The list of element numbers specified with the WAKE/SLEEP commands cannot be changed during any
subsequent restart analysis.
6.
Care should be taken using the WAKE/SLEEP commands when load type NODAL LO has been
specified. Internally, ASAS-NL attaches all nodal loads to the element with the highest system element
number which references the freedom to which the nodal load is applied. When an element which has
nodal loads attached in this manner is woken up or put to sleep, the nodal load is also woken up or put to
sleep, as are all element loads.
5.1.45
WEIGHTS Command
This command is used in conjunction with the DISP or RESF options of the CONVERGE command to enable
the user to weight each term when calculating the convergence criteria.
WEIGHTS
freedom
rv al
Parameters
WEIGHTS
: command keyword
freedom
: freedom name. (Alphanumeric)
rval
: weight associated with the specified freedom. (Real)
Notes
1.
2.
See Appendix -F for list of valid freedom names.
Freedom names omitted will have a weight of unity.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-52
ASAS (Non-Linear) User Manual
5.2
Structural Data
Structural Description Data
These data blocks define the physical properties and shape of the structure.
The following data blocks are defined
Coordinates ............. ................ ................ see Section 5.2.2
Element Topology ... ................ ................ see Section 5.2.3
Material Properties .. ................ ................ see Section 5.2.4
Geometric Properties ................ ................ see Section 5.2.5
Section Information .................. ................ see Section 5.2.6
Skew Systems.......... ................ ................ see Section 5.2.7
5.2.1
UNITS Command
If global units have been defined using the UNITS command in the Preliminary data (Section 5.1.42), it is
possible to override the input units locally to each data block by the inclusion of a UNITS command. The local
units are only operational for the data block concerned and will return to the default global units when the next
data block is encountered.
In general, one or more UNITS commands may appear in a data block (but see notes below) thus permitting the
greatest flexibility in data input. The form of the command is similar to that used in the Preliminary data.
UNITS
unitm
Parameters
UNITS
: keyword
unitnm
: name of unit to be utilised (see below)
Notes
1.
Force, length, temperature and angular unit may be specified. Only those terms which are required to be
modified need to be specified, undefined terms will default to those supplied on the global units definition
unless previously overwritten in the current data block. In the case of the angular unit, the default
depends on the data block concerned, see below.
2.
Valid unit names are as defined in Section 5.1.42.1.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-53
ASAS (Non-Linear) User Manual
3.
Structural Data
The mass unit is derived from the force and length unit currently defined. In order to determine the
consistent mass unit the force and length terms must both be either metric or imperial. Valid
combinations are shown in Table 3.1. This requirement is only necessary where mass or density data is
being specified, in other cases inconsistencies are permitted. See Note 4 below and Section 3.11.
4.
Applications for each data type
COOR
-
Coordinate data - only one UNITS command is permitted for each coordinate system defined and must appear immediately after the header
command. If different units are required, a new co-ordinate system must be
defined. The default angular unit is DEGREES.
ELEM
-
Element data - UNITS not applicable.
MATE
-
Material data - UNITS command may appear anywhere. Force and length
units must be within a consistent set.
GEOM
-
Geometric data - UNITS command may appear anywhere. Refer to data
definitions for individual element type for the default angular unit assumed.
SKEW and NSKW
-
Skew systems - UNITS not applicable.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-54
ASAS (Non-Linear) User Manual
Structural Data
Example
Data
Operational Units
Notes
SYSTEM DATA AREA 5000000
PROJECT ASAS
JOB STAT
EXAMPLESOLV 1.0
TITLE
*
OPTIONS GOON
UNITS KIPS FEET
END
Kips, feet, centigrade
Global definition
Kips, mm, centigrade,
Default angular
*
COOR
CART
UNITS MM
0.0
100.0
0.0
2
0.0
FIN
1
200.0
0.0
degs
CART FRED
UNITS M
101
0.1
0.1
0.0
102
END
0.1
0.2
0.0
Kips, m, centigrade,
Requires M as unit
degs
Therefore define
new coor system
*
ELEM
Units not used in
elem topology
*
MATP 1
BEAM 1
unit is degrees
for co-ordinates
2
1
BEAM 101 102 1
BEAM 2 102 2
END
MATE
1
Kips, feet, centigrade
4.32E06
0.3
0.0
global input
1.52E-02
Mass unit is
3.22 x 10 4 lbs
END
*
GEOM
1 BEAM
Units revert to
Kips, feet, centigrade
0.3
0.18
0.18
0.03
UNITS IN
2 BEAM 8.4
24.7
29.8
1.13
Kips, inch, centigrade
END
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-55
ASAS (Non-Linear) User Manual
5.2.2
Structural Data
COORDINATE Data
The coordinate data may comprise one or more local coordinate systems. Each of these systems must be headed
by a Coordinate System Header Line and all except the last terminated by a FIN keyword. The last system of
coordinate data is terminated by an END keyword.
COOR
CART
(name)
CYLI
SPHE
(units)
name
DCOS
x'x
ORIG
x-origin
node
x
RP
nrep
inode
x-inc
y-inc
z-inc
RRP
nrrep
iinode
x-inc
y-inc
z-inc
IMPE
ampl
x
y
z
x`y
x'z
y-origin
y
y'x
y'y
y'z
z-origin
z
SIN
hleng1
SIN
hleng2
COS
harno1
COS
harno2
FIN
END
Parameters
COOR
: compulsory header keyword to denote the start of the coordinate data
CART
: keywords to denote the start of each local coordinate system
CYLI
SPHE
IMPE
: keyword to denote imperfection data
FIN
: keyword to denote the end of each local coordinate system, except the last
END
: compulsory keyword to denote the end of the entire coordinate data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-56
ASAS (Non-Linear) User Manual
Structural Data
Notes
1.
The coordinate values are in the current local coordinate system or in the global system if no local system
has been defined.
2.
For cylindrical systems (CYLI) x,y,z are replaced by r, θ, z.
3.
For spherical systems (SPHE) x,y,z are replaced by r, θ, φ.
4.
For a detailed description of each parameter see Sections 5.2.2.1 to 5.2.2.4.
5.2.2.1 Local Coordinate System Header
To define the type of local coordinate system. Optional, if omitted CART is assumed.
(name)
CART
DEG
CYLI
SPHE
name
RAD
Parameters
CART
: cartesian system, global or local
CYLI
: cylindrical polar system
SHPE
: spherical polar system
name
: name of the coordinate system. Optional for CART and if blank, the global cartesian system is
assumed. Compulsory for CYLI and SPHE. (4 character alphanumeric, 1st character must be
alphabetic.)
DEG
: keyword used when the angular unit is degrees for θ and φ. If both DEG and RAD are omitted,
degrees are assumed.
RAD
: keyword used when the angular unit is radians.
Note
For an axisymmetric model the global axis system is the unnamed cartesian system with x and z equivalent to r
and z.
5.2.2.2 Local Coordinate System Orientation
One DCOS command and one ORIG command must be included for each cylindrical or spherical system, and
for each named cartesian system. Neither is needed for the global cartesian system with the name omitted.
These lines define the origin and direction of the local axis system.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-57
ASAS (Non-Linear) User Manual
DCOS
x’x
ORIG
x-origin
Structural Data
x’y
x’z
y-origin
y’x
y’y
y’z
z-origin
Parameters
DCOS
: keyword
x’x, x’y, x’z
: 6 directional cosines. See Section 5.2.7.1 for a full description. (Real)
y’x, y’y, y’z
ORIG
: keyword
x-origin
: 3 global coordinates of the origin of the local system. (Real)
y-origin
z-origin
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-58
ASAS (Non-Linear) User Manual
Structural Data
Coordinates for Cartesian Systems
x Distance from the local origin in the local x’ direction
y Distance from the local origin in the local y’ direction
z Distance from the local origin in the local z’ direction
Coordinates for Cylindrical Polar Systems
R Distance from the local origin in the local x’y’ plane.
θ Angle from the +ve side of the local x’ axis in the local
plane (+ve for right-hand screw rule applied to +ve
z
x’y’
local z’).
Distance from the local origin in the local z’ direction.
Coordinates for Spherical Polar Systems
R Distance from the local origin in 3-D.
θ Angle from the +ve side of the local x’ axis in the local x’y’
plane (+ve for right-hand screw rule applied to +ve local z’).
φ Angle from the +ve side of the local z’ axis to the radius,
measured in 3-D.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-59
ASAS (Non-Linear) User Manual
Structural Data
5.2.2.3 Node Coordinates
Parameters
node
: node number. (Integer, 1-999999)
x, y, z
: 3 coordinates for the node in a cartesian system. (Real)
r, θ, z
: 3 coordinates for the node in a cylindrical polar system
r, θ, φ
: 3 coordinates for the node in a spherical polar system
RP
: keyword to indicate data generation from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated. (Integer)
x-inc
: cartesian coordinate increments to be added each time the data is generated. (Real)
y-inc
z-inc
r-inc
: cylindrical coordinate increment to be added each time the data is generated. (Real)
θ-inc
z-inc
r-inc
: spherical coordinate increment to be added each time the data is generated. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-60
ASAS (Non-Linear) User Manual
Structural Data
θ-inc
φ-inc
RRP
: keyword to indicate data generation from the previous // symbol.
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated. (Integer)
Examples
Example of single coordinate data block using the global cartesian axis system.
COOR
CART
1
2
/
3
RP 4
/
7
RP 2
END
0.0
10.0
0.0
0.0
0.0
0.0
1
0.0
10.0
10.0
0.0
0.0
0.0
1
5.0
0.0
20.0
0.0
0.0
4.0
Example of a coordinate data block which uses several local axis systems beginning with the global cartesian
axis system.
COOR
****
CART
//
/
66
RP
RRP
69
73
FIN
****
CYLI
DCOS
ORIG
/
1
9
7
12
11
RP
FIN
****
CYLI
DCOS
ORIG
/
THE GLOBAL CARTESIAN SYSTEM, 8 NODES DEFINED
3,1
2,4
20.1
0.0
-10.0
20.0
11.0
0.0
4.0
0.0
0.0
0.0
-1.0
0.0
0.0
-1.0
0.0
A CYLINDRICAL SYSTEM, NAMED BWL2, 20 NODES DEFINED
BWL2
DEG
1.0
0.0
0.0
0.0
1.0
0.0
0.0
0.0
0.0
4,12
5.0
5.0
6.0
6.0
6.0
0.0
0.0
22.5
0.0
22.5
22.5
45.0
0.0
0.0
0.0
0.0
8.0
0.0
2ND CYLINDRICAL SYSTEM, NAMED HNDL, 7 NODES DEFINED
HNDL
DEG
1.0
0.0
0.0
0.0
-1.0
0.0
26.0
0.0
0.0
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-61
ASAS (Non-Linear) User Manual
85
RP
/
92
RP
/
93
RP
END
Structural Data
3,1
10.0
0.0
0.0
30.0
-1.0
0.0
2,-4
10.0
0.0
0.0
60.0
-5.0
0.0
9.5
0.0
0.0
60.0
-0.5
0.0
2,1
5.2.2.4 Coordinate Imperfection Data
Defines variations from the nodal coordinate values in the current local coordinate system.
Notes
1.
Up to 10 IMPE lines are allowed in each local coordinate system.
2.
All variation data is calculated for a node from the original local system coordinates and is then applied to
these coordinate values before any conversion to the global cartesian system.
3.
To input a variation depending on one direction only, use the COS parameter and hleng or harno value
of zero for the term corresponding to the direction of constant variation.
Cartesian Systems
Parameters
IMPE
: keyword to denote imperfection data
ampl
: amplitude of imperfection
X,Y,Z
: keywords to denote which coordinate direction is effected
SIN, COS
hlengx
hlengy
hlengz
:
keywords to denote a sine or cosine variation
: half-wavelength value for variation in corresponding coordinate direction
Variation data will be generated of the form:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-62
ASAS (Non-Linear) User Manual
Structural Data
Cylindrical Systems
IMPE
ampl
SIN
harno
SIN
hleng
COS
COS
Parameters
IMPE
: keyword to denote imperfection data
ampl
: amplitude of imperfection
SIN,COS : keywords to denote a sine or cosine variation
harno
: harmonic number of angular variation
hleng
: half wavelength value for variation in location z direction
Radial variation data will be generated of the form:
Spherical Systems
IMPE
ampl
SIN
harno1
COS
SIN
harno2
COS
Parameters
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-63
ASAS (Non-Linear) User Manual
IMPE
: keyword to denote imperfection data
ampl
: amplitude of imperfection
Structural Data
SIN,COS : keywords to describe a sine or cosine variation
harno1
: harmonic number of angular variation in θ direction
harno2
: harmonic number of angular variation in φ direction
Radial variation data will be generated of the form:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-64
ASAS (Non-Linear) User Manual
Structural Data
Example
Example of a coordinate data block which uses several local axis systems and imperfection data.
COOR
****
CART
//
/
66
RP
RRP
69
73
IMPE
FIN
****
CYLI
DCOS
ORIG
/
1
9
7
12
11
RP
IMPE
FIN
****
CYLI
DCOS
ORIG
/
85
RP
/
92
RP
/
93
RP
IMPE
END
5.2.3
THE GLOBAL CARTESIAN SYSTEM, 8 NODES DEFINED
3,1
2,4
20.1
0.0
-10.0
20.0
11.0
0.01 X COS
0.0
4.0
0.0
0.0
0.0
4.0
-1.0
0.0
0.0
-1.0
0.0
COS 0.0
A CYLINDRICAL SYSTEM, NAMED BWL2, 20 NODES DEFINED
BWL2
DEG
1.0
0.0
0.0
0.0
1.0
0.0
0.0
0.0
0.0
5.0
5.0
6.0
6.0
6.0
4,12
0.0
0.01 COS
0.0
22.5
0.0
22.5
22.5
45.0
4 COS
0.0
0.0
0.0
0.0
8.0
0.0
4.0
2ND CYLINDRICAL SYSTEM, NAMED HNDL, 7 NODES DEFINED
HNDL
DEG
1.0
0.0
0.0
0.0
-1.0
0.0
26.0
0.0
0.0
3,1
10.0
0.0
0.0
30.0
-1.0
0.0
2,-4
10.0
0.0
0.0
60.0
-5.0
0.0
2,1
0.01
9.5
0.0
-0.5
0.0
60.0
0.0
COS 6 COS 0.0
Element Topology Data
To define each element which makes up the structure.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-65
ASAS (Non-Linear) User Manual
Structural Data
ELEM
MATP
material
eltype
(mtype)
RP
nrep
inode
RRP
nrrep
iinode
//nodes//
geom
(elno)
END
Parameters
ELEM
: compulsory header keyword to denote the start of the element data.
MATP
: keyword to define the material to be assigned to all following elements until another MATP
line is used.
material
: material property integer. The material properties are defined in Section 5.2.4. (Integer,1-9999)
eltype
: element type. (Alphanumeric, 4 characters.) See Appendix -A for a full list of elements
available.
mtype
: type of mass matrix for this element (natural frequency analysis). For defaults, see Appendix A.
Permitted Values:
C - consistent mass
L - lumped mass
N - no mass
nodes
: list of node numbers to define the element. (Integer, 1-99999)
geom
: geometric property integer. (Integer, 1-9999.) Not required for certain element types, see
Appendix -A.
elno
: user number for the element. Every user element number, whether user defined or program
generated, must be unique. Generated elements are numbered successively in increments of 1.
If omitted the element numbers are assigned by the program, numbered according to the input
order of the elements, see Section 4.3.2. (Integer, 1-99999)
RP
: keyword to indicate the generation of data from the previous / symbol.
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment. (Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-66
ASAS (Non-Linear) User Manual
Structural Data
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment. (Integer)
END
: compulsory key word to denote the end of the element topology data.
Notes
1.
Continuation lines may be used if needed to define nodes, geom and elno.
2.
Where mid-side nodes are at the midpoint and their coordinates have not been defined in the COOR data,
the node number must be included in the nodes list.
Examples
An example of a simple element topology data block.
ELEM
MATP
1
FLA2
FLA2
8
9
9
10
1
2
FLA2
8
10
1
FLA2
END
10
11
1
An example of element topology data using data generation.
ELEM
MATP
/
1
FLA2
FLA2
1
1
21
41
3
2
FLA2
41
21
2
RP
END
10,1
An example of the use of element numbers and continuation lines.
BR15
:
:
5.2.4
1
2
3
4
5
6
21
41
23
42
25
43
44
45
46
130
Material Property Data
This data block defines the material models which will be used in the analysis. For each material required the
user should associate an integer number (the ‘material property integer’) which applies to all the properties of a
material and is used to cross-reference the material from other data blocks such as element topology. The types
of behaviour which may be associated with each material are:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-67
ASAS (Non-Linear) User Manual
Structural Data
•
Elastic, either isotropic, orthotropic, woven, anisotropic, hyperelastic or laminated (for shells)
(see Section 5.2.4.1).
•
Plastic, or more generally, time independent irreversible behaviour according to various
theories (see Section 5.2.4.2).
•
Creep or time dependent material behaviour (see Section 5.2.4.3).
•
Failure properties associated with limiting values for stresses and/or strains for laminated
composites (seeSection 5.2.4.4).
•
User defined material (see Section 5.2.4.1).
•
Material properties for general field analysis problems, eg electric conduction. (see Section
5.2.4.1)
•
Piezo-resistive material properties (see Section 5.2.4.1)
•
Convection and radiation models for heat analysis. (see Section 5.2.4.1)
A material may be defined by a combination of the above properties with the same integer identifier.
In general, all properties may be a function of temperature. This is specified by repeating material data at a
number of temperatures. The program interpolates linearly between these temperatures. The same temperatures
should be used for all material data types.
The material integer is unique to the problem and the same number cannot be used to reference different
materials in different groups.
Elasticity data must precede any plasticity data, which in turn must precede any creep data.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-68
ASAS (Non-Linear) User Manual
Structural Data
Parameters
MATE
: compulsory header keyword to denote the start of the material properties data
mat
: material property integer used to label different materials. (Integer, 1-9999)
ISO
: keyword to define an isotropic material
ORTH
: keyword to define an orthotropic material
WOVE
: keyword to define a woven material
AISO
: keyword to define an anisotropic material
AISI
: keyword to define an anisotropic material by specifying the inverse of the stress-strain relations
i.e. strain-stress relations
HYPE
: keyword to define a hyperelastic material. (Continuum elements only)
LAMI
: keyword to define a laminated material. (Shell and laminated brick elements only)
UMAT
: keyword to define a user supplied material
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-69
ASAS (Non-Linear) User Manual
Structural Data
FIEL
: keyword to define general field properties
PIER
: keyword to define piezo-resistive material properties
CVEC
: keyword to define heat convection properties
RADI
: keyword to define heat radiation properties
PLAS
: keyword to define plastic material properties
CREP
: keyword to define creep material properties
FAIL
: keyword to define failure data for orthotropic and laminated materials only
END
: compulsory keyword to denote the end of the material properties data block
Notes
1.
For full details for each type of material see Sections 5.2.4.1, 5.2.4.2, 5.2.4.3, 5.2.4.4 and Appendix -B.
2.
Every material referenced in the element topology data must be fully defined in this data block.
3.
PLAS not available with AISO, AISI, ORTH, WOVE or HYPE materials.
4.
FAIL only available with ISO, AISO, ORTH, WOVE and LAMI materials.
5.2.4.1 Elastic Material Properties
To define the properties for isotropic and anisotropic elastic material.
5.2.4.1.1
Isotropic material properties
mat
ISO
elas
pois
(expan)
(dens)
(dampm)
pois
expan
dens
dampm
(dampk) (temp)
kn
:
(ISO)
elas
dampk
temp
Parameters
mat
: material property integer. (Integer, 1-9999)
ISO
: keyword to define the material as isotropic
elas
: modulus of elasticity. (Real)
poisson
: Poisson’s ratio. (Real, 0.0 <poisson< 0.5)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-70
ASAS (Non-Linear) User Manual
Structural Data
expan
: linear coefficient of thermal expansion. (Real)
dens
: density, mass per unit volume. (Real)
dampm
: damping factor for mass. (Real)
dampk
: damping factor for elastic stiffness. (Real)
temp
: temperature at which these properties apply. (Real)
kn
: effective contact stiffness for gap elements and normal contact stiffness parameter for rigid
surface elements. (Real)
Notes
1.
The expansion coefficient is optional and is only required if temperatures are to be included in any of the
loading applied to the structure.
2.
The density is optional and is only required if acceleration or centrifugal loads are to be included in any
loading applied to the structure, or if a natural frequency or transient dynamics analysis is to be
performed.
3.
The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
analysis.
4.
The temperature is optional and is only required if the material properties vary with temperature and
temperature loading is applied to the structure.
5.
If an optional value is specified, all preceding optional values must also be specified.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-71
ASAS (Non-Linear) User Manual
Structural Data
Examples
A simple example with one material and no temperature or inertia type loading.
MATE
1
ISO
21.0E4
0.3
END
An example with several materials including the expansion coefficient and the density.
MATE
10
ISO
0.298E8
0.3
0.1182E-4
0.283
20
30
ISO
ISO
0.312E8
0.151E8
0.31
0.3
0.1212E-4
0.1566E-4
0.298
0.206
END
An example with one material which is temperature dependent but with no inertia type loading
MATE
1
ISO
7.200E10
0.3
16.32E-6
0.0
0.0
0.0
0.0
:
7.200E10
0.3
16.32E-6
0.0
0.0
0.0
70.0
:
:
7.098E10
7.047E10
0.3
0.3
18.26E-6
18.16E-6
0.0
0.0
0.0
0.0
0.0
0.0
100.0
200.0
:
:
6.895E10
6.767E10
0.3
0.3
18.92E-6
19.60E-6
0.0
0.0
0.0
0.0
0.0
0.0
300.0
400.0
:
:
6.640E10
6.462E10
0.3
0.3
20.20E-6
20.76E-6
0.0
0.0
0.0
0.0
0.0
0.0
500.0
600.0
END
5.2.4.1.2
Orthotropic material properties
Parameters
mat
: material property integer. (Integer, 1-9999)
skew
: optional skew system identifier, see Section 5.2.7. (Integer)
ORTH
: keyword to define the material as orthotropic
density
: density, mass per unit volume. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-72
ASAS (Non-Linear) User Manual
Structural Data
dampm
: damping factor for mass. (Real)
dampk
: damping factor for elastic stiffness. (Real)
temp
: temperature at which these properties apply. (Real)
E11-E33
: Young’s moduli in local 1, 2 and 3 directions respectively. (Real)
(The program will set E33=E22 if E33 is specified as zero.)
G12-G31
: shear moduli in local 12, 23 and 31 planes respectively. (Real)
ν12-ν13
: Poisson’s ratios in local 12, 23 and 13 planes respectively. (Real)
(The program will set ν23= ν12 and/or
ν13= ν12 if any of these is specified as zero.)
α11-α33
: coefficients of thermal expansion in the local 1, 2 and 3 directions respectively. (Real)
fl
: loss factor, i.e. volume fraction of material with no stiffness. If not specified, fl = 0.0. (Real)
Notes
1.
The density is optional and is only required if acceleration or centrifugal loads are to be included in any
loading applied to the structure, or if a natural frequency or transient dynamics analysis is being
performed.
2.
The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
analysis.
3.
The orthotropic properties must start on the first continuation line and may then spread onto further
continuation lines as required.
4.
The temperature is optional and is only required if the material properties vary with temperature and
temperature loading is applied to the structure.
5.
If an optional value is specified, all preceding optional values must also be specified.
6.
Up to 13 properties are expected but if less than 13 are specified, then the remaining properties default to
zero.
7.
The Poisson’s ratios ν21, ν32 and ν31 are determined inside the program from
ν 21 = ν12
E 22
E 11
ν32 = ν 23
E33
E 22
ν31 = ν13
E33
E 11
Examples
An example of an orthotropic material for a QUM8 element.
MATE
1
:
ORTH
7.8E6
2.6E6
0.0
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-73
ASAS (Non-Linear) User Manual
:
:
1.3E6
0.25
0.0
0.0
Structural Data
0.0
0.0
END
An example of an orthotropic material with temperature dependency for a QUX8 element.
MATE
1
ORTH
0.0
0.0
2.1E6
0.0
3.4E5
20.0
:
4.3E6
8.8E5
:
1
0.13E-5 0.23E-5 -0.12E-6
ORTH 0.0 0.0 0.0 80.0
:
:
4.3E6 1.8E6 3.2E5 4.4E5
0.17E-5 0.25E-5 -0.12E-6
0.0
0.0
0.25
0.13
0.0
0.0
0.0
0.21
0.17
0.0
END
5.2.4.1.3
Woven material properties
Parameters
mat
: material property integer. (Integer, 1-9999)
skew
: optional skew system identifier, see Section 5.2.7. (Integer)
WOVE
: keyword to define the material as woven
density
: density, mass per unit volume. (Real)
dampm
: damping factor for mass. (Real)
dampk
: damping factor for elastic stiffness. (Real)
temp
: temperature at which these properties apply. (Real)
E11-E33
: Young’s moduli in local 1, 2 and 3 directions respectively of the orthotropic sub-lamina. (Real)
(The program will set E33=E22 if E33 is specified as zero.)
G12-G31
: shear moduli in local 12, 23 and 31 planes respectively of the orthotropic sub-lamina. (Real)
ν12-ν13
: Poisson’s ratios in local 12, 23 and 13 planes respectively of the orthotropic sub-lamina. (Real)
(The program will set ν23= ν12 and/or
ν13= ν12 if any of these is specified as zero.)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-74
ASAS (Non-Linear) User Manual
Structural Data
α11-α33
: coefficients of thermal expansion in the local 1, 2 and 3 directions respectively. (Real)
fl
: loss factor, i.e. volume fraction of material with no stiffness. If not specified, fl = 0.0. (Real)
Notes
1.
The density is optional and is only required if acceleration or centrifugal loads are to be included in any
loading applied to the structure, or if a natural frequency or transient dynamics analysis is being
performed.
2.
The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
analysis.
3.
The woven properties must start on the first continuation line and may then spread onto further
continuation lines as required.
4.
The temperature is optional and is only required if the material properties vary with temperature and
temperature loading is applied to the structure.
5.
If an optional value is specified, all preceding optional values must also be specified.
6.
Up to 13 properties are expected but if less than 13 are specified, then the remaining properties default to
zero.
7.
The Poisson’s ratios ν21, ν32 and ν31 are determined inside the program from
ν 21 = ν12
E 22
E 11
ν32 = ν 23
E33
E 22
ν31 = ν13
E33
E 11
Examples
An example of an orthotropic material for a TCS8 element with loss factor 0.2.
MATE
1
WOVE
:
:
150E9
5.7E9
10E9
3.4E9
0.0
5.7E9
:
0.25
0.0
0.0
0.25E-5
0.0
:
0.17E-5
END
5.2.4.1.4
0.2
Anisotropic material properties
There are two options available to anisotropic behaviour. The first specifies the matrix C in relation σ=Cε (in
which σ is stress and ε strain). The second specifies the inverse of C to give strains as a function of stress.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-75
ASAS (Non-Linear) User Manual
Structural Data
AISO
mat
(density)
(skew )
(dampm)
(dampk)
(temp)
AISI
:
properties
Parameters
mat
: material property integer. (Integer, 1-9999)
skew
: optional skew system identifier, see Section 5.2.7. (Integer)
AISO
: keyword to define the material as anisotropic with properties defining the stress-strain relations
AISI
: keyword to define the material as anisotropic with properties defining the strain-stress relations
density
: density, mass per unit volume. (Real)
dampm
: damping factor for mass. (Real)
dampk
: damping factor for mass. (Real)
temp
: temperature at which these properties apply
properties
: coefficients of the anisotropic stress-strain matrix (AISO) or the strain-stress matrix (AISI) and
linear coefficients of expansion. See Appendix -A for a full definition of which terms are
required for each type of element. (Real)
Notes
1.
The density is optional and is only required if acceleration or centrifugal loads are to be included in any
loading applied to the structure, or if a natural frequency or transient dynamics analysis is being
performed.
2.
The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
analysis.
3.
The anisotropic properties must start on the first continuation line and may then spread onto further
continuation lines as required.
4.
A total of 30 properties is always needed, composed of up to 24 material constants and 6 coefficients of
thermal expansion. The coefficients of thermal expansion must start at position 25.
5.
If an optional value is specified, all preceding optional values must also be specified.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-76
ASAS (Non-Linear) User Manual
Structural Data
Examples
An example of an anisotropic material for a BR20 element.
MATE
1
AISI
:
0.536044 -0.16081 0.536044 -0.16081 -016081
:
0.0
0.0
0.0
0.139372 0.0
:
0.0
0.0
0.139372 0.0
0.0
:
0.0
0.0
0.139372 0.00172 0.00172
:
0.0
0.0
0.0
0.0
0.0
END
0.536044
0.0
0.0
0.00172
0.0
An example of an anisotropic material for a QUM8 element
MATE
1
AISO
:
23600.0 5720.0 20575.0
0.0
0.0 16750.0
:
0.0
0.0
0.0 12650.0
0.0
0.0
:
0.0
0.0
0.0
0.0
0.0
0.0
:
0.0
0.0
0.0 0.16E-4 0.14E-4
0.01E-4
:
0.0
0.0
0.0
0.0
0.0
0.0
END
5.2.4.1.5
Hyper-elastic material properties
mat
:
HYPE
bulk
con1
con2
(expan)
(dens)
(dampm)
(dampk)
(HYPE)
bulk
con1
con2
expan
dens
dampm
dampk
(temp)
temp
Parameters
mat
: material property integer. (Integer, 1-9999)
HYPE
: keyword to define the material as hyper-elastic
bulk
: bulk modulus. (Real)
con1
: Mooney-Rivlin constant, C10. (Real)
con2
: Mooney-Rivlin constant, C01. (Real)
expan
: linear coefficient of thermal expansion. (Real)
dens
: density, mass per unit volume. (Real)
dampm
: damping factor for mass. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-77
ASAS (Non-Linear) User Manual
Structural Data
dampk
: damping factor for stiffness. (Real)
temp
: temperature at which these properties apply. (Real)
Notes
1.
The damping factor for stiffness is currently restricted to be zero.
2.
The expansion coefficient is optional and is only required if temperatures are to be included in any of the
loading applied to the structure.
3.
The density is optional and is only required if acceleration or centrifugal loads are to be included in any
loading applied to the structure, or if a natural frequency analysis is to be performed.
4.
The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
analysis.
5.
The temperature is optional and is only required if the material properties vary with temperature and
temperature loading is applied to the structure.
6.
If an optional value is specified, all preceding optional values must also be specified.
Example
A simple example with one material and no temperature or inertia type loading.
MATE
1
HYPE
1.0E4
80.0
20.0
END
5.2.4.1.6
mat
Laminated Material Properties
(skew)
LAMI
(density)
(dampm)
(dampk)
(temp)
Parameters
mat
: material property integer. (Integer, 1-9999)
skew
: optional skew system identifier, see Section 5.2.7. (Integer)
LAMI
: keyword to define the material as a laminated shell
density
: density, mass per unit volume. (Real)
dampm
: damping factor for mass. (Real)
dampk
: damping factor for stiffness. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-78
ASAS (Non-Linear) User Manual
temp
Structural Data
: temperature at which these properties apply. (Real)
Notes
1.
The skew system identifier is optional and is only required if the laminate material reference axis system
does not coincide with the global axis system.
2.
The density is optional and is only required if acceleration or centrifugal loads are to be included in any
loading applied to the structure, or if a natural frequency or transient dynamics analysis is being
performed. If the density is specified both here and with the materials forming the laminate, the density
specified here will be used. If the density is omitted (or given a value of 0.0) the density for the laminate
will be calculated from the laminae densities in the manner described in Appendix -B.
3.
The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
analysis. If damping factors are specified both here and with the materials forming the laminate, the
factors specified here will be used. If the damping factors are omitted (or given a value of 0.0) the
damping factors for the laminate will be calculated from the laminae damping factors in the manner
described in Appendix -B.
4.
The temperature is optional and is only required if the material properties vary with temperature and
temperature loading is applied to the structure. If the properties specified here are temperature dependent
then the materials forming the laminate must be specified with the same range of temperatures.
5.
If an optional value is specified, all preceding optional values must be specified.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-79
ASAS (Non-Linear) User Manual
Structural Data
Example
A simple example of a laminated material where the material axes coincide with the global axis system (no skew
required), where the density is to be calculated from the laminae densities but where the damping factors for the
laminate are specified.
MATE
1 LAMI 0.0 0.039 0.0102
END
5.2.4.1.7
mat
:
User Material Properties
UMAT
(density)
(dampm)
(dampk)
up to 24 user material properties
(temp)
up to 6 thermal coefficients
Parameters
mat
: material property integer. (Integer, 1-9999)
UMAT
: keyword
density
: density, mass per unit volume. (Real)
dampm
: damping factor for mass. (Real)
dampk
: damping factor for stiffness. (Real)
temp
: temperature at which these properties apply. (Real)
Notes
1.
If thermal coefficients are supplied they must start at the 25th position as for AISO material properties.
2.
See Appendix B.6 for details concerning the user material interface.
3.
The density is optional and is only required if acceleration or centrifugal loads are to be included in any
loading applied to the structure, or if a natural frequency analysis is to be performed.
4.
The damping factors, dampm and dampk, are optional and are only required for a transient dynamics
analysis.
5.
The temperature is optional and is only required if the material properties vary with temperature and
temperature loading is applied to the structure.
6.
If an optional value is specified, all preceding optional values must also be specified.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-80
ASAS (Non-Linear) User Manual
5.2.4.1.8
Structural Data
Field Material Properties
mat
(skew )
:
FIEL
kxx
(kyy)
(kzz )
(kxy)
(k yz)
(kzx)
(dens)
(temp)
(FIEL)
kxx
kyy
kzz
kxy
kyz
kzx
dens
temp
Parameters
mat
: material property integer. (Integer, 1-9999)
skew
: skew system integer
FIEL
: keyword to define the material as field
kxx,kyy,kyy
: conductivities in xx direction, yy direction, etc. (Real)
kxy,kyz,kzx
dens
: generalised density. (Real)
temp
: temperature at which these properties apply. (Real)
Notes
1.
If only kxx is specified, it is assumed that the material is isotropic
(ie kxx = kyy = kzz and kxy = kyz = kzx = 0)
2.
If an optional value is specified, all preceding optional values must also be specified.
3.
For heat analysis, the generalised density is defined as the product of the specific heat capacity and the
density.
5.2.4.1.9
Piezo-resistivity Material Properties
mat
:
(skew)
q
n
PIER
µn
(dum)
p
µp
(dum)
π11
(dum)
π12
(temp)
π44
Parameters
mat
: material property integer. (Integer, 1-9999)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-81
ASAS (Non-Linear) User Manual
Structural Data
skew
: skew system integer. (Integer, 1-9999)
PIER
: keyword to define material as piezo-resistivity
dum
: dummy
temp
: temperature at which these properties apply. (Real)
q
: unit charge
n
: carrier concentration (n)
µn
: carrier mobility (n)
p
: carrier concentration (p)
µp
: carrier mobility (p)
π11
: Piezo-resistance coefficient, 11
π12
: Piezo-resistance coefficient, 12
π44
: Piezo-resistance coefficient, 44
Notes
1.
A total of 8 properties are always needed.
2.
If an optional value is specified, all preceding optional values must also be specified.
3.
The piezo-resistivity properties must start on the first continuation line and may then spread onto further
continuation lines as required.
5.2.4.1.10 Convective Heat Material Properties
mat
CVEC
h
r
:
(CVEC)
h
r
(temp)
temp
Parameters
mat
: material property integer. (integer, 1 - 9999)
CVEC
: keyword to define the material as convective heat
h
: film coefficient in the heat transfer equation. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-82
ASAS (Non-Linear) User Manual
r
: power index in the heat transfer equation. (Real)
temp
: temperature at which the properties apply. (Real)
Structural Data
Notes
1.
This material type is used to model convective heat transfer of the form:
q=h.(T1-T2)r
2.
CVEC material can only be used with FAT2 element in a heat analysis
5.2.4.1.11 Radiant Heat Material Properties
Parameters
mat
: material property integer. (integer, 1 - 9999)
RADI
: keyword to define the material as radiant heat
σ
: Stefan-Boltzmann constant (Real)
ε
: effective surface emissivity. (Real)
temp
: temperature at which the properties apply. (Real)
Notes
1.
This material type is used to model radiant heat transfer of the form:
q=σ.ε.(Τ14-Τ24)
2.
The temperatures required in the radiation equation are relative to absolute zero temperature. The default
temperature units assumed by ASAS(NL) are degrees Centigrade. If other temperature units are used for
an analysis, the correct absolute zero temperature in the appropriate units must be specified using the
PARA TAZERO command.
3.
RADI material can only be used with FAT2 element in a heat analysis.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-83
ASAS (Non-Linear) User Manual
Structural Data
5.2.4.2 Plastic Material Properties
To define the properties for a plastic material. Plastic material properties must be preceded by the elastic
isotropic material properties for any individual material integer.
A number of different plasticity models are available which are activated by 4-character directives defined on the
first line together with other basic data. Depending on the directives, so additional types of commands may also
be necessary. The directives fall into three categories:
(1)
Yield Criteria
MISE
-
Mises yield criterion to be used
TRES
-
Tresca yield criterion to be used
MOHR
-
Mohr-Coulomb yield criterion to be used
DRUC
-
Drucker-Prager yield criterion to be used
TCUT
-
Tension cutcriterion to be used
COUL
-
Coulomb friction yield criterion to be used (rigid surface elements only)
IVAN
-
Ivanov (gross section) yield criterion to be used (shell elements only)
BEM2
-
Beam stress resultant (gross section) yield criterion to be used (BM2D element only)
BEM3
-
Beam stress resultant (gross section) yield criterion to be used
(BEAM/BM3D/TUBE elements only)
BEAM
-
Generalised beam stress resultant (gross section) yield criterion to be used
(BEAM/BM3D/TUBE elements only)
SPRG
-
Inelastic model for spring elements
If no directive is given, then MISE’s criterion is assumed.
(2)
Post-Yield Behaviour
TABL
-
Tabular definition of uniaxial post-yield behaviour to be used.
If this directive is not given bi-linear behaviour is assumed.
(3)
Hardening Rule
PPRA
-
Prager type of kinematic hardening (see Note 2)
PZIG
-
Ziegler type of kinematic hardening
If no directive is given isotropic hardening is assumed.
Notes
1.
Associative flow rules are used in all cases.
2.
Prager type kinematic hardening is inapplicable to elements using a reduced stress space - i.e. plane stress
membranes, beams and shells.
3.
Temperature loads cannot be used in conjunction with IVANOV yield criterion.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-84
ASAS (Non-Linear) User Manual
4.
Structural Data
Kinematic hardening is only available for MISE and TRES criteria
(MISE)
(mat)
sigy
PLAS
(ep)
(temp)
TRES
PPRA
sigy
TCUT
ep
hard
(temp)
PZIG
:
sigy
ep
(hard)
temp
MOHR
(mat)
PLAS
c
phi
(temp)
mu
shrlmt
DRUC
(mat)
PLAS
COUL
kt
(mat)
PLAS
IVAN
sigy
(mat)
PLAS
BEM2
Po
Mpz
(temp)
BEM3
Po
M pz
M py
(temp)
BEAM
Po
Mpz
Mpy
(temp)
(mat)
PLAS
:
C1
(C2)
(C3)
(C4)
(C5)
(C6)
(MISE)
(mat)
PLAS
TABL
sigy
(temp)
TRES
PPRA
sigy
TCUT
hard
(temp)
PZIG
:
(mat)
properties
PLAS
SPRG
K1
K2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-85
ASAS (Non-Linear) User Manual
Structural Data
Parameters
mat
: property integer. (Integer, 1-9999)
PLAS
: keyword to define the material as plastic
MISE
: yield criterion keyword
TRES
: yield criterion keyword
TCUT
: yield criterion keyword
sigy
: uni-axial yield stress. (Real)
ep
: slope of post yield stress/strain relation. (Real)
temp
: temperature at which these properties apply. (Real)
PPRA
: kinematic hardening keyword
PZIG
: kinematic hardening keyword
hard
: for keywords PPRA and PZIG, the ratio of isotropic to kinematic hardening. 1.0 for isotropic
hardening, 0.0 for pure kinematic hardening. (Real)
MOHR
: yield criterion keyword
DRUC
: yield criterion keyword
c
: cohesion
phi
: angle of friction
COUL
: yield criterion keyword
kt
: tangential contact stiffness parameter (unit: stress per unit length). (Real)
mu
: coefficient of friction. (Real)
shrlmt
: limiting shear stress. (Real)
IVAN
: yield criterion keyword
BEM2
: yield criterion keyword
Po
: yield force. (Real)
Mpz
: yield moment about beam local z axis. (Real)
BEM3
: yield criterion keyword
Mpy
: yield moment about beam local y axis. (Real)
BEAM
: yield criterion keyword
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-86
ASAS (Non-Linear) User Manual
C1 - C6
: yield function constants in the equation:
C1(P/Po)C2 + C3(Mz/Mpz)C4 + C5(My/Mpy)C6 = 1 (Real)
SPRG
: inelastic spring model keyword
K1
: unloading stiffness factor (Real)
Structural Data
(set to 1.0 if zero specified)
K2
: kinematic hardening factor (Real)
TABL
: keyword required if a tabular definition of the uni-axial post yield behaviour is to be specified
properties
: if TABL is specified, properties will consist of pairs of stress/strain values defining the
uniaxial post yield behaviour. The strains required are total strains. (Real)
Notes
1.
All elastic material property data must appear before the plastic material property data for any individual
material integer.
2.
For details of the various models, see Appendix B.3.
3.
The slope of the post yield stress/strain curve must be less than the elastic modulus. Apart from tension
cutmaterial, the slope must be non negative (i.e. ≥0.0). For tension cutmaterial, the slope must not be less
than -E/ν
4.
If the material properties vary with temperature, each set of data should be repeated for a different
temperature.
5.
The following notes apply to tabulated definition only:
(a)
The stress-strain table may be continued on as many lines as necessary.
(b)
For linear elastic/plastic material the first point in the table (σ,ε) will correspond to a point after yield.
The coordinates of the yield point are computed from the elastic modulus and yield stress.
(c)
The program interpolates linearly for intermediate points.
(d)
There are a maximum of 40 different strain values allowed.
(e)
A slope defined in the table should not be equal to the elastic modulus. Apart from tension cutmaterial
the slope must be non negative (i.e. ≥ 0.0) For tension cutmaterial, the slope must not be less than -E/ν.
(f)
If curves are specified for different temperatures (see third example) then the order the plasticity data is
presented should correspond to the order in which the elastic data is presented.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-87
ASAS (Non-Linear) User Manual
Structural Data
Examples
Simple elastic-perfectly plastic model with isotropic hardening.
MATE
1
PLAS
END
ISO
21000.0
MISE
0.3
250.0
Simple elastic-plastic model with isotropic hardening.
MATE
1
ISO
21000.0
PLAS MISE
250.0
0.3
30.0
END
Metal satisfying MISE’s yield criterion and associated flow rule with isotropic hardening. Uniaxial behaviour is
as in figure below.
MATE
10
ISO
20900.0
20500.0
21900.0
0.3
0.3
0.3
0.276E-6
0.276E-6
0.276E-6
0.0
0.0
PLAS
:
MISE
TABL
σy1
T1
σ11
ε11
σ12
ε12
:
PLAS
σ14
ε14
σ15
ε15
MISE
TABL
σy2
T2
:
σ21
PLAS
:
MISE
σ31
ε21
σ22
22
TABL
σy3
T3
ε31
σ32
ε32
0.0
T1
T2
T3
σ13
σ23
σ33
ε13
ε23
ε33
END
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-88
ASAS (Non-Linear) User Manual
Structural Data
5.2.4.3 Creep Material Properties
To define the properties for a material with creep. Creep material properties must be preceded by elastic
isotropic material properties and plastic material properties if present.
This data defines the creep law to be used for each material type. The user may choose from 4 in-built laws.
Alternatively up to 5 user supplied laws (in subroutine form) can be used. Appendix B.4 gives full details. Inbuilt laws require creep constants which are given in the data. Creep constants for use with the user supplied
laws may be defined if required.
(mat)
:
CREP
constants
NORT
LAW2
LAW3
LAW4
USE1
USE2
USE3
USE4
USE5
(temp)
Parameters
mat
: material property integer. (Integer, 1-9999)
CREP
: keyword to define the material properties for creep
NORT
LAW2
LAW3
LAW4
USE1
USE2
USE3
USE4
temp
: keyword to define ASAS-NL creep law
: keyword to define user supplied creep law
: temperature at which these properties apply. (Real)
constants : creep law constants. (Real)
Note
Refer to creep law expressions in Appendix B.4 for definition of creep constants.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-89
ASAS (Non-Linear) User Manual
Structural Data
Examples
Norton (power) law for a Cr-Mo-V ferritic stainless steel. No temperature or time dependence.
Units: N, mm.
εc = 2.05 x 10-28 σ 10.42
MATE
1
ISO
1.41E5
CREP NORT
: 2.05E-28
0.3
10.42
0.0
END
Norton (power) law with temperature dependence but no time dependence. Units: N, mm, °C.
εc = 2.05 x 10-28 σ 10.42
T=525°C
εc = 6.72 x 10-28 σ 10.42
T=550°C
εc = 2.05 x 10-27 σ 10.42
T=575°C
MATE
1 ISO
1.41E5
0.3
16.0E-6
7.93E-9
0.0
0.0
525.0
:
:
1.36E5
1.31E5
0.3
0.3
16.0E-6
16.0E-6
7.93E-9
7.93E-9
0.0
0.0
0.0
0.0
550.0
575.0
CREP
:
NORT 525.0
2.05E-28 10.42
CREP
NORT
:
CREP
6.72E-28 10.42
NORT 575.0
0.0
:
END
2.05E-27
0.0
0.0
550.0
10.42
Creep law 2 which represents primary/secondary creep or secondary/tertiary creep. Note that the creep law is
implicitly temperature dependent. Further versatility is available by allowing the coefficients to vary with
temperature as illustrated in the example above. This example is for a Cr-Mo-V ferritic stainless steel for a
temperature range of approximately 565° ± 50°, Units: N, mm, seconds and °C.
εc = 7.46 x 10-5 σ 5.4 e-3.116 x10 /T + 9.69 x 10-16 σ 5.4 t1.364 e-3.116 x10 /T
4
4
MATE
1
ISO
1.31E5
CREP LAW2
: 7.46E-5
: 9.69E-16
END
0.3
16.0E-6
7.9E-9
5.4
0.0
3.11E4
5.4
1.364
3.116E4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-90
ASAS (Non-Linear) User Manual
Structural Data
Blackburn law for 316 stainless steel. Note that no numerical creep data is required and that the units assumed
by ASAS-NL are N, mm, seconds and °C.
MATE
1
:
ISO
1.53E5
1.48E5
0.3
0.3
14.0E-6
14.0E-6
7.93E-9
7.93E-9
0.0
0.0
0.0
0.0
450.0
537.0
:
:
1.43E5
1.38E5
0.3
0.3
14.0E-6
14.0E-6
7.93E-9
7.93E-9
0.0
0.0
0.0
0.0
580.0
593.0
:
1.33E5
0.3
14.0E-6
7.93E-9
0.0
0.0
648.0
:
1.28E5
CREP LAW4
0.3
14.0E-6
7.93E-9
0.0
0.0
700.0
END
5.2.4.4 Failure Material Properties
To define the failure (limiting) values for lamina stresses and strains and laminate stress/strain resultants.
(mat)
:
FAIL
FLW1
FLW2
FLW3
FLW4
FLW5
(temp)
up to 14 failure v alues
Parameters
mat
: material property integer. (Integer, 1-9999)
FAIL
: keyword to define the properties as failure values
FLW1
FLW2
FLW3
FLW4
FLW5
temp
: keyword to define failure law type
: temperature at which these properties apply. (Real)
Notes
1.
FLW1 and FLW2 are in-built lamina failure laws.
Appendix B.5.3 for further details.
FLW3 to FLW5 are user-defined laws.
2.
The actual failure values required depend upon whether lamina or laminate values are being defined (see
following sections).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
See
Page 5-91
ASAS (Non-Linear) User Manual
5.2.4.4.1
Structural Data
Lamina Failure Values
The following data input is required for an elastic laminated composite.
Parameters
mat
: material property integer. (Integer, 1-9999)
FAIL
: keyword to define the properties as failure values
temp
: temperature at which these properties apply. (Real)
xt, xc
: limiting direct tensile and compressive stresses respectively in fibre direction. (Real)
yt, yc
: limiting direct tensile and compressive stresses respectively normal to fibre in direction 2. (Real)
zt, zc
: limiting direct tensile and compressive stresses respectively normal to fibre in direction 3. (Real)
s12
: limiting shear stress of lamina in 1-2 plane. (Real)
s23
: limiting shear stress of lamina in 2-3 plane. (Real)
s31
: limiting shear stress of lamina in 3-1 plane. (Real)
zl
: limiting interlaminar tensile stress. (Real)
sl
: limiting interlaminar shear stress. (Real)
ε1t, ε1c : limiting direct tensile and compressive strains respectively in fibre direction. (Real)
ε2t, ε2c : limiting direct tensile and compressive strains respectively normal to fibre in direction 2. (Real)
ε3t, ε3c : limiting direct tensile and compressive strains respectively normal to fibre in direction 3. (Real)
γ12
: limiting shear strain of lamina in 1-2 plane. (Real)
γ23
: limiting shear strain of lamina in 2-3 plane. (Real)
γ31
: limiting shear strain of lamina in 3-1 plane. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-92
ASAS (Non-Linear) User Manual
Structural Data
Notes
1.
Up to 20 failure values are expected but if less are specified then the remaining values default to zero.
2.
If a failure value is set (or defaults) to zero, the relevant term in the failure criterion is ignored.
3.
Isotropic, orthotropic or anisotropic failure material properties must be preceded by material properties.
4.
Using the above data, a number of lamina failure criteria are evaluated in POSTNL when options FEMVLAMI are selected. See Appendix B.5.1 for further details.
5.2.4.4.2
Plastic Lamina Failure FLW1 Values
The following data input is required for a ‘plastic’ laminated composite i.e. when an element referencing this
material belongs to a group of elements with directive PLAS.
Parameters
mat
: material property integer. (Integer, 1-9999)
FAIL
: keyword to define the properties as failure values
FLW1
: keyword to denote that the in-built failure law type 1 is to be used. See Appendix B.5.3.1 for
details
ftype
: failure criterion for matrix failure. Valid keywords are:
TSWU
-
Tsai-Wu (default)
TSAI
-
Azzi-Tsai
HOFF
-
Hoffman
NORR
-
Norris
MISE
-
von Mises
MXCS
-
maximum stress
temp
: temperature at which these properties apply. (Real)
xt, xc
: limiting direct tensile and compressive stresses respectively in fibre direction. (Real)
yt, yc
: limiting direct tensile and compressive stresses respectively normal to fibre in direction 2. (Real)
zt, zc
: limiting direct tensile and compressive stresses respectively normal to fibre in direction 3. (Real)
s12
: limiting shear stress of lamina in 1-2 plane. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-93
ASAS (Non-Linear) User Manual
Structural Data
s23
: limiting shear stress of lamina in 2-3 plane. (Real)
s31
: limiting shear stress of lamina in 3-1 plane. (Real)
zl
: limiting interlaminar tensile stress. (Real)
sl
: limiting interlaminar shear stress. (Real)
βE
: dimensionless material parameter
0≤
β E defining the reduction in fibre stiffness after matrix failure.
β E ≤ 1.0. A value of β E=0.0 means no reduction in fibre stiffness, a value of 1.0 means a
complete loss of fibre stiffness. (Real)
β2
: dimensionless material parameter β2 defining the reduction in fibre stiffness after fibre failure. (0
≤
β 2 ≤ 1.0). By default, β 2=0.0 and this means that the matrix stiffness is assumed after fibre
failure. For
β 2 •0.0, the fibre stiffness after failure is (1- β 2) times its value before failure.
Notes
1.
Up to 13 failure values are expected but if less are specified then the remaining values default to zero.
2.
If the failure law type is left blank, the failure data will have the same meaning as for an elastic laminated
composite. When analysis beyond first ply failure is required, FLW1 will be assumed with
β E= β 2=0.0.
3.
If a failure value is set (or defaults) to zero, the relevant term in the failure criterion is ignored.
5.2.4.4.3
Plastic Lamina Failure FLW2 Values
The following data input is required for a ‘plastic’ laminated composite, i.e. when an element referencing this
material belongs to a group of elements with directive PLAS.
Parameters
mat
: material property integer. (Integer, 1-9999)
FAIL
: keyword to define the properties as failure values
FLW2
: keyword to denote that the in-built failure law type 2 is to be used. See Appendix B.5.3.1 for details
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-94
ASAS (Non-Linear) User Manual
ftype
Structural Data
: failure criterion for matrix failure. Valid keywords are:
TSWU
-
Tsai-Wu (default)
TSAI
-
Azzi-Tsai
HOFF
-
Hoffman
NORR
-
Norris
MISE
-
von Mises
MXCS
-
maximum stress
temp
: temperature at which these properties apply. (Real)
xt, xc
: limiting direct tensile and compressive stresses respectively in fibre direction. (Real)
yt, yc
: limiting direct tensile and compressive stresses respectively normal to fibre in direction 2. (Real)
zt, zc
: limiting direct tensile and compressive stresses respectively normal to fibre in direction 3. (Real)
s12
: limiting shear stress of lamina in 1-2 plane. (Real)
s23
: limiting shear stress of lamina in 2-3 plane. (Real)
s31
: limiting shear stress of lamina in 3-1 plane. (Real)
zl
: limiting interlaminar tensile stress. (Real)
sl
: limiting interlaminar shear stress. (Real)
β 1- β 8 : dimensionless material parameters defining the reduction in lamina stiffness after different modes of
failure. (0 ≤
β i ≤ 1.0). The default of all the β s are β =0.0. See Appendix B.5.3.1 for details
Notes
1.
Up to 18 failure values are expected but if less are specified then the remaining values default to zero.
2.
If a failure strength is set (or defaults) to zero, the relevant term in the failure criterion is ignored.
5.2.4.4.4
Laminate Failure Values
The following data input is required for an elastic laminated composite when it is required that failure criteria in
terms of the shell stress/strain resultants are to be calculated.
(mat)
:
FAIL
εˆx
(temp)
εˆy
εˆxy
ψˆx
ψˆy
ψˆxy
εˆxz
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
εˆyz
Page 5-95
ASAS (Non-Linear) User Manual
Structural Data
Parameters
mat
: material property integer. (Integer, 1-9999)
FAIL
: keyword to define the properties as failure values
temp
: temperature at which these properties apply. (Real)
εˆx
: allowable direct strain in element local x direction. (Real)
εˆy
: allowable direct strain in element local y direction. (Real)
εˆxy
: allowable shear strain in element local xy plane. (Real)
ψˆx
: allowable bending curvature in element local x direction. (Real)
ψˆy
: allowable bending curvature in element local y direction. (Real)
ψˆxy
: allowable torsional curvature in element local xy plane. (Real)
εˆxz
: allowable shear strain in element local xz plane. (Real)
εˆyz
: allowable shear strain in element local yz plane. (Real)
Notes
1.
Using the above data, the laminate failure criterion as described in Appendix B.5.2 is evaluated in
POSTNL when options FEMV-GFAI are selected. Note that up to four further user defined criteria may
be evaluated and that up to 14 failure values may be specified. To be consistent with the calculation of
the first failure criterion, the first 8 failure values should be those defined above.
2.
The laminate failure data must be specified immediately after the LAMI material property data.
3.
If a failure value is set (or defaults) to zero, the relevant term in the failure criterion is ignored.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-96
ASAS (Non-Linear) User Manual
Structural Data
Examples
A simple example of an orthotropic lamina for a laminated shell with failure values specified for the direct
stresses in the fibre directions only.
MATE
1
10
LAMI
ORTH 1350.0
: 84.0E6 6.0E6 0.0 2.1E6 2.1E6 2.1E6 0.34 0.0 0.0
: -3.0E-6 35.OE-6 0.0
10 FAIL
: 1280.0E3 290.0E3
END
An example showing the data for 3 different orthotropic laminae for a laminated shell with failure values for all
stress components.
MATE
1
LAMI
10 ORTH 1350.0
: 84.0E6 6.0E6 0.0 2.1E6 2.1E6 2.1E6 0.34 0.0 0.0
: -3.0E-6 35.OE-6 0.0
10 FAIL
: 1280.0E3 290.0E3 39.0E3 150.0E3 52.0E3
20 ORTH 1610.0
: 130.0E6 9.0E6 0.0 4.8E6 4.8E6 4.8E6 0.28 0.0 0.0
: -0.1E-6 28.0E-6 0.0
20 FAIL
: 1370.0E3 1000.0E3 42.0E3 200.0E3 60.OE3
30 ORTH 1800.0
: 40.0E6 8.0E6 0.0 4.0E6 4.0E6 4.0E6 0.25 0.0 0.0
: 6.3E-6 36.0E-6 0.0
30 FAIL
: 800.0E3 600.0E3 36.0E3 150.0E3 60.0E3
END
An example showing the data for a non-linear composite material composed of layers of orthotropic material
obeying failure law 1 (FLW1)
MATE
11 ORTH
: 5.72E4 3.9E3 3.9E3 2.3E3 2.3E3 2.3E3 0.35 0.35 0.35
11 FAIL FLW1
: 1.3E3 1.3E3 12.0 53.0 34.0 0.8
1 LAMI
END
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-97
ASAS (Non-Linear) User Manual
Structural Data
An example showing the data for a linear elastic composite material composed of two different orthotropic
materials with a laminate failure criterion based on limiting curvatures only.
MATE
1
1
LAMI
FAIL
: 0.0 0.0 0.0 0.015 0.015 0.015
2 ORTH
: 5.72E4 3.9E3 3.9E3 2.3E3 2.3E3 2.3E3 0.35 0.35 0.35
3 ORTH
: 3.81E4 4.75E3 4.7E3 2.3E3 2.3E3 2.3E3 0.32 0.32 0.32
END
5.2.5
Geometric Properties Data
To define the geometric properties, such as thickness, area, or bending inertia, for every element used in the
structure.
GEOM
geom
:
eltype
(sect)
CABL
properties
properties
END
Parameters
GEOM
: compulsory header keyword to denote the start of the geometric property data
geom
: identifying number of the geometric properties integer. This number must be unique, and
independent of the type of element. (Integer, 1-999999)
eltype
: element type. This must correspond with the element type defined in the element topology
data for this geometric property integer
sect
: keyword to denote cross-section type for element STF4
properties
: list of geometric properties. See Appendix -A for the details of which properties are required
for each element type. Continuation lines may be used if necessary. (Real)
CABL
: keyword to denote the cable option for element FLA2. See Appendix -A for further details
END
: keyword to denote the end of the geometric properties data block
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-98
ASAS (Non-Linear) User Manual
Structural Data
Notes
1.
Geometric property data for elements SST4 and WST4 must be input in a different format. Details are
given in Section 5.2.5.1.
2.
Geometric property data for elements SPR1 and SPR2 must have stiffness and/or damping properties.
Details are given in Section 5.2.5.2.
3.
Geometric property data for laminated shells requires additional information concerning the layup
sequence. Details are given in Section 5.2.5.3.
4.
Geometric property data for rigid surface elements requires additional information concerning the
definition of rigid surface geometry. Details are given in Section 5.2.5.4.
5.
Geometric property data for beam elements where local axes orientation and/or offsets may be defined is
given in section 5.2.5.5
Example
A simple example of geometric property data for a model composed of beams and shells.
GEOM
1 STF4
:
:
2 TCS8
3 TCS8
END
RECT
0.05
0.05
0.05
0.05
0.05
0.05
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.0
0.010
0.008
5.2.5.1 Geometric Properties - (WST4 and SST4)
To define geometric properties for stiffeners (WST4 and SST4) the following format is used in the geometric
properties data.
geom
eltype
(isec)
scoor
tcoor
nstart
nfinish
rmul
MCOR
mn
SCON
segno
nstat
nlay
thick
FIN
Parameters
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-99
ASAS (Non-Linear) User Manual
Structural Data
geom
: identifying number of the geometric properties integer. This number must be unique, and
independent of the type of element. (Integer, 1-999999)
eltype
: element type. This must correspond with the element type defined in the element topology
data for this geometric property integer. (One of WST4 or SST4)
isec
: median point corresponding to warping origin (WST4 only). (Integer)
rmul
: rigidity multiplier (1.0 for full cross-section, 0.5 for half symmetric section). (Real)
MCOR
: compulsory header keyword to denote start of median point coordinate definition
mn
: median point number (consecutive). (Integer)
scoor
: s coordinate of median point. (Real)
tcoor
: t coordinate of median point. (Real)
SCON
: compulsory header keyword to denote start of segment connectivity data
segno
: segment number (consecutive)
nstart
: start median point of segment. (Integer)
nfinish
: finish median point of segment. (Integer)
nstat
: number of stations along segment. (Integer)
nlay
: number of layers through the thickness of segment. (Integer)
thick
: segment thickness. (Real)
FIN
: indicates end of the property set
Notes
1.
See element description sheet (Appendix -A) for details of stiffener elements.
2.
Median point numbers can be assigned in any convenient manner. Segment numbering however is not
arbitrary but must adhere to the following rules:
(a)
The first segment starts at a free edge.
(b)
Each subsequent segment starts from the end of a previously defined segment.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-100
ASAS (Non-Linear) User Manual
3.
Structural Data
The full cross-section geometry must always be defined irrespective of the value specified for rmul
Example
An example of a tee-section stiffener with the origin at the junction of web and flange
GEOM
1
MCOR
SST4
1.0
1
-0.2
0.0
2
3
0.0
0.2
0.0
0.0
4
SCON
0.0
0.256
1
1
2
3
3
0.012
2
3
2
2
3
4
3
5
3
3
0.012
0.015
FIN
END
5.2.5.2 Geometric Properties - (SPR1 and SPR2)
Stiffness and/or damping characteristics are required for springs SPR1 and SPR2 in the following format.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-101
ASAS (Non-Linear) User Manual
Structural Data
px
py
geom
eltype
:
STIF
stifprops
:
DAMP
dampprops
pz
Parameters
geom
: identifying number of the geometric properties. This number must be unique and independent
of the element type. (Integer, 1-999999)
eltype
: element type (one of SPR1 or SPR2)
Px,Py,Pz
: global coordinates of a point which defines the line of action of the spring. (Real)
STIF
: keyword to denote that stiffness characteristics are to be defined for springs
stifprops
: linear stiffness, K, or tabulated values of displacement (or rotation) and force (or moment)
(δ1, F1, δ2, F2....... δn, Fn). (Real)
DAMP
: keyword to denote that damping characteristics are to be defined for springs
dampprops : linear damping factor, C, or tabulated values of velocity (or angular velocity ) and force (or
moment) (v1, F1, v2, F2....... vn, Fn). (Real)
Notes
1.
2.
STIF and DAMP must be the first item on a line after the continuation marker (:).
If px, py and pz are zero, the line of action of the spring coincides with the local X axis (see element
description in Appendix -A).
3.
The stiffness and damping properties are extrapolated beyond the user defined points.
4.
A maximum of 20 pairs of (δ,F) and (v,F) are allowed.
5.
The angular unit must be radians and this cannot be changed
6.
S and V must be specified in ascending order.
7.
The spring curve must pass through the origin when applied to an inelastic material model.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-102
ASAS (Non-Linear) User Manual
Structural Data
Examples
An example of a rotational spring with constant stiffness, no damping and aligned with the element local axis
system.
GEOM
1 SPR2
: STIF 200.0
END
An example of a translational spring/dashpot with piecewise linear definition of stiffness and damping with a
fixed line of action.
F
F
.
v
δ
GEOM
2 SPR1
: STIF
:
: DAMP
:
1.0
-0.5
1.0
-300.0
0.0
-0.2
-200.0
0.1
400.0
0.4
600.0
0.7
650.0
-60.0
0.0
-3000.0
0.0
-30.0
20.0
-2500.0
4000.0
50.0
5000.0
END
5.2.5.3 Geometric Properties - (Laminated Construction)
To define the geometric properties and layup data for laminated elements.
geom
eltype
properties
:
LAMI
nlam
(sym)
:
mat
thick
theta
RP
nrep
(layno)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-103
ASAS (Non-Linear) User Manual
Structural Data
Parameters
geom
: identifying number of the geometric properties integer. This number must be unique and
independent of the type of element. (Integer, 1-999999)
eltype
: element type. This must correspond with the element type defined in the element topology
data for this geometric property integer. (One of QUS4, TCS6, TCS8, TCS9, LB15 or
LB20)
properties
: list of geometric properties. These must be specified for shells and omitted for bricks. See
Appendix -A for details of which properties are required for each element type. Continuation
lines may be used if necessary. (Real)
LAMI
: compulsory keyword to denote that the data for a laminate is to be defined
nlam
: number of laminae of which the laminate is composed or half the number of laminae if sym is
set to 1. See below. (Integer)
sym
: optional flag to be set to 1 if a symmetrical laminate. By default sym will be set to zero which
implies that data for all laminae is to be supplied. (Integer)
mat
: material property integer defining the material for this lamina. (Integer)
thick
: the thickness of this lamina. (Real)
theta
: the angle between the principal material axis direction for this lamina and the laminate
principal material axis direction. Default unit is degrees. (Real) Note: -90° ≤ theta ≤ + 90°
layno
: layer number to be assigned to layer.
If omitted, layers are numbered sequentially
commencing at one. The layer number is only used for post-processing purposes at present.
(Integer)
RP
: keyword to indicate the generation of lamina data from the previous / command.
nrep
: number of times the data is to be repeated. (Integer)
Notes
1.
The shell nodal thicknesses must be specified and be non-zero. The laminae data specified here are used
to calculate the equivalent anisotropic material matrix coefficients C1 to C24 in the manner described in
Appendix -B. The thickness terms appearing in the C matrix as described in Appendix -A are
interpolated from the nodal thicknesses supplied here. For laminated brick elements, the laminated
thickness is directly obtained from the element geometry and the nodal thickness data are not required.
2.
The properties mat, thick, theta and layno are repeated nlam times. There is no limit to the number of
laminae that may be used to define a laminate.
3.
The material for a lamina may be defined as isotropic, orthotropic or anisotropic.
4.
Layer number 1 lies on the bottom surface of an element as defined by the element local axis system. See
Appendix -A.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-104
ASAS (Non-Linear) User Manual
5.
Structural Data
A number of layers, delimited by a / command and an RP command, may be repeated nrep times to
create a regular region of the laminate. See example 3.
Examples
A simple example of the geometric property data for a laminated QUS4 shell element of constant thickness equal
to the sum of the thicknesses for all laminae. The laminate is composed of 5 laminae using 2 different material
types. The layup sequence is [-90/-45/0/45/90].
GEOM
1
QUS4
:
LAMI
: 10 1.0
: 10 1.0
: 20 3.0
: 10 1.0
: 10 1.0
END
7.0
5
-90.0
-45.0
0.0
45.0
90.0
An example showing the geometric property data for a laminated and tapered TCS8 shell element where the sum
of the thicknesses of all the laminae equals the average thickness for the element as defined by the nodal
thicknesses. Note that the laminate is formed of 4 laminae but as the layup is symmetrical sym is set to 1. The
layup sequence is [90/0/0/90] or in abbreviated form [90/0]s.
GEOM
1
TCS8
:
:
LAMI
: 98 1.0
: 99 1.0
END
5.0 5.0 5.0 4.0
3.0 3.0 3.0 4.0
2 1
90.0
0.0
An example showing the use of both the symmetry option and the repeat facility for a laminate brick composed
of a total of 60 layers. Two materials are used, one is orthotropic and the other is isotropic. The corresponding
material data is also shown.
GEOM
1
LB20
:
LAMI 30 1
/
: 11 0.045 0.0
: 12 0.06 0.0
: 11 0.045 90.0
RP 10
END
*
MATE
1
LAMI
11 ORTHO
: 25.0E6 1.0E6 1.0E6
12 ISO
3.7E6 0.3
END
0.5E6
0.2E6
0.5E6
0.25
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
0.25
0.25
Page 5-105
ASAS (Non-Linear) User Manual
Structural Data
5.2.5.4 Geometric Properties - (Rigid Surface Elements)
To define the geometric properties, if present, and rigid surface geometry for rigid surface elements.
geom
eltype
(thick)
:
RIGS
nseg
LINE
node1
node2
CIRC
node1
node2
:
node3
Parameters
geom
: identifying number of the geometric properties integer. This number must be unique, and
independent of the type of element. (Integer, 1-999999)
eltype
: element type. This must correspond with the element type defined in the element topology
data for this geometric property integer, (one of RG23, RG24, RGX3 or RGX4)
thick
: nodal thickness, only required for element types RG23 and RG24 when attached to plane
stress membrane elements. See Appendix -A for details of which properties are required for
each element type. Continuation lines may be used if necessary. (Real)
RIGS
: keyword to denote that geometry of the rigid surface is to be defined
nseg
: number of segments defining the rigid surface. (Integer)
LINE
: keyword to denote that the current segment type is linear
CIRC
: keyword to denote that the current segment type is circular
node1
: node number at start of segment. (Integer)
node2
: node number at end of segment. (Integer)
node 3
: node number defining centre of the segment if circular. (Integer)
Notes
1.
The coordinates of the node numbers must be defined in the Coordinate data.
2.
The order of input of the nodes defines the direction of positive progression along the rigid surface
(indicated by s in the example below). A right handed rotation of 90° from the positive tangent direction
then defines the outward normal to the surface (i.e. n in example below).
3.
The user should ensure that the rigid surface definition extends far enough to cover all expected motions
of the deforming and rigid parts of the model.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-106
ASAS (Non-Linear) User Manual
Structural Data
Example
An example of an axisymmetric rigid punch
GEOM
n
1
RGX3
:
:
RIGS
LINE
3
1
2
:
CIRC
2
3
: LINE
END
3
4
1
2
s
n
s
5
3
5
n
s
CL
4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-107
ASAS (Non-Linear) User Manual
Structural Data
5.2.5.5 Definition of geometric properties for beam elements having local axes definition
and/or rigid offsets
There are four engineer’s theory of bending, two-node beam types in ASAS for which the user can define the
local axes and/or specify rigid offsets. In order to prevent confusion, the data requirements for each of these
have been presented explicitly. These definitions may be used in any combination together with the general
definition described in Section 5.2.5 to build a complete geometric data block (headed by the keyword GEOM
and terminated by the keyword END) for a structure consisting of a mixture of any of the ASAS elements.
a) BEAM
sectid
geom
BEAM
:
OFFG
glboff
OFFS
locoff
OFSK
skew
OFCO
coords
j
iy
iz
a
skw off
b) BM2D
sectid
geom
BM2D
a
:
OFFG
glboff
OFFS
locoff
OFSK
skew
OFCO
coords
iz
ay
skw off
Notes
1.
Only 4 offset values are specified relating only to offsets in the global XY and local X’Y’ planes.
2.
Only skewed systems that are a rotation about the global Z may be used.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-108
ASAS (Non-Linear) User Manual
Structural Data
c) BM3D
sectid
geom
BETA
angle
NODE
nodeno
(COOR)
pcoor
(XY)
(SHAR)*
BM3D
a iz iy j
GPOS
ay
az
XZ
GNEG
axis
SPOS
skew
SNEG
VECT
:
OFFG
glboff
OFFS
locoff
OFSK
skew
OFCO
coords
*
Shear areas
must not be defined here if
section data has been referenced.
The shear areas should be given as part
of the section data.
vcoor
skwoff
d) TUBE
sectid
geom
BETA
angle
NODE
nodeno
(COOR)
pcoor
(XY)
TUBE
dia thick
GPOS
XZ
GNEG
axis
SPOS
skew
SNEG
VECT
:
OFFG
glboff
OFFS
locoff
OFSK
skew
OFCO
coords
vcoor
skwoff
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-109
ASAS (Non-Linear) User Manual
Structural Data
Parameters
a) General
geom
: identifying number for the geometric property. This number must be unique, a separate
number being required for every different element type as well as for each differing
geometric definition. (Integer)
BEAM, BM2D,
BM3D, TUBE
sectid
: element type. This must correspond to the element type defined in the element topology
referencing this geometric property.
: section identifier. (Alphanumeric up to 12 characters). This refers to a section input as
SECTION data. See Section 5.2.6.
b) Axes Definition
BETA
: keyword to denote that local axis defined by beta angle (rotation of default local axes about
member X axis). See Appendix A.2.
angle
: beta angle. (Real, degrees)
NODE
: keyword to denote that local axis defined by third node point. See Appendix A.2.
nodeno
: third node number. (Integer)
COOR
: keyword to denote that local axis defined by third point coordinates. See Appendix A.2.
pcoor
: global coordinates (x, y, z) of third point. (Real)
GPOS
: keyword to denote that local axis defined by positive axis direction in global reference
plane. See Appendix A.2.
GNEG
: keyword to denote that local axis defined by negative axis direction in global reference
plane. See Appendix A.2.
SPOS
: keyword to denote that local axis defined by positive axis direction in a skewed reference
plane. See Appendix A.2.
SNEG
: keyword to denote that local axis defined by negative axis direction in a skewed reference
plane. See Appendix A.2.
axis
: axis defining global/skewed reference plane (X,Y or Z).
skew
: skew integer for defining skewed reference plane. (Integer)
VECT
: keyword to denote that local axis defined by vector. See Appendix A.2.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-110
ASAS (Non-Linear) User Manual
Structural Data
vcoor
: global coordinates (x,y and z) which define a vector direction from the origin.
XY,XZ
: keywords to denote that axis being defined is in local XY or local XZ plane. See Appendix
A.2.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-111
ASAS (Non-Linear) User Manual
Structural Data
c) Offset Definition
OFFG
: keyword to denote that offsets are to be defined using global coordinate axes.
See
Appendix A.3.
glboff
: global offset values for both ends of the beam element. (Real)
OFFS
: keyword to denote that offsets are to be defined using the elemental local axes. See
Appendix A.3.
locoff
: local offset values for both ends of the beam element. (Real)
OFSK
: keyword to denote that offsets are to be defined using a skewed coordinate axis system.
See Appendix A.3.
skew
: integer for the skew system in which offsets are to be defined.
skwoff
: skewed offset values for both ends of the beam element. (Real)
OFCO
: keyword to denote that offsets are to be defined by explicit definition of the global end
coordinates of the physical member.
coords
: coordinates of both ends of the physical member. (Real)
d) Basic properties (see Appendix A for full element specification)
a
: cross-sectional area, constant for section. (Real)
iz
: 2nd moment of area about local ZZ axis, constant for section. (Real)
iy
: 2nd moment of area about local YY axis, constant for section. (Real)
j
: torsion constant, constant for section. (Real)
SHAR
: keyword indicating that shear areas follow.
ay
: shear area in local Y, constant for section. (Real)
az
: shear area in local Z, constant for sectio. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-112
ASAS (Non-Linear) User Manual
Structural Data
Notes
1.
Nonsections must not be assigned to TUBE elements.
2.
Only relevant flexural properties will be utilised for a given element type, for example
BEAM
3.
BM2D
BM3D
TUBE
Area
A
♦
♦
♦
Moment of Inertia
IZ
♦
♦
♦
Moment of Inertia
IY
♦
♦
Torsion constant
J
♦
♦
Shear Area
AY
Shear Area
AZ
Diameter
D
♦
Thickness
T
♦
♦
♦
♦
When the properties for some beams are to be given by section data and for others explicitly, the two
types of definition may be mixed.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-113
ASAS (Non-Linear) User Manual
5.2.6
Structural Data
Section Data
To define section type, dimensions and properties for sections to be used with element types BEAM, BM2D,
BM3D and TUBE elements.
SECT
sectid
type
XSEC
dimensions
sectid
FAB
ftype
dimensions
ftype
dimensions
:
flexprops
:
FLEX
proptype
:
ORIG
property
TOP
(zoff)
LEFT
(yoff)
BOTT
(zoff)
RIGH
(yoff)
(CENT)
(CENT)
END
Parameters
SECT
: compulsory header to denote the start of the section data.
sectid
: section identifier. (Alphanumeric, up to 12 characters). This identifier must be unique and is
independent of the section type.
type
: type, or shape, of section being defined. (Alphanumeric, up to 4 characters).
Valid types are:
WF
wide flange
FBI
Fabricated I beam
TUB
tubular
RHS
rolled hollow section
BOX
fabricated box
CHAN
channel
ANGL
angle
TEE
tee
PRI
general prismatic section
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-114
ASAS (Non-Linear) User Manual
Structural Data
see Section 5.2.6.1
XSEC
: keyword to denote that cross-section dimensions are to be defined on this line. See Note 1
dimensions : list of section dimensions. See Section 5.2.6.1 for the details of which dimensions are required
for each section type. (Real)
FAB
: keyword to denote that a FABricated plate section is to be defined on this and subsequent lines.
ftype
: type of dimensional property being defined for Fabricated plate section (Alphanumeric, up to 4
characters).
Valid types are:
BLOC
flat plate section
CURB
curved plate section
CUT
cut line
POIN
stress point
see Section 5.2.6.2
FLEX
: keyword to denote that geometric properties are to be defined on this line. See Note 1
flexprops
: list of geometric properties. For all section types this is AX,IZ,IY,J,AY,AZ
where
AX
cross sectional area
IZ
principal moment of inertia about element local Z axis
IY
principal moment of inertia about element local Y axis
J
torsion constant
AY
effective shear area for forces in element local Y direction
AZ
effective shear area for forces in element local Z direction
Shear strain is neglected for a given direction if AY and/or AZ is zero.
proptype
: name of geometric property to be defined. Valid names are AX,IZ,IY,J,AY,AZ with the
meaning as above.
property
: value to be assigned to the named geometric property.
Notes
1.
For any given section identifier XSEC and/or FLEX commands may be supplied with the following
interpretations.
If only XSEC is defined, the geometric properties will be automatically calculated by the program for use
in the structural analysis.
If only FLEX is defined, all property values must be supplied.
If both XSEC and FLEX commands are utilised, any geometric properties explicitly defined will
overwrite those calculated from the section dimensions. This feature permits modification to the stiffness
of the section to model ring or web stiffeners, built up sections, etc.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-115
ASAS (Non-Linear) User Manual
Structural Data
The FLEX and XSEC sub-commands and associated data are interchangeable, i.e. FLEX appears on the
sectid line with the (optional) XSEC command on a continuation line.
2.
e.g
W24x100
WF
:
XSEC
24.0
12.0
0.775
0.468
FLEX
29.11
2950.0
223.4
4.405
FLEX
XSEC
29.11
24.0
2950.0 223.4 4.405
12.0
0.775 0.468
is the same as
W24x100
WF
:
3.
For FABbricated plate sections, notes 1 and 2 also apply but XSEC replaced by BLOC, CURB, CUT or
POIN. The order of these data lines are interchangeable, but a logical sequence is recommended.
4.
Only 4 POIN definitions may be used for each FABricated section.
5.2.6.1 Section Types and Dimensions
ASAS only requires areas and inertias to be specified for beam elements to determine the elemental forces. In
order to simplify data input the section dimensions may be supplied in lieu of, or in addition to, the flexural
properties. The following describes the dimensions required for each section type currently valid in ASAS.
Note
The axes shown correspond to the local axes of the member for element types BEAM, BM3D, TUBE and
BM2D.
Example
SECT
W24x100
WF
XSEC
24.0
12.0
P3.5STD
:
TUB
XSEC
FLEX
4.0
2.68
0.226
4.79
W18x105
WF
FLEX
30.621
R10x6x3/8
:
RHS
XSEC
FLEX
10.0
IZ
1836.4
6.0
184.0
0.775
4.79
0.468
1.34
249.07
6.7164
0.375
END
Tube - Type TUB
Two dimensions must be defined
Values are D T
where
D
is the outer diameter
T
is the wall thickness
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-116
ASAS (Non-Linear) User Manual
Structural Data
Wide flange - Type WF
A maximum of five dimensions can be provided : the first four are obligatory.
Values are
where
D
B
TF TW (F)
D
is the beam depth
B
is the flange width
TF
is the flange thickness
TW
is the web thickness
F
is the fillet radius
(optional, assumed zero)
Fabricated I beam - Type FBI
A maximum of six dimensions can be provided : the first four are obligatory.
Values are
where
D
BT
TT TW BB
TB
D
is the beam depth
BT
is the top flange width
TT
is the top flange thickness
TW
is the web thickness
BB
is the bottom flange width
(optional, assumed same as BT)
TB
is the bottom flange thickness
(optional, assumed same as TT)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-117
ASAS (Non-Linear) User Manual
Structural Data
Rolled Hollow Section - Type RHS
A maximum of four dimensions can be provided: the first three are obligatory.
Values are
where
D B T (F)
D
is the beam depth
B
is the beam width
T
is the thickness
F
is the fillet radius (optional, assumed zero)
Fabricated Box - Type BOX
A maximum of five dimensions can be provided: the first four are obligatory.
Values are D B TT TS TB
where
D
is the beam depth
B
is the beam width
TT
is the thickness of the ‘top’ plate
TS
is the thickness of the ‘side’ plates
TB
is the thickness of the ‘bottom’ plate
(optional, assumed same as TT)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-118
ASAS (Non-Linear) User Manual
Structural Data
Channel - Type CHAN
A maximum of five dimensions can be provided: the first four are obligatory.
Values are D B TF TW (F)
where
D
is the beam depth
B
is the flange width
TF
is the flange thickness
TW
is the web thickness
F
is the fillet radius
(optional, assumed zero)
Angle - Type ANGL
A maximum of four dimensions can be provided: the first three are obligatory.
Values are
where
D B T (F)
D
is the beam depth
B
is the flange width
T
is the thickness
F
is the fillet radius (optional, assumed zero)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-119
ASAS (Non-Linear) User Manual
Structural Data
Tee - Type TEE
A maximum of five dimensions can be provided: the first four are obligatory.
Values are D B TF TW (F)
where D
B
is the beam depth
is the flange width
TF
is the flange thickness
TW
is the web thickness
F
is the fillet radius
(optional, assumed zero)
Prismatic section - Type PRI
Two dimensions must be defined. For this section type, the flexural properties must also be defined.
Values are D B
where
D
is the maximum depth crossing the Z axis
B
is the maximum breadth crossing the Y axis
5.2.6.2 Fabricated Plate Sections
The Fabricated plate section is defined by a series of plate segments arranged to form the required cross-section.
These plate segments may either be straight (BLOC) or curved (CURB), and are defined by their dimensions and
location, with respect to an arbitrary origin on the cross-section. In addition, cut lines may be introduced, to
prevent adjacent segments being physically joined. Finally, up to four stress points may be defined on the
section for the purpose of stress evaluation in post-processing.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-120
ASAS (Non-Linear) User Manual
Structural Data
BLOC - Straight Plate Segment
A maximum of seven values can be provided: the first four are obligatory.
Values are L T YL ZL (AL C1 C2)
where
L
is the length of the plate segment
T
is the thickness of the plate segment
YL
is the Y location of plate centroid
ZL
is the Z location of plate centroid
AL
is the angular orientation of the plate
(optional, assumed zero)
C1
is the integer for the first associated cell
C2
is the integer for the second associated cell
(C1 and C2 are optional, assumed zero)
Note
AL must be in range -90° to +90°
CURB - Curved Plate Segment
A maximum of eight values can be provided: the first five are obligatory
Values are R T A YL ZL (AL C1 C2)
where
R
is the mean radius of plate segment
T
is the thickness of the plate segment
A
is the angle subtended by the plate
YL
is the Y location of the plate centroid
ZL
is the Z location of the plate centroid
AL
is the angular orientation of the plate
(optional, assumed zero)
C1
is the integer for the first associated cell
C2
is the integer for the second associated cell
(C1 and C2 are optional, assumed zero)
Note
A and AL are measured anti-clockwise (AL from Z axis) in degrees.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-121
ASAS (Non-Linear) User Manual
Structural Data
CUT - Cut Line
A maximum of four values can be provided: the first two are obligatory
Values are Y1 Z1 (Y2 Z2)
where
Y1, Z1
give the position of start of cut line
Y2, Z2
give the position of end of cut line
(optional, assumed same as Y1, Z1)
Note
Cut line must occur at a segment boundary. If only two values specified, the nearest boundary will be cut.
POIN - Stress Point
Two values must be defined.
Values are Y1 Z1
where
Y1, Z1
give the position of the stress point
Example
SECT
FABSEC001
:
:
:
:
:
:
:
:
:
:
END
FAB
BLOC
CURB
BLOC
BLOC
BLOC
BLOC
CUT
POIN
POIN
POIN
POIN
50
15
20
70
30
30
40
0
50
50
0
10
10
10
10
10
10
5
0
0
70
70
45
90
20
5
25
25
25
30
65
35
25
5
0
50
90
0
90
90
1
0 1
1
1
1
*segment 1
*segment 2
*segment 3
*segment 4
*segment 5
*segment 6
*segment 6&1
*stress point
*stress point
*stress point
*stress point
1
2
3
4
Notes
1.
The location of the segments may be defined in relation to any origin. The centroidal axes will be
calculated automatically.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-122
ASAS (Non-Linear) User Manual
Structural Data
2.
The axes used to define cut lines and stress points must be the same as that used to locate the segments.
3.
The positioning of stress points is not restricted in any way. Thus a stress point could be off the section.
5.2.7
Skew System Data
There are two methods of defining skew systems. These are by the ‘skew system’ data using direction cosines
and by the ‘nodal skew’ data using 3 node points. The two facilities are complementary, the user may use either
or both types of data as is convenient.
5.2.7.1 Skew Systems - Direction Cosines
To define skew systems in terms of six direction cosines.
SKEW
x'x
skew
x'y
x'z
y'x
y'y
y'z
END
Parameters
SKEW
: compulsory header keyword to denote the start of the skew system data
skew
: skew system integer. (Integer, 1-9999)
x’x,x’y,x’z
:
6 directional cosines. (Real)
y’x,y’y,y’z
END
: compulsory keyword to denote the end of the skew system data block
Notes
1.
The skew integers must be unique between the SKEW and NSKW data.
2.
The direction cosines supplied are checked for unity and orthogonality as follows:
3.
x ′ x 2 + x ′ y2 + x ′ z 2
= 1.0 ± 0.001
y′ x 2 + y′ y2 + y′ z 2
= 1.0 ± 0.001
x ′x* y′x+ x ′y* y′y+ x ′z* y′z
= 0.0 ± 0.001
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-123
ASAS (Non-Linear) User Manual
Structural Data
Example 1
Example of Skew Systems data
SKEW
1 0.8660
2 0.6830
END
0.5000
0.2588
0.0
-0.6830
-0.5000
0.1830
0.8860
-0.9659
0.0
-0.1830
Y
The first line gives the direction cosines for a local axis
Y'
system which has local Z’ coincident with global Z, and
local X’ and local Y’ rotated by 30° in the global XY
X'
plane.
30°
X
Angle between local X’ and global X
= 30°
Direction cosine X’X
=
0.8660
Angle between local X’ and global Y
= 60°
Direction cosine X’Y
=
0.5000
Angle between local X’ and global Z
= 90°
Direction cosine X’Z
=
Angle between local Y’ and global X
= 120°
Direction cosine Y’X
=
-0.5000
Angle between local Y’ and global Y
= 30°
Direction cosine Y’Y
=
0.8660
Angle between local Y’ and global Z
= 90°
Direction cosine Y’Z
=
0.0
Example 2
0.0
Z'
X'
The second line gives the direction cosines for a local
axis system which is inclined to all the global axes.
The local X’ axis is defined by the coordinates
(46,27.789,27)
(36,24,37)
(37.895,14,35.105)
(36,24,37) and (46,27.789,27). The distance between
these points is:
2
2
2
(46 - 36) + (27.789 - 24) + (27 - 37) = 14.641
Hence, the direction cosines for local X’ are given by:
X ′X =
46 - 36
= 0.6830
14.641
X ′Y =
27.789 - 24
= 0.2588
14.641
Y'
X ′Z = 27 -
37
= -0.6830
14.641
Similarly, the local Y’ axis is defined by two points 10.353 apart and the direction cosines for local Y’ are given
by:
Y ′X =
37.895 − 36
= 0.1830
10.353
YY=
14 − 24
= -0.9659
10.353
Y ′Z =
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
35.150 − 37
= -0.1830
10.353
Page 5-124
ASAS (Non-Linear) User Manual
Structural Data
5.2.7.2 Skew Systems - Nodal Definition
To define skew systems in terms of three node points
NSKW
node1
skew
node2
node3
END
Parameters
NSKW
: compulsory header keyword to denote the start of the nodal skew data
skew
: skew system integer. (Integer, 1-9999)
node1
node2
node3
: 3 node numbers. Used to define a local axis set in the following manner. The line from the first
node to the second node defines the local x’ direction. The plane defined by the three nodes
contains the local y’ direction which lies from the first node towards the third. The local z’ axis
forms a right handed set with local x’ and y’
END
: compulsory keyword to denote the end of the nodal skew system data block
Notes
1.
The skew integers must be unique between SKEW and NSKW data.
2.
The nodes used to define a skew system must appear in the COOR data. It is not necessary for these
nodes to be physically present on the structure i.e. they need not appear in the ELEM data.
Example
The first line in the example below describes a 2-D rotation in the x-y plane. Note, the global z axis points
towards the reader but the local z’ axis, forming a right handed set with x’ and y’,
points away from the reader.
z
NSKW
100
101
16
109
25
216
37
54
x'
END
25
y
16
37
z'
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
x
y'
Page 5-125
ASAS (Non-Linear) User Manual
5.3
Boundary Conditions Data
BOUNDARY Conditions Data
These data blocks define the various ways in which the structure is supported and constrained.
The following data blocks are defined
Freedom Releases .... ................ ................ see Section 5.3.2
Suppressions ............ ................ ................ see Section 5.3.3
Displaced Freedoms ................. ................ see Section 5.3.4
Constraint Equations ................ ................ see Section 5.3.5
Rigid Constraints ..... ................ ................ see Section 5.3.6
Note
Freedom Release Data, if it exists, must be the first data block in the Boundary Conditions Data.
5.3.1
UNITS Command
The units command is not valid in the Boundary Conditions Data and will be ignored. Therefore any constants
and factors utilised in constraint equations must be consistent with any global units (analysis units) defined in the
Preliminary Data (see Section 5.1.42).
5.3.2
FREEDOM Release Data
To define elements which are to have particular freedoms released from being rigidly connected to the
surrounding elements. Release can only apply to beam elements and the freedoms released are in their local axis
system. See Notes below for more details. If used, freedom release data must be the first data block in the
Boundary Conditions Data.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-126
Boundary Conditions Data
ASAS (Non-Linear) User Manual
RELE
(skew )
dof
//elno//
//node//
RP
nrep
ielem
inode
RRP
nrrep
iielem
iinode
END
Parameters
RELE
: compulsory header to define the start of the freedom release data.
skew
: skew system integer. (Integer) Optional.
dof
: name of freedom to be released. See notes.
elno
: user element number of element to be released. (Integer)
node
: node number on the element at which the freedom is to be released. (Integer)
RP
: keyword to indicate data generation from the previous / symbol.
nrep
: the number of times the data is to be generated.
ielem
: user element number increment. (Integer)
inode
: node number increment. (Integer)
RRP
: keyword to indicate data generation from the previous // symbol.
nrrep
: the number of times the data is to be generated.
iielem
: user element number increment. (Integer)
iinode
: node number increment. (Integer)
END
: compulsory keyword to denote the end of the freedom release data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-127
ASAS (Non-Linear) User Manual
Boundary Conditions Data
Notes
1.
Only one skew system is allowed at a node. A node may not be given a different skew system in the
suppression data from that defined in the freedom release data, etc.
2.
When beam offsets are used at an element and node which is to be released, the release is applied to the
element at the offset position in the offset local axes.
3.
Care should be taken when using local releases on a beam which has its local axes defined by the
coordinates of a 3rd point in the geometric property data. If the basic COOR data has been rotated by use
of a DCOS command, the 3rd point is not similarly rotated.
Local Releases
Local releases are only available on the following element types: BEAM, BM2D, BM3D and TUBE. Valid
released freedom names are X, Y, Z, RX, RY and RZ. (only X, Y and RZ for BM2D)
Rotational releases may be used to put hinged or pinned connections into the member. Translational releases
will produce a sliding joint.
The user should not specify an excessive number of releases for an element. For example one release of a local
RX freedom will be adequate to prevent that member carrying torque, but if both RX local freedoms of an
element are released then that element can turn on its own axis as a local mechanism.
Displacements corresponding to the local releases are not calculated or printed.
If a skew is defined, all skewable degrees of freedom at the node are rotated to the new axis system, not only
those defined by dof.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-128
Boundary Conditions Data
ASAS (Non-Linear) User Manual
Example
1.
In this example, three beam elements with User elements number 5, 7 and 10 meet at node 20. Elements
7 and 10 have local RZ released to create a pinned joint. RZ on element 5 is not released. If a release had
been applied to element 5, the original RZ freedom would be left with zero stiffness and would need to be
suppressed to prevent a local singularity in the structure. (Note that the rotations on elements 7 and 10
cannot be obtained).
10
20
Y
5
7
X
RELE
RZ
7
20
RZ
20
10
END
5.3.3
SUPPRESSED Freedoms Data
This data defines the nodes and freedoms which are to be suppressed. Any degree of freedom defined here will
have a value of zero for displacement for all load cases in the results.
SUPP
(skew )
dof
RP
nrep
inode
RRP
nrrep
iinode
//nodes//
END
Parameters
SUPP
: compulsory header to define the start of the suppressed freedom data
skew
: optional skew system identifier, see Section 5.2.7. (Integer)
dof
: names of the freedoms to be suppressed. Up to 5 freedoms may be defined. See Appendix -F
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-129
ASAS (Non-Linear) User Manual
nodes
Boundary Conditions Data
: list of nodes at which the degrees of freedom are to be suppressed. Continuation lines may be
used if required. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command. (Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node increment to be added each time the data is generated by the RRP command. (Integer)
END
: compulsory keyword to define the end of the suppressed freedom data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-130
Boundary Conditions Data
ASAS (Non-Linear) User Manual
Notes
1.
The word ALL may be used to indicate that all freedoms at the given node or nodes are to be suppressed.
2.
If a skew is defined, all skewable degrees of freedom at the node are rotated to the new axis system, not
only those defined by dof.
3.
Reference to a node number or degrees of freedom which does not exist on the structure will produce a
warning message. Reference to a node number outside the range of node numbers used on the structure
will produce an error message.
Examples
A simple example of the use of several freedoms at a node, a skew system and the use of ALL.
SUPP
X
Y
1
RZ
15
Z
25
35
39
40
19
ALL
END
1
20
An example to suppress the Z degree of freedom for all nodes in a 2-D membrane structure, say 500 nodes.
SUPP
/
Z
1
RP 500
END
5.3.4
1
Prescribed Freedom Data
This data defines the nodes and freedoms which can be given a prescribed non-zero value of displacement,
velocity or acceleration in the load data. See also Section 5.4.3.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-131
Boundary Conditions Data
ASAS (Non-Linear) User Manual
DISP
VELO
ACCN
(skew )
dof
RP
nrep
inode
RRP
nrrep
iinode
//nodes//
END
Parameters
DISP
: compulsory header to define the start of the prescribed displacement data
VELO
: compulsory header to define the start of the prescribed velocity data
ACCN
: compulsory header to define the start of the prescribed acceleration data
skew
: optional skew system identifier (see Section 5.2.7)
dof
: names of the freedoms to be displaced. Up to 5 freedom may be defined. See Appendix -F
nodes
: list of nodes at which the degrees of freedom are to be given a fixed displacement, velocity or
acceleration. Continuation lines may be used if required. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command. (Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
END
: compulsory keyword to define the end of the prescribed displaced freedom data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-132
ASAS (Non-Linear) User Manual
Boundary Conditions Data
Notes
1.
Only one of the three compulsory headers is allowed in an analysis.
2.
The word ALL may be used to indicate that all freedoms at the given node or nodes are to have
prescribed displacements, velocities or accelerations.
3.
If a skew is defined, all skewable degrees of freedom at a node are rotated to the new axis system, not
only those defined by dof.
4.
If a skew is used at a node, the same skew integer must be defined when the prescribed displacement,
velocity or acceleration is defined in the loading data. See Section 5.4.3.
5.
Prescribed velocities and accelerations may only be used in transient dynamic analyses.
6.
Reference to a node number or degrees of freedom which does not exist on the structure will produce a
warning message. Reference to a node number outside the range of node numbers used on the structure
will produce an error message.
7.
For transient analysis, non-zero prescribed displacements or velocities should not be applied at time t =
0.0. Any such values specified will be ignored by the program. The initial conditions (INIT) data block
should be used to specify initial conditions instead.
Example
An example to define nodes 126 and 128 as having displaced freedoms in the Y direction.
DISP
Y
126
END
5.3.5
128
CONSTRAINT Equation Data
This data defines degrees of freedom on the structure whose displacements are to be linearly dependent on one
or more other degrees of freedom in the structure. Currently, constraint equation data is not allowed in explicit
transient dynamics analysis.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-133
Boundary Conditions Data
ASAS (Non-Linear) User Manual
CONS
(skew )
ddof
//dnode//
RP
nrep
inode
RRP
nrrep
iinode
factor
dof
//node//
END
Parameters
CONS
: compulsory header to define the start of the constraint equation data
skew
: optional skew system identifier. Only the dependent node is skewed. (Integer)
Data for the dependent freedom on the left hand side of the constraint equation:
ddof
: dependent freedom name. See Appendix -F
dnode
: dependent node number. (Integer)
Data for the independent freedoms on the right hand side of the constraints equation:
factor
: multiplying factor for the following independent freedom. (Real)
dof
: independent freedom name. See Appendix -F
node
: independent node number. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
END
: compulsory keyword to define the end of the constraint equation data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-134
ASAS (Non-Linear) User Manual
Boundary Conditions Data
Notes
1.
Continuation lines may be used where necessary.
2.
The word ALL cannot be used in the constraint equation data. Each equation must be separately and
explicitly defined or generated with RP and RRP commands.
3.
If a skew is defined for a dependent node, all skewable degrees of freedom at the dependent node are
rotated to the new axis system, not only the ddof freedom. Freedoms at the independent nodes are
unaffected by this skew.
4.
The equations must be organised in such a way that a dependent freedom is never used in another
constraint equation as an independent freedom.
for example
Y18 = 0.5Y20 + 0.5Y21
Y16 = Y18
is not admissable since Y at node 18 is the dependent freedom in the first equation and an independent
freedom in the second. These equations should be rearranged as
Y18 = 0.5Y20 + 0.5Y21
Y16 = 0.5Y20 + 0.5Y21
5.
Dependent freedoms must be truly free and not suppressed, displaced or otherwise restrained.
6.
A constant term may be introduced into the right hand side of the equation. In this case the node number
and freedom of the first independent term should be omitted and the factor becomes the constant
displacement. This is equivalent to constraining to a displaced freedom with the same displacement.
(See example 3 below).
7.
Constraints may be used to remove local singularities in a structure. For example, an out-of-plane
membrane freedom which has zero stiffness may be constrained to a suitable neighbouring point which
has stiffness.
However, constraints cannot be used to remove a rigid body motion from a whole structure which is due
to a lack of overall support. This can only be done with suppressed or displaced nodes.
8.
The forces associated with the constraint systems are printed out as reactions.
9.
Note that constraint equations may sometimes be used to remove local singularity but this must be treated
with caution. Consider the example where a model is created by joining together two detached
components, one properly supported and one unrestrained, through the use of constraints, singularity can
be removed if each dependent freedom of a constraint lies in the supported side of the model and the
element that it is being attached to has a lower system number than the other side where the constraint is
connecting to.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-135
Boundary Conditions Data
ASAS (Non-Linear) User Manual
Examples
In this example, the displacements of node 19 in the global X and Y directions are to be tied to the global X, Y
and RZ displacements of nodes 30 and 33. Because the displacements are all related to the global axes, there is
no need for skew systems. The displacements are related by the following equations:
X19 = 0.5 X30 + 0.5 X33
Y19 = 0.3 X30 - 0.3 Y30 + 0.5 RZ30 - 0.3 X33 + 0.3 Y33
CONS
X
19
0.5
X
30
0.5
Y
:
19
0.3
-0.3
X
X
30
33
-0.3
0.3
X
33
Y 30
Y 33
0.5
RZ
30
END
A Pin-ended Beam
The beam 88-89 is to be attached by a pin joint to the continuous
column 23-24-25. The nodes 24 and 89 have the same coordinates. In
this example the joint is taken to a ball joint, with complete freedom
of rotation. The details of some joints require the constraining of one
25
or two of the rotational freedoms.
CONS
X
Y
89
89
1.0
1.0
X
Y
24
24
Z
89
1.0
Z
24
88
89
24
END
23
A Rigid Edge
The edge 1-2-3 of the structure is to be kept rigid whilst node 2 is to
be displaced by 0.2 units in the X-direction. The displacements are
4
related by the equation:
1
X2 = 0.2 = (X1 + X3) /2
5
2
6
3
0.2
giving:
X2 = 0.2 (a prescribed displacement)
X3 = 0.4 - X1
CONS
X
3
END
0.4
-1.0
X
1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-136
Boundary Conditions Data
ASAS (Non-Linear) User Manual
5.3.6
RIGID Constraints Data
To define rigid regions of the structure. Rigid constraints (rigid elements) are a more convenient method of
specifying constraint equations for particular modelling situations. They can be considered as equivalent to a
string of one or more rigid elements linking the list of nodes. Currently, rigid constraint data is not allowed in
explicit transient dynamics analysis.
RCON
(skew )
eltype
//indep//
RP
nrep
inode
RRP
nrrep
iinode
//nodelist//
END
Parameters
RCON
: compulsory header to denote the start of the rigid constraint data
skew
: optional skew system identifier. Only the dependent freedom is skewed. (Integer)
eltype
: rigid element type. See notes. Allowable element types are RLNK, RBM2, RBM3, RLSY,
RBSY, SBRK, SBSY
indep
: independent node number. (Integer)
nodelist
: list of dependent nodes. (Integer) Continuation lines may be used if required
RP
: keyword to indicate data generation from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: the increment for the independent node and the dependent nodes. (Integer)
RRP
: keyword to indicate data generation from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: the increment for the independent node and the dependent nodes. (Integer)
END
: compulsory keyword to denote the end of the rigid constraint data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-137
Boundary Conditions Data
ASAS (Non-Linear) User Manual
Notes
1.
The following Rigid Element types are available:
RLNK - 3-D rigid pin-ended link
RBM2 - 2-D rigid beam
RBM3 - 3-D rigid beam
RLSY - 3-D rigid pin-ended link system
RBSY - 3-D rigid beam system
SBRK - shell-brick interface link
SBSY - shell-brick interface system
2.
Currently, there is a restriction that the dependent node must not be skewed in large displacement
analysis.
The characteristics of each element are as follows:
Name
No of Nodes
Nodal
RLNK
RBM2
RBM3
RLSY
RBSY
SBRK
SBSY
2
2
2
arbitrary
arbitrary
2
arbitrary
X,Y,Z
X,Y
X,Y,Z
X,Y,Z
X,Y,Z
X,Y,Z
X,Y,Z
X,Y,Z
X,Y,RZ
X,Y,Z
X,Y,Z
X,Y,Z
X,Y,Z
X,Y,Z
RX,RY,RZ
for
for
dependent
dependent
X,Y,Z
X,Y,Z
RX,RY,RZ
RX,RY,RZ
for
for
independent
independent
coordinates
Degrees of
RX,RY,RZ
Freedom linked
by the element
(Minimum)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-138
ASAS (Non-Linear) User Manual
Boundary Conditions Data
Rigid Systems
RLSY
This is a 3-D pin-jointed rigid link system whereby one node can be rigidly connected to an
arbitrary number of other nodes on a structure. The single independent node must have at least
X,Y,Z degrees of freedoms. The dependent nodes will have X,Y,Z as dependent freedoms.
Since the system reduces to a triangulated series of rigid links, it may not be entirely rigid in all
three dimensions. For example, a RLSY with all nodes in a plane will not be rigid normal to the
plane. If full rigidity is required, use RBSY.
RBSY
This is a 3-D rigid-jointed rigid beam system whereby one node can be rigidly connected to an
arbitrary number of other nodes on a structure. The independent node and all dependent nodes
must have X, Y, Z, RX, RY, RZ degrees of freedom.
SBSY
This is a shell-brick interface system whereby one node on a shell element is connected to an
arbitrary number of nodes on brick elements that lie in the shell normal (thickness) direction. The
independent node must be a shell node and have X,Y,Z,RX,RY,RZ degrees of freedom. The
dependent nodes are brick nodes and will have X,Y,Z degrees of freedom.
Use of Rigid Elements
The following rules apply:
1.
All nodes used to define a rigid element must be connected to the structure. In the situation where a rigid
element is connected between a node in space and a node on the structure a dummy element must first be
used to connect the two nodes. Elements with compatible degrees of freedom must be used.
2.
Skew integers refer to the dependent node for rigid elements RLNK, RBM2, RBM3 and SBRK. Skew
integers are not valid for RLSY, RBSY and SBSY and if specified will be ignored.
3.
An independent freedom can be suppressed, displaced, or constrained; dependent freedoms cannot.
4.
The addition of rigid elements may overcome local singularity in a structure but this must be treated with
caution. See notes in Section 5.3.5.
5.
There are no limitations on the number of rigid elements joining at a node or the number of occurrences
of a dependent node.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-139
ASAS (Non-Linear) User Manual
5.4
Loading Data
Loading Data
These data blocks define the various types of loading which can be applied to the structure.
The following load types are available
Nodal loads.............. ................ ................ ................ ................ see Section 5.4.3
Prescribed displacements, velocities and accelerations ............... see Section 5.4.4
Pressure loads .......... ................ ................ ................ ................ see Section 5.4.5
Distributed loads ..... ................ ................ ................ ................ see Section 5.4.6
Temperature loads ... ................ ................ ................ ................ see Section 5.4.7
Face temperature loads ............. ................ ................ ................ see Section 5.4.8
Body force loads...... ................ ................ ................ ................ see Section 5.4.9
Centrifugal loads ..... ................ ................ ................ ................ see Section 5.4.10
Angular acceleration loads ....... ................ ................ ................ see Section 5.4.11
Nodal flux ............... ................ ................ ................ ................ see Section 5.4.12
Prescribed Field Variable ......... ................ ................ ................ see Section 5.4.13
Flux density ............. ................ ................ ................ ................ see Section 5.4.14
Wave load................ ................ ................ ................ ................ see Section 5.4.15
Tank loads ............... ................ ................ ................ ................ see Section 5.4.16
Load functions ......... ................ ................ ................ ................ see Section 5.4.17
5.4.1
UNITS Command
If global units have been defined using the UNITS command in the Preliminary data (Section 5.1.42), it is
possible to override the input units locally to load type by the inclusion of a UNITS command. The local units
are only operational for the current load type concerned and will return to the default global units when the next
load type, or loadcase, is encountered.
In general, one or more UNITS commands may appear in a data block thus permitting the greatest flexibility in
data input. The form of the command is similar to that used in the Preliminary data.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-140
Loading Data
ASAS (Non-Linear) User Manual
UNITS
unitnm
Parameters
UNITS
: keyword
unitnm
: name of unit to be utilised (see below)
Notes
1.
Force, length, temperature and angular unit may be specified. Only those terms which are required to be
modified need to be specified, undefined terms will default to those supplied on the global units definition
unless previously overwritten in the current data block.
2.
The default angular unit for all load types is radians
3.
Valid unit names are as defined in Section 5.1.42.1.
Example
Data
Operational Units
Notes
UNITS NEWTON METRE
Newtons, metres,
Global definition
END
centigrade
SYSTEM DATA AREA 5000000
PROJECT ASAS
STRUCTURE ASAS
JOB STATTITLE * EXAMPLESOLV 1.0
.
..LOAD 2
SET 1 ‘NODAL AND DISTRIBUTED LOADS’
NODAL LO
UNITS KN
X
10.0
5
6
Y
15.0
1
2
7
UNITS MM
RY
250.0
8
RZ
300.0
5
6
Kilonewtons, metres,
Note default
radians
angular unit
Kilonewtons,
Note default
millimetres, radians
angular unit
7
END
DISTRIBU
Y
BL1
1000.0
1200.0
5
6
Z
BL1
900.0
1050.0
5
6
UNITS KN
Newtons, metres,
Units revert to
radians
global units
Kilonewtons, metres
Change force
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-141
Loading Data
ASAS (Non-Linear) User Manual
Y
BL1
1.5
1.6
5
unit to KN
6
END
*
SET 2 ’DISTRIBUTED LOAD ONLY’
DISTRIBU
Z
BL5
1200.0
5
6
Newtons, metres,
New loadcase reverts
radians
units to global
END
STOP
5.4.2
LOADING Data
The loading data consists of a header keyword followed by one or more sets of load data.
LOAD
SET
(nset)
setno
(ptime)
title
loadtype
data
END
Parameters
LOAD
: compulsory header keyword to denote the start of the loading data
nset
: total number of load sets to be specified. Optional. (Integer 1-9999). If supplied, nset must equal
the number of load sets supplied.
SET
: compulsory keyword denoting the start of a load set
setno
: set number. Every set number must be unique. (Integer, 1-9999)
ptime
: pseudo time for load set, required only if loading is defined using pseudo-times. (Real)
title
: load case title. (Alphanumeric string, 40 characters)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-142
Loading Data
ASAS (Non-Linear) User Manual
loadtype : keyword to denote the start of each type of load data
END
: compulsory keyword to denote the end of the data for each load type
Notes
1.
If the load history is defined using load functions, then the load function data must be after all other
loading data have been specified.
2.
Proportional loading is assumed if there is only one load set and both pseudo-time and load function data
are absent.
3.
Title must be specified in quotes if the first word is a number.
5.4.3
NODAL LOADS Data
To define the application of nodal loads to the structure. These may be forces or moments.
NODAL LO
(skew )
dof
RP
nrep
inode
RRP
nrrep
iinode
load
//nodelist//
END
Parameters
NODAL LO
: compulsory header keyword to denote the start of nodal load data
skew
: skew system integer. (Integer)
dof
: freedom name. See Appendix -F
load
: value of nodal load. (Real)
nodelist
: list of the node numbers which are being loaded. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-143
ASAS (Non-Linear) User Manual
inode
Loading Data
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
END
: compulsory keyword to denote the end of the nodal load data for this load case
Notes
1.
Any of the degrees of freedom which exists at a node by virtue of the element types attached to it can be
loaded with nodal loads.
2.
The nodal loads are applied in the global axis system or, if a skew system has been applied in the
Boundary Condition data, in the node local axis system, as defined by that skew system.
3.
If a skew system integer is used in the nodal load data, the direction of the applied loads is the
combination of this skew system and any skew system applied in the Boundary Condition data.
4.
Use of a skew system in the nodal load data does not cause the degrees of freedom at the node to be
rotated by that amount. The nodal loads are resolved into separate components.
5.
If the same node and freedom are loaded more than once in the nodal loads for a load case, the loads are
additive.
Example
An example of a single load set consisting only of nodal loads. A point load of 25.0 is applied in the X direction
at all nodes from 1 to 150.
LOAD
1
SET
100
’TO GENERATE 150 NODAL LOADS’
NODAL L0
//
/
X
RP
RRP
END
25.0
10
15
1
1
10
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-144
Loading Data
ASAS (Non-Linear) User Manual
5.4.4
PRESCRIBED Displacements, Velocities and Accelerations Data
To define the values of displacements, velocities or accelerations to be applied in this load case to those
freedoms declared as prescribed freedoms in the Boundary Condition data (see Section 5.3.4).
PRESCRIB
(skew )
dof
prv al
RP
nrep
inode
RRP
nrrep
iinode
//nodelist//
END
Parameters
PRESCRIB
: compulsory header keyword to denote the start of prescribed freedoms data
skew
: skew system integer. Optional. (Integer)
dof
: freedom name. See Appendix -F
prval
: value of prescribed displacement, velocity or acceleration. (Real)
nodelist
: list of the node numbers to which the prescribed displacement, velocity or acceleration is to be
applied. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
END
: compulsory keyword to denote the end of prescribed freedoms data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-145
ASAS (Non-Linear) User Manual
Loading Data
Notes
1.
All freedoms used in the prescribed displacements, velocities or accelerations data must have been
defined in the prescribed freedoms data (see Section 5.3.4).
2.
In any load case, a prescribed displacement, velocity or acceleration is set to zero if it is not assigned a
value and in this case a suppression is assumed for this freedom.
3.
If a skew system has been defined in the Boundary Conditions data for a prescribed freedom node, the
same skew integer must appear in prescribed displacement, velocity or acceleration load data for that
node.
Examples
An example of prescribed displacements for two load sets. In case 1, both nodes are given equal displacement.
In case 2, node 15 is given zero displacement and has become, in effect, a suppression.
LOAD 2
SET 1 1.0
PRESCRIB
Z
Z
5.0
5.0
END
SET
2
’EQUAL DISPLACEMENT OF 5mm’
10
15
2.0
’NODE 10 DISPLACED, NODE 15 FIXED’
PRESCRIB
Z
Z
5.0
0.0
10
15
END
STOP
5.4.5
PRESSURE Load Data
To define uniform pressure or varying pressure loading applied to the faces of panel or solid elements.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-146
ASAS (Non-Linear) User Manual
Loading Data
Parameters
PRESSURE
: compulsory header to denote the start of pressure load data.
LDIR
: keyword to define direction of pressure load.
dir
: load direction. Optional. Valid names are:
GX
GY
global X direction
global Y direction
GZ
global Z direction
X
Y
local X direction
local Y direction
Z
local Z direction
Default direction is assumed if dir is omitted.
U
: keyword to define data as uniform pressure.
F
: keyword to define data as face definition.
P
: keyword to define data as nodal pressure values.
FIN
: keyword to denote the end of a block of U data, F data or P data.
END
: compulsory keyword to denote the end of the pressure load data for this loadcase.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-147
Loading Data
ASAS (Non-Linear) User Manual
Note
1.
The sign convention for pressure in the default direction on each element type is defined in the element
description sheets in Appendix -A.
2.
Local pressure load direction is only permitted for shell elements.
5.4.5.1 UNIFORM Pressure Load Data
To define values of the uniform pressure and the element faces to which they are applied.
U
(lfunno)
press
RP
nrep
inode
RRP
nrrep
iinode
//nodes//
FIN
Parameters
U
: keyword to define uniform pressure data
lfunno
: load function number; required if, and only if, LFUN specified. (Integer)
press
: value of the uniform pressure. (Real)
nodes
: the element faces to which the uniform pressure is applied. A face of an element is defined by up
to 3 corner nodes. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-148
Loading Data
ASAS (Non-Linear) User Manual
FIN
: keyword to denote the end of the uniform pressure data block
Notes
1.
A face of a panel or a face of a brick is defined by any 3 corner nodes on the face. For TRX6 and QUX8
a face is defined by the 3 nodes forming the loaded edge. For TRX3 and QUX4 a face is defined by the
two nodes forming the loaded edge and any other node on the element.
2.
For panel elements, if 2 corner nodes are supplied, pressure is applied to the edge of the element, positive
towards the centre of the element. If 3 corner nodes are supplied, pressure is applied normal to the face of
the elementin the local element axes.
3.
For coincidental faces, for example where a panel overlays the face of a brick, the program will apply the
pressure to the element with the lowest user number. The direction of the pressure load will be
determined by this element’s local axis system.
4.
See Table 6.1 for default values and Section 6.2 for the significance of some of the system parameter.
5.4.5.2 NON-UNIFORM Pressure Load Data
To define non-uniform pressure on element faces. A face can have a different value of pressure at each node.
The data required is a set of face (F) definitions followed by a set of nodal pressure values (P). Unspecified
mid-side node pressures are interpolated between adjacent corner nodes.
FACE Data
To define the element faces to which non-uniform pressure is to be applied. This data must be followed by a list
of nodal pressure values.
//nodes//
F
RP
nrep
inode
RRP
nrrep
iinode
FIN
Parameters
F
: keyword to define face data
nodes
: the element faces to which the non-uniform pressure is applied. A face is defined by up to 3
corner nodes. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-149
ASAS (Non-Linear) User Manual
Loading Data
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
FIN
: keyword to denote the end of set of face definitions
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-150
Loading Data
ASAS (Non-Linear) User Manual
PRESSURE Data
To define the nodal pressure values which are to be applied to the previously defined set of element faces.
P
(lfunno)
press
RP
nrep
inode
RRP
nrrep
iinode
//nodes//
FIN
Parameters
P
: keyword to denote nodal pressure data
lfunno
: load function number; required if, and only if, LFUN specified. (Integer)
press
: value of the pressure at the nodes. (Real)
nodes
: the nodes to which the pressure is applied. These nodes must exist on the faces defined by the
preceding set of face definitions. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment. (Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment. (Integer)
FIN
: keyword to denote the end of a nodal pressure block
Notes
1.
To define a region of non-uniform pressure, a set of one or more element faces is defined. The set of face
data is terminated by a FIN keyword. This is immediately followed by a set of nodal pressure values
which must be sufficient to completely define the pressure field over the selected faces. The nodal
pressure data is also terminated by a FIN keyword, unless it is the final set in which case it is terminated
by an END keyword.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-151
Loading Data
ASAS (Non-Linear) User Manual
2.
Regions of uniform pressure and non-uniform pressure may be mixed in any order.
3.
A face of a panel or a face of a brick is defined by any 3 corner nodes on the face. For TRX6 and QUX8
elements, a face is defined by the 3 nodes forming the loaded edge. For TRX3, and QUX4 elements, a
face is defined by the 2 nodes forming the loaded edge and any other node on the element.
Examples
Two Uniform Pressures are to be applied, a pressure of 10 over area 1-2-3-8-7-6, and a pressure of 20 over area
3-4-5-10-9-8. The following lines will generate the data.
8
7
6
p = 10
9
p = 10
1
10
p = 20
2
3
p = 20
4
5
PRESSURE
U
U
10.0
10.0
*
/
EXAMPLE OF GENERATING PRESSURE ON SEVERAL FACES
U
20.0
RP 2
END
1
2
3
2
3
4
7
8
9
1
Non-uniform Pressure on one face. The program will assign a pressure of 7.5 to node 2 and 11.0 to node 4 by
interpolation between the adjacent corner nodes.
5
6
7
p = 12
p = 10
p=5
4
8
p=5
p=5
1
p = 10
2
3
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-152
Loading Data
ASAS (Non-Linear) User Manual
PRESSURE
F
1
5
7
FIN
P
5.0
1
7
P
10.0
3
6
P 12.0
END
5
8
Example of a complete block of Pressure data for Uniform and Non-uniform Pressures
p = 20
15
20
10
13
14
7
8
1
2
10
5
15
16
17
18
9
10
11
12
3
4
5
6
PRESSURE
U
20.0
1
2
8
U 20.0
FIN
7
8
14
//
/
F
RP
2
2
3
6
RRP 3
1
9
FIN
P 20.0
2
8
14
P
P
10.0
15.0
3
5
9
11
15
17
5.0
5
6
12
4
10
16
FIN
/
U
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-153
ASAS (Non-Linear) User Manual
RP 2
END
5.4.6
Loading Data
6
DISTRIBUTED Load Data
This type of loading consists of patterns of load applied to the element as opposed to being applied to the nodes.
Distributed Loads data can contain several load patterns, and an element can be loaded with several load patterns
of the same or different types within one load set.
The following load patterns are available:
BL1
-
Linearly varying normal load or bending moment on beams
BL2
-
Linearly varying axial load or torque on beams
BL3
-
Stepped uniform load on beams
BL4
-
Partial uniform axial or normal load, torque or bending moment on beams
BL5
-
Intermediate axial or normal point load, torque or bending moment on beams
BL6
-
Partial linearly varying normal or axial load, torque or bending moment on beams
BL7
-
Partial quadratically varying normal or axial load, torque or bending moment on beams
BL8
Equal and opposite axial or normal point load, torques or bending moments on beam elements
applied at both ends
GL1
-
Linearly varying global load, torque or bending moment on beams
GP1
-
Linearly varying global load, torque or bending moment on projected length of beams
GL4
-
Partial uniform global load, torque or bending moment on beams
GP4
-
Partial uniform global load, torque or bending moment on projected length of beams
GL5
-
Intermediate global point load, torque or bending moment on beams
GL6
-
Partial linear varying global load, torque or bending moment on beams
GP6
-
Partial linear varying global load, torque or bending moment on projected length of beams
GL7
-
Partial quadratically varying global load, torque or bending moment on beams
GP7
-
Partial quadratically varying global load, torque or bending moment on projected length of beams
ML1
-
Varying shear load along the edge of membrane and shell elements
ML2
-
Varying normal load on the edge of membrane and shell elements
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-154
Loading Data
ASAS (Non-Linear) User Manual
ML3
-
Varying transverse shear load on the edge of membrane and shell elements
CB1
-
Varying distributed load on STF4
The general form of the distributed loads data block is shown below. A detailed description of each type of
distributed load and its parameters are given in the following sections. See Appendix A, element descriptions.
//nodes//
DISTRIBU
type
dof
v alues
RP
nrep
inc
RRP
nrrep
iinc
ELEM
//elno//
EDGE
//edgeno//
ELEM
//elno//
END
Parameters
DISTRIBU :
compulsory header keyword to denote the start of distributed load data.
dof
: freedom code for the direction of loading.
type
: type of distributed loading to be applied.
values
: values of force and distance to describe the loading. (Real)
nodes
: node numbers to define the loaded elements. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: element numbers to define the loaded elements. (Integer)
EDGE
: keyword to indicate following data is an edge number.
edgeno
: edge number of the element to be loaded. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol.
nrep
: the number of times the data is to be generated. (Integer)
inc
: node or element number increment to be added each time the data is generated by the RP
command. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-155
ASAS (Non-Linear) User Manual
Loading Data
RRP
: keyword to indicate the generation of data from the previous // symbol.
nrrep
: the number of times the data is to be generated. (Integer)
iinc
: node or element number increment to be added each time the data is generated by the RRP
command. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-156
Loading Data
ASAS (Non-Linear) User Manual
Example
To apply a uniformly distributed load (BL1) of 8/unit length in the local Y direction to a BM3D defined by
nodes 15 and 18.
Y BL1 8.0 8.0 15 18
Notes
1.
For BL, GL and GP type loading, the elements to which the loads relate are defined by the two end nodes.
If two or more beam elements are defined between the same two nodes (and in the same order), the
loaded element cannot be uniquely identified and the program will apply the load to the element with the
lowest user number. If this is not appropriate, the user may overcome this problem in a number of ways.
(i)
Use element number input.
(ii)
Alter the user element numbers.
(iii)
Reverse the order of the element topology and associated loading for the second beam.
(iv)
Subdivide second and subsequent elements into two or more beams.
(v)
Use different node numbering for the two beams and apply constraint equations to join them together.
2.
There is a restriction in the repeat facility where nodal type input and element type input may not be in
the same repeat block.
3.
The continuation facility is available in both nodal and element type input. However, the first line must
contain at least two nodes or one element. The continuation line must contain the keywords
ELEM/EDGE if element type input is being used.
4.
The edge number follows the topology of the element, eg edge 2 is between nodes 2 and 3 of a 4-nodal
quadrilateral element and edge 3 is between nodes 5 and 1 of a 6-noded triangular element.
Examples
DISTRIBU
ML2 10.0 10.0 10.0 EDGE
: EDGE 2 ELEM 5 6 7
1
ELEM
2
3
4
DI STRIBU
Y
:
BL6 10.0
ELEM 102
DISTRIBU
Y BL1 5.0
:
3
4
:
4
5
10.0 0.0
103 104
5.0
2
8.5
ELEM
100
101
3
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-157
ASAS (Non-Linear) User Manual
Loading Data
5.4.6.1 Local Beam Distributed Loads
The local distributed loads on beams (BL types) are applied in terms of the local axis system, with X’ along the
length of the element. A load is +ve when applied to the beam in the +ve direction of the local axis as defined
by the element topology data and geometric property data. For normal loads which are not in a local axis plane,
the appropriate components must be derived.
The Load Patterns BL1, BL2, BL6 and BL7 can be used to apply uniform load as well as linearly varying load.
The Load Pattern BL7 can be used to apply linearly varying load as well as quadratically varying load.
Load pattern BL8 is useful particularly to impose initial strain conditions such as those arising from thermal
loading when nodal temperatures are not appropriate.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-158
Loading Data
ASAS (Non-Linear) User Manual
DISTRIBUTED LOAD PATTERNS BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
on BEAM, BM2D, BM3D, TUBE
BL1
BL2
Y”
1
2
Y”
1
Normal
X”
Y”
Bending
X”
Y”
2
BL3
BL4
Axial
2
1
Torsion
X”
2
1
2
1
2
1
2
1
Torsion
X”
2
1
Normal
X”
2
1
2
1
2
1
2
Y”
Y”
Y”
1
2
Normal
X”
Y”
Y”
1
Y”
1
Axial
X”
2
Bending
X”
2
Y”
1
Y”
1
Torsion
X”
2
Y”
1
Normal
X”
2
Axial
Y”
Y”
Y”
BL7
Y”
BL8
Y”
Y”
Y”
1
Bending
X”
2
Y”
1
Torsion
X”
2
X”
Bending
X”
Torsion
X”
Normal
X”
2
Axial
X”
2
Y”
Bending
X”
Axial
1
1
Y”
X”
BL6
Normal
X”
2
Y”
Normal
X”
Axial
Y”
BL5
X”
1
1
1
1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
2
X”
Bending
X”
2
Torsion
X”
2
Page 5-159
Loading Data
ASAS (Non-Linear) User Manual
Example of Distributed Load Data for BL Patterns
34
8
p = 14
p = 10
p = 20
6
5
26
p = 16
p = 10
p = 15
4
3
9
38
2000
2000
p = 10
p = 10
1
2
Data
DISTRIBU
Y
Y
BL1
BL1
-10.0
-15.0
-15.0
-20.0
1
3
3
5
/
Y
BL1
-10.0
-10.0
2
4
RP
2
34.0
26.0
5
3
6
4
3
3
4
4
2
Y
Y
BL4
BL4
-14.0
-16.00
Y
Y
BL5
BL5
-2000
-2000
8.0
0.0
9.0
38.00
END
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-160
Loading Data
ASAS (Non-Linear) User Manual
5.4.6.1.1
BL1 and BL2 Load Patterns
Distributed Load Pattern BL1 - Linearly varying normal load or moment
Element
Valid freedom directions
Y”
Normal
BEAM
BM2D
Y”
Y”
Z”
RY”
RZ”
RZ”
BM3D
Y”
Z”
RY”
RZ”
TUBE
Y”
Z”
RY”
RZ”
1
X”
2
Y”
Bending
1
X”
2
Distributed Load Pattern BL2 - Linearly varying axial load or torque
Element
Valid freedom directions
Y”
Axial
BEAM
BM2D
X”
X”
RX”
BM3D
TUBE
X”
X”
RX”
RX”
1
X”
2
Y”
Torsion
X”
1
2
Data Line
BL1
dof
force1
//node1//
//node2//
ELEM
//elno//
force2
BL2
Parameters
dof
: local freedom code for direction of loading. See list above.
BL1
BL2
: load pattern type
force1
: force/unit length at end 1. (Real)
force2
: force/unit length at end 2. (Real)
node1
node2
: pairs of node numbers to define the elements to which this loading applies. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: list of element numbers to which this loading applies. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-161
Loading Data
ASAS (Non-Linear) User Manual
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.1
5.4.6.1.2
BL3 Load Pattern
Distributed Load Pattern BL3 - Stepped uniform normal load
Element
Valid freedom directions
BEAM
BM2D
Y”
Y”
Z”
BM3D
TUBE
Y”
Y”
Z”
Z”
Y”
Normal
1
X”
2
Data Line
dof
BL3
force1
force2
//node1//
//node2//
ELEM
//elno//
dist
Parameters
dof
: local freedom code for direction of loading. See list above.
BL3
: load pattern type.
force1
: force/unit length at end 1. (Real)
force2
: force/unit length at end 2. (Real)
dist
: distance to load step from end 1. (Real)
node1
node2
: pairs of node numbers to define the elements to which this loading applies. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: list of element numbers to which this loading applies. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-162
Loading Data
ASAS (Non-Linear) User Manual
Notes
(i)
The nodes must be listed in the same order as the element topology data.
(ii)
This loading must not be applied to stepped beams. Apply in two parts using BL4 or BL6 loading.
Example
See Section 5.4.6.1
5.4.6.1.3
BL4 Load Pattern
Distributed Load Pattern BL4 - Uniform normal or axial load, moment or torque
over a part of the element
Element
Valid freedom directions
Y”
Normal
BEAM
X”
Y”
Z”
BM2D
BM3D
X”
X”
Y”
Y”
Z”
TUBE
X”
Y”
Z”
RX”
RY”
RZ”
RX”
RY”
RZ”
RZ”
RX”
RY”
RZ”
1
X”
2
Y”
Axial
1
X”
2
Y”
Bending
1
X”
2
Y”
Torsion
1
2
X”
Data Line
dof
BL4
force
dist1
//node1//
//node2//
ELEM
//elno//
dist2
Parameters
dof
: local freedom code for direction of loading. See list above.
BL4
: load pattern type.
force
: force/unit length. (Real)
dist1
: distance to start of loaded part from end 1. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-163
Loading Data
ASAS (Non-Linear) User Manual
dist2
: distance to finish of loaded part from end 1. (Real)
node1
node2
: pairs of node numbers to define the elements to which this loading applies. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: list of element numbers to which this loading applies. (Integer)
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.1
5.4.6.1.4
BL5 Load Pattern
Distributed Load Pattern BL5 - Intermediate point load or moment
Element
Valid freedom directions
Y”
Normal
BEAM
BM2D
BM3D
X”
X”
X”
Y”
Y”
Y”
Z”
RX”
RY”
Z”
RX”
RY”
RZ”
RZ”
RZ”
TUBE
X”
Y”
Z”
RX”
RY”
RZ”
1
2
X”
Y”
Axial
X”
1
2
1
Bending
X”
2
Y”
Y”
Torsion
1
2
X”
Data Line
dof
BL5
force
//node1//
//node2//
ELEM
//elno//
dist
Parameters
dof
: local freedom code for direction of loading. See list above.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-164
Loading Data
ASAS (Non-Linear) User Manual
BL5
: load pattern type.
force
: value of the point load or moment. (Real)
dist
: distance to load point from end 1. (Real)
node1
node2
: pairs of node numbers to define the elements to which this loading applies. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: list of element numbers to which this loading applies. (Integer)
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.1
5.4.6.1.5
BL6 Load Pattern
Distributed Load Pattern BL6 -
Linearly varying normal or axial load, torque or
moment over part of the element
Element
Y”
Valid freedom directions
BEAM
BM2D
X”
X”
Y”
Y”
Z”
BM3D
TUBE
X”
X”
Y”
Y”
Z”
Z”
RX”
RX”
RX”
RY”
RY”
RY”
Normal
RZ”
RZ”
RZ”
RZ”
1
X”
2
Y”
Axial
1
X”
2
Y”
Bending
1
X”
2
Y”
Torsion
2
1
X”
Data Line
dof
BL6
force1
force2
dist1
//node1//
//node2//
ELEM
//elno//
dist2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-165
Loading Data
ASAS (Non-Linear) User Manual
Parameters
dof
: local freedom code for direction of loading. See above list
BL6
: load pattern type.
force1
: force/unit length at the start of the loaded part. (Real)
force2
: force/unit length at the end of the loaded part. (Real)
dist1
: distance to the start of the loaded part from end 1. (Real)
dist2
: distance to the finish of the loaded part from end 1. (Real)
node1
node2
: pairs of node numbers to define the elements to which this loading applies. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: list of element numbers to which this loading applies. (Integer)
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.1
5.4.6.1.6
BL7 Load Pattern
Distributed Load Pattern BL7 - Quadratically varying normal or axial load, torque or
moment over part of the element
Y”
Element
Normal
Valid freedom directions
1
BEAM
BM2D
X”
X”
Y”
Y”
Z”
BM3D
TUBE
X”
X”
Y”
Y”
Z”
Z”
RX”
RX”
RX”
RY”
RY”
RY”
RZ”
RZ”
RZ”
RZ”
2
X”
Y”
Axial
1
2
X”
Y”
Bending
1
2
X”
Y”
Torsion
1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
2
X”
Page 5-166
Loading Data
ASAS (Non-Linear) User Manual
Data Line
dof
BL7
force1
force2
force3
dist1
//node1//
//node2//
ELEM
//elno//
dist2
Parameters
dof
: local freedom code for direction of loading. See list above.
BL7
: load pattern type.
force1
: force/unit length at the start of the loaded part. (Real)
force2
: force/unit length at the centre of the loaded part. (Real)
force3
: force/unit length at the end of the loaded part. (Real)
dist1
: distance to the start of the loaded part from end 1. (Real)
dist2
: distance to the end of the loaded part from end 1. (Real)
node1
node2
: pairs of node numbers to define the elements to which this loading applies. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: list of element numbers to which this loading applies. (Integer)
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.1
5.4.6.1.7
BL8 Load Pattern
Distributed Load Pattern BL8 - Equal and opposite point loads or moments at either
end of beam
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-167
Loading Data
ASAS (Non-Linear) User Manual
Y”
Element
Normal
Valid freedom directions
1
BEAM
X”
Y”
BM2D
BM3D
X”
X”
Y”
Y”
Z”
Z”
TUBE
X”
Y”
Z”
RX”
RY”
RZ”
RX”
RY”
RZ”
RZ”
RX”
RY”
RZ”
X”
2
Y”
Axial
1
X”
2
Y”
Bending
X”
1
2
Y”
Torsion
1
2
X”
Data Line
dof
BL8
//node1//
//node2//
ELEM
//elno//
force
Parameters
dof
: local freedom code for direction of loading. See list above.
BL8
: load pattern type.
force
: value of the load or moment. This value of load is applied to the beam (not the node) in an equal
and opposite sense at each end of the beam. (Real)
node1
node2
: pairs of node numbers to define the elements to which this loading applies. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: list of element numbers to which this loading applies. (Integer)
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.1
5.4.6.2 Global Beam Distributed Loads
The global beam distributed loads (GL and GP types) are similar to the BL load types except that the loading is
applied in terms of the global axis system.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-168
Loading Data
ASAS (Non-Linear) User Manual
The load for GL type loading is applied to the beam in one of the global directions with the value of loading
defined in terms of load per unit length of the beam element.
For GP type, loading is also applied in global direction but the value of loading is defined in terms of load per
unit length measure in the plane normal to the direction of the load.
DISTRIBUTED LOAD PATTERNS GL1, GP1, GL4, GP4, GL5, GL6, GP6,
GL7, and GP7 on BEAM, BM2D, BM3D, TUBE
GL1
Global X
GP1
Global X
X”
Y”
X
X”
2
2
Y”
X
1
1
Global Z
Z
Global Z
Z
X”
X”
2
Y”
2
Y”
1
1
GL4
Global X
X”
Y”
GP4
Y”
2
2
1
X
1
X
Global RZ
X”
Z
2
Y”
Global X
X”
Global RZ
X”
Z
2
Y”
1
1
GL5
Global X
X”
Y”
2
X
1
Z
Global RY
X”
Y”
2
1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-169
Loading Data
ASAS (Non-Linear) User Manual
DISTRIBUTED LOAD PATTERNS GL1, GP1, GL4, GP4, GL5, GL6, GP6,
GL7, and GP7 on BEAM, BM2D, BM3D, TUBE
GL6
GP6
Global X
X”
Y”
Global X
X”
Y”
2
2
X
1
1
X
Global RY
Z
Global RY
Z
X”
X”
2
Y”
2
Y”
1
GL7
1
Global X
GP7
X”
Y”
X”
Y”
2
X
Global X
2
X
1
1
Global RY
Z
2
Y”
1
Global RY
Z
X”
X”
2
Y”
1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-170
Loading Data
ASAS (Non-Linear) User Manual
Example
Example of Distributed Global Loads
p = 10.0
3
p = 10.0
p = 10.0
p = 20.0
4
2
5.0
p = 17.2
Z
Y
1
X
p = 80.0
5
Global Axis Sy stem
Data
DISTRIBU
X
GP1
80.0
20.0
1
2
/
Z
GL1
10.0
10.0
2
3
RP
X
2
GL5
17.2
5.0
1
4
5
END
5.4.6.2.1
GL1 and GP1 Load Patterns
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-171
Loading Data
ASAS (Non-Linear) User Manual
Distributed Load Pattern GL1 - Linearly varying Global load or moment
Distributed Load Pattern GP1 - Linearly varying Global Projected load or moment
GL1 - Global X
X”
2
Y”
Element
BM2D
BM3D
TUBE
X
X
X
Valid freedom directions
Y
Y
Y
Z
Z
RX
RX
RY
RY
1
RZ
RZ
RZ
GL1 - Global Z
X”
Y”
X
2
1
GP1 - Global X
Z
X”
Y”
2
1
GP1 - Global Z
X”
2
Y”
Data Line
1
GL1
dof
(lfunno)
force1
force2
//node1//
//node2//
GP1
Parameters
dof
: global freedom code for direction of loading. See list above
GL1
GP1
: load pattern types
lfunno
: load function number; required if, and only if, LFUN specified. (Integer)
force1
: force/unit length at end 1. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-172
Loading Data
ASAS (Non-Linear) User Manual
force2
: force/unit length at end 2. (Real)
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.2.
5.4.6.2.2
GL4 and GP4 Load Patterns
Distributed Load Pattern GL4 - Uniform Global load or moment over a part of the
element
Distributed Load Pattern GP4
Element
- Uniform Global Projected load or moment over a part of
the element
Valid freedom directions
GL4 - Global X
X”
Y”
2
BM2D
BM3D
X
X
Y
Y
Z
RX
RY
RZ
RZ
TUBE
X
Y
Z
RX
RY
RZ
1
GL4 - Global RZ
X”
2
Y”
X
1
Z
GP4 - Global X
X”
Y”
2
1
GP4 - Global RZ
X”
2
Y”
1
Data Line
GL4
(lfunno)
dof
force
dist1
dist2
//node1//
//node2//
GP4
Parameters
dof
: local freedom code for direction of loading. See list above
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-173
Loading Data
ASAS (Non-Linear) User Manual
GL4
: load pattern type
GP4
lfunno
: load function number; required if, and only if, LFUN specified. (Integer)
force
: force/unit length. (Real)
dist1
: distance to start of loaded part from end 1. (Real)
dist2
: distance to finish of loaded part from end 1. (Real)
node1
: element node numbers. (Integer)
node2
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.2
5.4.6.2.3
GL5 Load Pattern
Distributed Load Pattern GL5 - Intermediate Global point load or moment
Element
Valid freedom directions
Global X
X”
Y”
2
BM2D
BM3D
X
X
Y
Y
Z
RX
RY
RZ
RZ
TUBE
X
Y
Z
RX
RY
RZ
1
Global Z
X”
2
Y”
X
1
Z
Global RY
X”
Y”
2
1
Global RZ
X”
2
Y”
1
Data Line
dof
GL5
(lfunno)
force
dist
//node1//
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
//node2//
Page 5-174
Loading Data
ASAS (Non-Linear) User Manual
Parameters
dof
: local freedom code for direction of loading. See list above
GL5
: load pattern type
lfunno
: load function number; required if, and only if, LFUN specified. (Integer)
force
: value of the point load or moment. (Real)
dist
: distance to load point from end 1. (Real)
node1
: element node numbers. (Integer)
node2
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.2
5.4.6.2.4
GL6 and GP6 Load Patterns
Distributed Load Pattern GL6 - Linearly varying Global load or moment over part of
the element
Distributed Load Pattern GP6 - Linearly varying Global Projected load or moment
over part of the element
Element
GL6 - Global X
X”
Valid freedom directions
Y”
BM2D
BM3D
X
X
Y
Y
Z
RX
RY
RZ
RZ
TUBE
X
Y
Z
RX
RY
RZ
2
1
GL6 - Global RY
X”
2
Y”
X
1
Z
Y”
GP6 - Global X
X”
2
1
2
Y”
Data Line
GP6 - Global RY
X”
1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-175
Loading Data
ASAS (Non-Linear) User Manual
GL6
(lfunno)
dof
force1
force2
dist1
dist2
//node1//
//node2//
GP6
Parameters
dof
: local freedom code for direction of loading. See above list
GL6
: load pattern type
GP6
lfunno
: load function number; required if, and only if, LFUN specified. (Integer)
force1
: force/unit length at the start of the loaded part. (Real)
force2
: force/unit length at the end of the loaded part. (Real)
dist1
: distance to the start of the loaded part from end 1. (Real)
dist2
: distance to the finish of the loaded part from end 1. (Real)
node1
: element node numbers. (Integer)
node2
Note
The nodes must be listed in the same order as the element topology data.
Example
See Section 5.4.6.2
5.4.6.2.5
GL7 and GP7 Load Patterns
Distributed Load Pattern GL7 - Quadratically varying Global load or moment over part
of the element
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-176
Loading Data
ASAS (Non-Linear) User Manual
Distributed Load Pattern GP7 - Quadratically varying Global Projected load or moment
over part of the element
GL7 - Global X
Element
BM2D
BM3D
X
X
Y
Y
Z
RX
RY
RZ
RZ
TUBE
X
Y
Z
RX
RY
RZ
X”
Y”
Valid freedom directions
2
GL7 - Global RY
X”
1
2
Y”
X
1
GP7 - Global X
X”
Z
Y”
2
1
GP7 - Global RY
X”
2
Y”
Data Line
1
GL7
dof
(lfunno)
force1 force2
force3
dist1
dist2
//node1//
//node2//
GP7
Parameters
dof
: local freedom code for direction of loading. See list above
GL7
: load pattern type
GP7
lfunno
: load function number; required if, and only if, LFUN specified. (Integer)
force1
: force/unit length at the start of the loaded part. (Real)
force2
: force/unit length at the centre of the loaded part. (Real)
force3
: force/unit length at the end of the loaded part. (Real)
dist1
: distance to the start of the loaded part from end 1. (Real)
dist2
: distance to the end of the loaded part from end 1. (Real)
node1
: element node numbers. (Integer)
node2
Note
The nodes must be listed in the same order as the element topology data.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-177
ASAS (Non-Linear) User Manual
Loading Data
Example
See Section 5.4.6.2
5.4.6.3 Panel Edge Distributed Loads
Distributed Load Patterns ML1, ML2 and ML3 can be applied on element types QUM4, QUM8, QUS4, TCS6,
TCS8, TCS9, TRM3, TRM6.
Load Pattern ML1 - Varying axial load along an edge
The load is positive if it acts in the direction of the order of nodes in the element topology data. For QUM8,
TCS6, TCS8, TCS9, TRM6 a quadratic variation of the load is allowed, so linear variation and uniform loading
are also acceptable. For QUS4, QUM4, TRM3 a linear variation of load is allowed, so uniform loading is also
acceptable. For a curved edge, the loading is tangential at any point.
Load Pattern ML2 - Varying normal load along an edge
The load is positive if it acts away from the centre of the element. For QUM8, TCS6, TCS8, TCS9, TRM6 a
quadratic variation of load is allowed, so linear variation and uniform loading are also acceptable. For QUM4,
TRM3, QUS4, a linear variation of load is allowed, so uniform loading is also acceptable. For a curved edge,
the loading is normal to the edge at any point.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-178
Loading Data
ASAS (Non-Linear) User Manual
Load Pattern ML3 - Varying Transverse Edge Shear Load
The load is positive if it acts in the positive local Z direction for the element.
For QUM8, TCS6, TCS8, TCS9 and TRM6 a quadratic variation of load is allowed, so linear variation and
uniform loading are also acceptable. For QUM4, QUS4 and TRM3 a linear variation of load is allowed, so
uniform loading is also acceptable. For a curved element the load is always normal to the surface of the element.
Data Line
ML1
//nodes//
ML2
force1
force2
force3
EDGE
//edgeno//
ELEM
//elno//
ML3
Parameters
ML1
: load pattern types
ML2
ML3
lfunno
: load function number; required if, and only if, LFUN specified. (Integer)
force1
: value of the load/unit length at the first corner node on the edge. (Real)
force2
: value of the load/unit length at the second corner node on the edge. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-179
ASAS (Non-Linear) User Manual
force3
Loading Data
: value of the load/unit length at the mid-side node for QUM8, TCS6, TCS8, TCS9, TRM6. This
mid-side value must be calculated and given. Any value for low order elements. (Real)
nodes
: element node list of the edge of the element to be loaded. (Integer)
EDGE
: keyword to indicate following data are edge numbers.
edgeno
: edge number of the element to be loaded. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: element numbers to define the loaded elements. (Integer)
Notes
Order of the nodes in element node list
1.
node number of first corner on the edge
2.
node number of second corner on the edge
3.
node number of any other corner on the element
Example
Example of Distributed Load Data for ML Patterns
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-180
Loading Data
ASAS (Non-Linear) User Manual
Data
DISTRIBU
ML2
-10.0
-10.0
-10.0
1
3
8
ML2
-10.0
-10.0
-10.0
6
1
3
ML2
ML2
-15.0
-21.0
-10.0
-15.0
-11.0
-18.0
11
16
6
11
8
13
ML1
ML1
-7.0
8.0
-7.0
8.0
-7.0
8.0
13
18
18
16
16
11
END
5.4.6.4 Curved Beam Distributed Loads
Distributed Load Pattern CB1 on element STF4
Normal (freedom Y’s or Z’s), axial (freedom X’s), torsional (freedom RX’s) and bending (freedom RY or RZ)
loads are allowed. The load is applied in terms of the local axis system, with X’ along the length of the element
and Y’ and Z’ as defined in Appendix -A.
Data Line
//nodes//
dof
CB1
force1
force2
force3
ELEM
//elno//
Parameters
dof
: local freedom code for direction of loading
CB1
: load pattern type
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-181
ASAS (Non-Linear) User Manual
lfunno
: load function number; required if, and only if, LFUN specified. (Integer)
force1
: value of load/unit length at end 1. (Real)
force2
: value of load/unit length at mid-side node. (Real)
force3
: value of load/unit length at end 2. (Real)
nodes
: element node list. (Integer)
ELEM
: keyword to indicate following data are element numbers.
elno
: list of element numbers to define the loaded elements. (Integer)
Loading Data
Note
The nodes must be listed in the same order as the element topology data.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-182
Loading Data
ASAS (Non-Linear) User Manual
Example
Example of Distributed Load Data for Pattern CB1
Y'
q=34.4 (uniform)
43
48
42
X'
p=3.3
p=6.6
p=9.9
Data
DISTRIBU
X
CB1
-34.4
-34.4
-34.4
42
43
48
Y
CB1
END
-6.6
-3.3
-9.9
42
43
48
5.4.7
TEMPERATURE Load Data
5.4.7.1 NODAL Temperature Data
To define the temperature values at node points throughout the structure.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-183
Loading Data
ASAS (Non-Linear) User Manual
TEMPERAT
GROU
grpno
//nodes//
temp
RP
nrep
inode
RRP
nrrep
iinode
GRES
sname
(lc)
isub
(node1)
(node2)
END
Parameters
TEMPERAT : compulsory header keyword to denote the start of the nodal temperature data
GROU
: keyword to indicate that the following temperature data applies to a single group
grpno
: group number to which temperature data applies. (Integer)
temp
: temperature value at the nodes. (Real)
nodes
: list of nodes at which the given value of temperature applies. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: number of times the data is to be generated. (Integer)
inode
: node increment to be added each time the data is generated by the RP command. (Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: number of times the data is to be generated. (Integer)
iinode
: node increment to be added each time the data is generated by the RRP command. (Integer)
GRES
: keyword to indicate reading temperatures from the database of a previous thermal analysis
sname
: 4 character structure name where temperature results are to be retrieved from.
Ic
: user load case number in the thermal analysis. By default, Ic has the same user load case
number as that specified in the stress analysis. (Integer)
isub
: the load sub-case number. Default is 0. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-184
ASAS (Non-Linear) User Manual
node1
Loading Data
: the lower limit of a node range where results will be transferred. The default value 0 means
from the lowest node on structure. (Integer)
node2
: the upper limit of a node range where results will be transferred. The default value 0 means to
the highest node on structure. (Integer)
END
: compulsory keyword to denote the end of the temperature data block
Notes
1.
Temperature values are actual temperatures. The thermal loads are calculated due to the difference
between these and the reference temperatures.
2.
Any missing corner node temperature is taken as the reference temperature.
3.
Mid-side node temperatures, whether specified or not, are always linearly interpolated between adjacent
corner nodes. For elements without mid-side nodes, the average temperature on element is taken to
calculate the thermal strain.
4.
Loading due to temperatures and face temperatures is additive at common nodes
5.
Nodal and element temperature data must not be present in the same load set.
6.
If the material properties are temperature dependent, temperature load, if specified, must be present in all
of the runs (i.e. initial and restarts). If any run does not have temperature load, then the reference
temperature should be specified in the data
7.
The following points are concerned with the usage of the GRES command.
• Temperature results must have been saved in a previous thermal analysis under the same project.
• It is assumed that all the structural corner nodes have the same node numbers as the thermal model.
• The node range data node1 and node2 enable certain nodes to be excluded from the stress analysis.
This facility is useful if non-structural nodes have been used in the thermal model, for example, to
model ambient temperature in convection or radiation boundaries.
• It is acceptable to have more than one GRES command in a local case.
• GRES can be specified together with ordinary nodal temperature data in the same load case.
5.4.7.2 ELEMENT Temperature Data
To define uniform or varying temperatures on elements. See Section 5.4.7.3 for details of uniform element
temperature data and Section 5.4.7.4 for non-uniform element temperatures data.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-185
Loading Data
ASAS (Non-Linear) User Manual
EL TEMPE
U
temp
elno
FIN
E
elno
FIN
T
temp
nodes
FIN
END
Parameters
EL TEMPE
: compulsory header to denote the start of element temperature data.
U
: keyword to define data as uniform element temperature.
E
: keyword to define data as element definition.
T
: keyword to define data as nodal temperature values.
FIN
: keyword to denote the end of a block of U data, E data, or T data.
END
: compulsory keyword to denote the end of the element temperature data block.
5.4.7.3 UNIFORM Element Temperature Data
To define values of the uniform temperature and the elements to which they apply.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-186
Loading Data
ASAS (Non-Linear) User Manual
U
temp
//elno//
RP
nrep
ielno
RRP
nrrep
iielno
FIN
Parameters
U
: keyword to define uniform temperature data.
temp
: value of the uniform temperature. (Real)
elno
: list of user element numbers to which the uniform temperature is applied. (Integer)
RP
: keyword to indicate data generation from the previous / symbol.
nrep
: the number of times the data is to be generated. (Integer)
ielno
: user element number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate data generation from the previous // symbol.
nrrep
: the number of times the data is to be generated. (Integer)
iielno
: user element number increment to be added each time the data is generated by the RRP command.
(Integer)
FIN
: keyword to denote the end of the uniform temperature data block.
5.4.7.4 NON-UNIFORM Element Temperature Data
To define non-uniform temperature on elements. An element can have a different value of temperature at each
node. The data required is a set of element (E) definitions followed by a set of nodal temperature values (T).
Mid-side temperatures are always linearly interpolated between the adjacent corner nodes.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-187
Loading Data
ASAS (Non-Linear) User Manual
ELEMENT Data
To define the elements to which non-uniform temperature is to be applied. This data must be followed by a list
of nodal temperature values.
E
//elno//
RP
nrep
ielno
RRP
nrrep
iielno
FIN
Parameters
E
: keyword to define element data.
elno
: list of user element numbers to which the non-uniform temperature is applied. (Integer)
RP
: keyword to indicate data generation from the previous / symbol.
nrep
: the number of times the data is to be generated. (Integer)
ielno
: user element number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate data generation from the previous // symbol.
nrrep
: the number of times the data is to be generated. (Integer)
iielno
: user element number increment to be added each time the data is generated by the RRP command.
(Integer)
FIN
: keyword to denote the end of set of element definitions.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-188
Loading Data
ASAS (Non-Linear) User Manual
TEMPERATURE Data
To define the nodal temperature values which are to be applied to the previously defined set of elements.
T
temp
//nodes//
RP
nrep
inode
RRP
nrrep
iinode
FIN
Parameters
T
: keyword to denote nodal temperature data
temp
: value of the temperature at the nodes. (Real)
nodes
: the nodes to which the temperature is applied. These nodes must exist on the elements defined by
the preceding set of element definitions. (Integer)
RP
: keyword to indicate data generation from the previous / symbol.
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment. (Integer)
RRP
: keyword to indicate data generation from the previous // symbol.
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment. (Integer)
FIN
: keyword to denote the end of a nodal temperature block.
Notes
1.
To define a region of non-uniform element temperature, a set of one or more elements is defined. The set
of element data is terminated by a FIN keyword. This is immediately followed by a set of nodal
temperature values which must be sufficient to completely define the temperature field over the selected
elements. The nodal temperature data is also terminated by a FIN keyword, unless it is the final set in
which case it is terminated by an END keyword.
2.
Regions of uniform element temperature and non-uniform element temperature may be mixed in any
order.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-189
Loading Data
ASAS (Non-Linear) User Manual
3.
Unspecified corner node temperatures are taken as the reference temperature.
4.
Mid-side node temperatures, whether specified or not, are always linearly interpolated between adjacent
corner nodes. For elements without mid-side nodes, the average element temperature is taken to calculate
the thermal strain.
5.
Loading due to element temperature and element face temperature are additive.
6.
If temperature is defined more than once on an element the loadings will be additive.
7.
Nodal and element temperature data must not be present in the same load set.
8.
If the material properties are temperature dependent, temperature load, if specified, must be present in all
of the runs (i.e. initial and restarts). If any run does not have temperature load, then the reference
temperature should be specified in the data.
Example
In this example 5 BM3D elements are given element temperature values. Elements 11 and 12 have a constant
temperature of 50°, element 13 varies from 50° to 75°, element 14 varies from 75° to 100° and element 15 varies
from 50° to 25°.
100
75
T=50
50
50
50
25
11
12
1
2
14
13
3
4
5
6
EL TEMPE
/
U
RP
50.0
1
2
1
FIN
/
E
RP
FIN
13
2
1
T
T
50.0
75.0
3
4
T
100.0
5
FIN
E
15
FIN
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-190
Loading Data
ASAS (Non-Linear) User Manual
T
T
50.0
25.0
5
6
END
5.4.8
FACE TEMPERATURE Data
5.4.8.1 Nodal Face Temperature
To define temperature gradients through plate and shell elements in terms of face temperatures at node points
throughout the structure.
FACE TEM
GROU
grpno
temp1
temp2
RP
nrep
inode
RRP
nrrep
iinode
//nodes//
END
Parameters
FACE TEM
: compulsory header to denote the start of nodal face temperature data
GROU
: keyword to indicate that the following face temperature data applies to a single group
grpno
: group number to which face temperature data applies. (Integer)
temp1
: temperature value on face 1. (Real)
temp2
: temperature value on face 2. (Real)
nodes
: list of nodes at which the face temperatures apply. (Integer)
RP
: keyword to indicate data generation from the previous / symbol
nrep
: number of times the data is to be generated. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-191
ASAS (Non-Linear) User Manual
Loading Data
inode
: node increment to be added each time the data is generated by the RP command. (Integer)
RRP
: keyword to indicate data generation from the previous // symbol
nrrep
: number of times the data is to be generated. (Integer)
iinode
: node increment to be added each time the data is generated by the RRP command. (Integer)
END
: compulsory keyword to denote the end of the face temperature data block
Notes
1.
The position of Face 1 and Face 2 for each element is defined in the element description sheets in
Appendix -A.
2.
Since face temperatures are applied to all elements attached to the given nodes within the specified group,
care must be taken to ensure the consistent use of local axes on adjacent elements.
3.
Loading due to temperature and face temperature are additive.
4.
Nodal and element face temperature data must not be present in the same load set
5.
Notes for temperature data also apply here.
6.
If the material properties are temperature dependent, temperature load, if specified, must be present in all
of the runs (i.e. initial and restarts). If any run does not have face temperature load, then the reference
temperature should be specified as the top and bottom surface temperatures in the data.
5.4.8.2 ELEMENT FACE TEMPERATURE Data
To define uniform or varying face temperatures on elements. See Section 5.4.8.3 for details of uniform element
face temperature data and Section 5.4.8.4 for non-uniform element face temperature data.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-192
Loading Data
ASAS (Non-Linear) User Manual
EL FACET
U
temp1
temp2
elno
temp2
nodes
FIN
E
elno
FIN
T
temp1
FIN
END
Parameters
EL FACET
: compulsory header to denote the start of element face temperature data.
U
: keyword to define data as uniform face temperature.
E
: keyword to define data as element definition.
T
: keyword to define data as nodal face temperature values.
FIN
: keyword to denote the end of a block of U data, E data, or T data.
END
: compulsory keyword to denote the end of the element face temperature data block.
5.4.8.3 UNIFORM Element Face Temperature Data
To define values of the uniform face temperatures and the element faces to which they are applied.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-193
Loading Data
ASAS (Non-Linear) User Manual
U
temp1
RP
nrep
ielno
RRP
nrrep
iielno
temp2
//elno//
FIN
Parameters
U
: keyword to define uniform face temperature data.
temp1
: temperature value on face 1. (Real)
temp2
: temperature value on face 2. (Real)
elno
: list of user element numbers to which the uniform face temperature is applied. (Integer)
RP
: keyword to indicate data generation from the previous / symbol.
nrep
: the number of times the data is to be generated. (Integer)
ielno
: user element number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate data generation from the previous // symbol.
nrrep
: the number of times the data is to be generated. (Integer)
iielno
: user element number increment to be added each time the data is generated by the RRP command.
(Integer).
FIN
: keyword to denote the end of the uniform face temperature data block.
5.4.8.4 NON-UNIFORM Element Face Temperature Data
To define non-uniform face temperature on elements. An element can have a different value of face temperature
at each node. The data required is a set of element (E) definitions followed by a set of nodal temperature values
(T) on element faces. Mid-side face temperatures are always linearly interpolated between adjacent corner
nodes.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-194
Loading Data
ASAS (Non-Linear) User Manual
ELEMENT Data
To define the element faces to which non-uniform face temperature is to be applied. This data must be followed
by a list of nodal face temperature values.
//elno//
E
RP
nrep
ielno
RRP
nrrep
iielno
FIN
Parameters
E
: keyword to define element data.
elno
: list of user element numbers to which the non-uniform face temperature is applied. (Integer)
RP
: keyword to indicate data generation from the previous / symbol.
nrep
: the number of times the data is to be generated. (Integer)
ielno
: user element number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate data generation from the previous // symbol.
nrrep
: the number of times the data is to be generated. (Integer)
iielno
: user element number increment to be added each time the data is generated by the RRP command.
(Integer)
FIN
: keyword to denote the end of set of element definitions.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-195
Loading Data
ASAS (Non-Linear) User Manual
FACE TEMPERATURE Data
To define the nodal face temperature values which are to be applied to the previously defined set of elements.
T
temp1
RP
nrep
inode
RRP
nrrep
iinode
temp2
//nodes//
FIN
Parameters
T
: keyword to denote nodal face temperature data.
temp1
: temperature value on face 1. (Real)
temp2
: temperature value on face 2. (Real)
nodes
: the nodes to which the face temperature is applied. These nodes must exist on the elements
defined by the preceding set of element definitions. (Integer)
RP
: keyword to indicate data generation from the previous / symbol.
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment. (Integer)
RRP
: keyword to indicate data generation from the previous // symbol.
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment. (Integer)
FIN
: keyword to denote the end of a nodal face temperature block.
Notes
1.
To define a region of non-uniform face temperature, a set of one or more elements is defined. The set of
element data is terminated by a FIN keyword. This is immediately followed by a set of nodal face
temperature values which must be sufficient to completely define the temperature field over the selected
elements. The nodal face temperature data is also terminated by a FIN keyword, unless it is the final set
in which case it is terminated by an END keyword.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-196
Loading Data
ASAS (Non-Linear) User Manual
2.
Regions of uniform and non-uniform face temperature may be mixed in any order.
3.
The position of Face 1 and Face 2 for each element is defined in the element description sheets in
Appendix A.
4.
Care must be taken to ensure the consistent use of local axes on adjacent elements because the definitions
of Face 1 and Face 2 are local axes dependent.
5.
Unspecified values for element corner nodes are taken as the reference temperature. Mid-side node
temperatures, whether specified or not, are always linearly interpolated between adjacent corner nodes.
For elements without mid-side nodes, the average temperature on each face is taken to calculate the
thermal strain.
6.
Loading due to temperatures and face temperatures are additive.
7.
If face temperature is defined more than once on an element, the loading will be additive.
8.
Nodal face temperature and element face temperature data must not be present in the same load set.
9.
If the material properties are temperature dependent, temperature load, if specified, must be present in all
of the runs (i.e. initial and restarts). If any run does not have temperature load, then the reference
temperature should be specified as the top and bottom surface temperatures in the data.
Example
Uniform Element Face Temperature on 4 elements
1
2
3
4
temperature on face 1 = 100.0
temperature on face 2 = 50.0
EL FACET
/
U
RP
100.0
4
1
50.0
1
END
5.4.9
BODY FORCE Data
To define forces due to linear acceleration of the structure, arising from the mass of the elements and added
masses. Only one body force loading may be defined per load set.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-197
Loading Data
ASAS (Non-Linear) User Manual
BODY FOR
x-acc
y-acc
z-acc
END
Parameters
BODY FOR : compulsory header keyword to denote the start of body force data
x-acc
: values of acceleration in the direction of the three global axes. (Real)
y-acc
z-acc
END
: compulsory keyword to denote the end of the body force data block
Notes
1.
A +ve acceleration produces +ve forces along the corresponding axis. Thus if the vertical global axis is
positive upwards, a negative value of ‘g’ is required to generate self weight.
2.
Non-zero values of density must be included for any materials used for elements whose mass is to be
included in the calculation of the body forces.
3.
Accelerations must be input in units (Length/Time2) consistent with those used for length and density.
Example
An example of a body force load set.
BODY
0.0
END
5.4.10
FOR
10.5
32.2
CENTRIFUGAL Loads Data
To define forces due to uniform rotation about a given point, arising from the mass of the elements and added
mass. Only one centrifugal loading may be defined per load set.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-198
Loading Data
ASAS (Non-Linear) User Manual
CENTRIFU
xc
yc
zc
x-vel
y-vel
z-vel
END
Parameters
CENTRIFU
: compulsory header keyword to denote the start of the centrifugal load data
xc
: global coordinates of the centre of rotation of the structure. (Real)
yc
zc
x-vel
: values of angular velocity in radians/sec about the the three global axes. (Real)
y-vel
z-vel
END
: compulsory keyword to denote the end of the centrifugal load data block
Note
Non-zero values of density must be included for any materials used for elements whose mass is to be included in
the calculation of the centrifugal forces.
Example
An example of a centrifugal load case.
CENTRIFU
17.3
103.0
96.5
0.134
0.53
0.05
END
5.4.11
ANGULAR ACCELERATION Loads Data
To define forces due to angular velocity and angular acceleration about a given point, arising from the mass of
the elements and added masses. Only one angular acceleration loading may be defined per load set.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-199
Loading Data
ASAS (Non-Linear) User Manual
ANG ACCE
xc
yc
zc
x-acc
y-acc
z-acc
(x-vel
y-vel
z-vel)
END
Parameters
ANG ACCE : compulsory header keyword to denote the start of the angular acceleration data
xc,yc,zc
: global coordinates of the centre of rotation of the structure. (Real)
x-acc
: values of angular acceleration in radians/sec2 about the three global axes. (Real)
y-acc
z-acc
x-vel
: values of angular velocity in radians/sec about the three global axes. If omitted zero is
y-vel
z-vel
assumed. (Real)
END
: compulsory keyword to denote the end of the angular acceleration data block
Notes
1.
Non-zero values of density must be included for any materials used for elements whose mass is to be
included in the calculation of angular acceleration forces.
2.
Element forces due to angular accelerations are based on the total mass of an element subject to the
velocities and accelerations pertaining at the centroid of that element. Therefore large elements
positioned close to the centre of rotation can produce significant discretisation errors.
3.
The sign convention for angular accelerations is such that input of a positive clockwise acceleration will
produce element forces acting in a counter-clockwise direction. Note, this convention is different to the
body force convention where a positive input value produces element forces in the positive direction.
Example
An example of an angular acceleration load case.
ANG
15.9
ACCE
0.0
-17.6
0.16
0.02
0.0
0.23
-0.07
0.0
END
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-200
Loading Data
ASAS (Non-Linear) User Manual
5.4.12
NODAL FLUX Data
To define the application of nodal fluxes to the structure. This load type may only be specified in a HEAT
analysis.
NODAL FL
load
dof
RP
nrep
inode
RRP
nrrep
iinode
//nodelist//
END
Parameters
NODAL FL
: compulsory header keyword to denote the start of nodal flux data
dof
: freedom name. Must be T
load
: value of nodal load. (Real)
nodelist
: list of the node numbers which are being loaded. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
END
: compulsory keyword to denote the end of the nodal load data for this load case
Note
If the same node and freedom are loaded more than once in the nodal flux data for a load case, the fluxes are
additive.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-201
Loading Data
ASAS (Non-Linear) User Manual
Example
An example of a single load set consisting only of nodal fluxes. A point flux of 25.0 is applied at all nodes from
1 to 150.
LOAD
1
SET
100
NODAL FL
1.0
’TO GENERATE 150 NODAL FLUXES’
//
/
T
RP
25.0 1
10 1
RRP
15
10
END
5.4.13
PRESCRIBED Field Variable Data
To define the field variable values to be applied in this load case to those freedoms declared as prescribed
freedoms in the Boundary Condition data (see Section 5.3.4).
PRESCRIB
dof
prv al
RP
nrep
inode
RRP
nrrep
iinode
//nodelist//
END
Parameters
PRESCRIB
: compulsory header keyword to denote the start of prescribed freedoms data
dof
: freedom name. Must be T
prval
: value of prescribed field variable. (Real)
nodelist
: list of the node numbers to which the prescribed field variable is to be applied. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-202
ASAS (Non-Linear) User Manual
inode
Loading Data
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
END
: compulsory keyword to denote the end of prescribed freedoms data
Notes
1.
All freedoms used in the prescribed field variables data must have been defined in the prescribed
freedoms data (see Section 5.3.4).
2.
In any load case, a prescribed field variables is set to zero if it is not assigned a value and in this case a
suppression is assumed for this freedom.
Examples
An example of prescribed field variable data for two loadcases. In case 1, both nodes are given equal values. In
case 2, node 15 is given a value of zero.
LOAD 2
SET
1
1.0
’EQUAL TEMPERATURE OF 5’
PRESCRIB
T 5.0 10
T 5.0
END
15
SET
2.0
2
’NODE 10 = 5 DEG, NODE 15 = ZERO’
PRESCRIB
T 5.0 10
T 0.0
END
15
STOP
5.4.14
FLUX DENSITY Data
To define uniform or varying flux density applied to the faces of panel or solid elements, or generated within an
element. This load type may only be specified in a HEAT analysis.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-203
Loading Data
ASAS (Non-Linear) User Manual
FLUX DEN
V
fden
//nodes//
fden
//nodes//
FIN
E
//nodes//
FIN
D
FIN
END
Parameters
FLUX DEN
: compulsory header keyword to denote the start of pressure load data
V
: keyword to define data as uniform flux density
E
: keyword to define data as face or element definition
D
: keyword to define data as nodal flux density values
FIN
: keyword to denote the end of a block of V data, E data or D data
END
: compulsory keyword to denote the end of the pressure load data block
5.4.14.1.1 UNIFORM Flux Density Data
To define values of the uniform flux density and the elements or element faces to which they are applied.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-204
Loading Data
ASAS (Non-Linear) User Manual
V
fden
RP
nrep
inode
RRP
nrrep
iinode
//nodes//
FIN
Parameters
V
: keyword to define uniform flux density data
fden
: value of the uniform flux density. (Real)
nodes
: the elements or element faces to which the uniform flux density is applied. An element is defined
by up to 4 corner nodes. A face of an element is defined by up to 3 corner nodes. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
FIN
: keyword to denote the end of the uniform flux density data block
Notes
1.
For surface flux, a face of a brick is defined by any 3 corner nodes on the face. For TMT6, QMT8, TXT6
and QXT8, a face is an edge defined by the 3 nodes forming the loaded edge. For TMT3, QMT4, TXT3
and QXT4, a face is an edge defined by the two nodes forming the loaded edge. Here flux density is
defined as flux per unit area.
2.
For internal flux, a brick element is defined by any 4 corner nodes on the element. The nodes must not all
lie on one face. For membrane or axisymmetric solid field elements, an element is defined by any 3
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-205
Loading Data
ASAS (Non-Linear) User Manual
corner nodes on it. The nodes must not all lie on one edge, however. Here flux density is defined as flux
per unit volume.
3.
If both surface and internal fluxes are present, they must be defined in separate data blocks.
5.4.14.1.2 NON-UNIFORM Flux Density Data
To define non-uniform flux density on elements or element faces. An element or a face can have a different
value of flux density at each node. The data required is a set of element or face (E) definitions followed by a set
of flux density values (D). Unspecified mid-side node flux densities are interpolated between adjacent corner
nodes.
ELEMENT/FACE Data
To define the elements or element faces to which non-uniform flux density is to be applied. This data must be
followed by a list of nodal flux density values.
E
//nodes//
RP
nrep
inode
RRP
nrrep
iinode
FIN
Parameters
E
: keyword to define element/face data
nodes
: the elements or element faces to which the non-uniform pressure is applied. An element is defined
by up to 4 corner nodes. A face is defined by up to 3 corner nodes (see Notes 3 and 4 in Flux
Density Data). (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-206
ASAS (Non-Linear) User Manual
iinode
Loading Data
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
FIN
: keyword to denote the end of set of element/face definitions
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-207
Loading Data
ASAS (Non-Linear) User Manual
FLUX DENSITY Data
To define the nodal flux density values which are to be applied to the previously defined set of elements or
element faces.
D
fden
RP
nrep
inode
RRP
nrrep
iinode
//nodes//
FIN
Parameters
D
: keyword to denote nodal flux density data
fden
: value of the flux density at the nodes. (Real)
nodes
: the nodes to which the flux density is applied. These nodes must exist on the elements/faces
defined by the preceding set of element/face definitions. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: the number of times the data is to be generated. (Integer)
inode
: node number increment. (Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: the number of times the data is to be generated. (Integer)
iinode
: node number increment. (Integer)
FIN
: keyword to denote the end of a nodal flux density block
Notes
1.
To define a region of non-uniform pressure, a set of one or more elements or element faces is defined.
The set of element/face data is terminated by a FIN keyword. This is immediately followed by a set of
nodal flux density values which must be sufficient to completely define the flux density field over the
selected elements/faces. The nodal flux density data is also terminated by a FIN keyword, unless it is the
final set in which case it is terminated by an END keyword.
2.
Regions of uniform flux density and non-uniform flux density may be mixed in any order.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-208
ASAS (Non-Linear) User Manual
3.
Loading Data
For surface flux, a face of a panel or a face of a brick is defined by any 3 corner nodes on the face. For
TXT6 and QXT8 a face is defined by the 3 nodes forming the loaded edge. For TXT3 and QXT4 a face
is defined by the two nodes forming the loaded edge and any other node on the element. Here, the flux
density has unit flux per unit area.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-209
Loading Data
ASAS (Non-Linear) User Manual
4.
For internal flux, a brick element is defined by any 4 corner nodes on the element. The nodes must not all
lie on one face. For membrane or axisymmetric solid field elements, an element is defined by any 3
corner nodes on it. The nodes must not all lie on one edge, however. Here the flux density has unit flux
per unit volume.
5.
If both surface and internal fluxes are present, they must be defined in separate data blocks.
Examples
Two Uniform Flux Densities are to be applied, a surface flux density of 10 over edge 1-2-3, and an internal flux
density of 20 over volume covered by 3-4-5-10-9-8. The following lines will generate the data.
8
9
10
7
6
dv = 20
dv = 20
1
2
3
4
5
ds = 10
FLUX DEN
* SURFACE FLUXES
V
10.0
1
2
V
*
10.0 2 3
FIN TO SEPARATE SURFACE AND VOLUME FLUX DATA
*
FIN
EXAMPLE OF GENERATING FLUXES ON SEVERAL FACES
*
/
INTERNAL GENERATED FLUXES
V
20.0
RP 2
END
3
4
9
1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-210
Loading Data
ASAS (Non-Linear) User Manual
Example of a non-uniform flux density on an element. The program will assign a flux density of 7.5 to node 2
and 11.0 to node 4 by interpolation between the adjacent corner nodes.
6
E 1
FIN
5
7
5.0
10.0
1
3
D 12.0
END
5
D
D
d = 10
d=5
7
6
8
5
d = 12
7
FLUX DEN
4
8 d=5
d = 10
d=5
1
2
3
Example of a complete block of flux density data for uniform and non-uniform volume flux densities
dd = 20
20
15
10
10
5
1
13
14
7
8
2
15
16
17
18
9
10
11
12
3
4
5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
6
Page 5-211
Loading Data
ASAS (Non-Linear) User Manual
FLUX DEN
V 20.0 1
V 20.0
FIN
7
2
8
8
14
//
/
E
2
3
RP 2
RRP 3
6
1
9
FIN
D 20.0
2
8
14
D
10.0
3
9
15
D 15.0
FIN
5
11
17
5
6
12
/
V
5.0
RP
2
4
10
16
6
END
5.4.15
WAVE LOAD Data
WAVE LOA
data
END
Parameters
WAVE LOA : compulsory keyword to denote start of the wave data
data
: wave load data (see Appendix -M for detailed descriptions)
END
: compulsory keyword to denote end of the wave data
Notes
1.
Wave load data should not be defined more than once in the entire load deck. The loading specified will
be applied to all load sets.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-212
Loading Data
ASAS (Non-Linear) User Manual
2.
The wave loading generated cannot be scaled using any of the load history types. The LFUN command
in the wave load data should be used instead to associate the loading with a load function.
3.
SOLU procedure cannot be used when wave load is present.
4.
If modification of wave environment is required during an analysis, this can be achieved by restart with
modified wave data supplied.
5.4.16
TANK LOAD data
To define pressure loading on the tank walls due to action of the fluid inside a tank. The specified tank load data
will be converted to pressure loads by the programe internally.
TANK LOAD
ACCN
setname
xtrans
elno
ytrans
inface
ztrans
elev
xrot
yrot
zrot
denfl
END
Parameters
TANK LOAD
ACCN
:
compulsory header to denote the start of tank load data
: command keyword to denote the start of tank acceleratio data. The accelerations will apply to
all following sets until antoher ACCN command is encountered.
xtrans
: Translational acceleration in global X direction (Real)
ytrans
: Translational acceleration in global Y direction (Real)
ztrans
: Translational acceleration in global Z direction (Real)
xrot
: Rotational acceleration about the global X axis (Real)
yrot
: Rotational acceleration about the global Y axis (Real)
zrot
: Rotational acceleration about the global Z axis (Real)
setname
: ASAS set name containing elements forming the tank (up to 8 characters)
elno
: User element number of an element in tank with known internal surface (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-213
ASAS (Non-Linear) User Manual
inface
Loading Data
: Internal fact indicator for element elno (Integer)
1
+ve local z side is internal
-1
-ve local z side is internal
elev
: Z elevation of fluid surface in tank (Real)
denfl
: fluid density (Real)
END
: compulsory keyword to denote the end of the tank load data block
Notes
1.
Both pressure and tank load data can appear in the same load case.
2.
Accelerations of the tank structure are required in the ACCN data and these are equal and opposite to
those experienced by the fluid. It is assumed that the accelerations for the whole tank are uniform and
given by the accelerations at the centre of gravity position of the fluid in the tank.
3.
The accelerations specified in an ACCN data will apply to all sets that follow the command until another
ACCN command is encountered.
4.
A positive gravitational acceleration must be added to the Z acceleration data (ztrans) in order to include
the effect of gravity. It is assumed that gravity always acts in the global Z direction.
5.
Fluid surface is assumed to remain still, i.e. sloshing effect is ignored.
6.
Tank load can only be applied to shell and membrane elements as stated in Appendix A. All other
element types in the set will be ignored.
7.
Tank pressure loads will only be calculated for the wetted nodes (i.e. nodes that are on or below the fluid
surface elevation elev).
8.
A warning will be given if the element set does not form a proper tank shape. Pressure loads will still be
calculated for the elements and this will enable the application of tank loading to other modelling
situations, e.g. applying hydostatic pressure to a wall.
9.
Each tank should only contain elements that form the surface of the tank (i.e. those that will be subjected
to internal pressure). Any stiffeners modelled by shell elements must be excluded from the tank set or
else pressure will be incorrectly applied to them. An error will be reported if a branched surface is
encountered.
10.
The tank surface must be continuous. A warning will be given if a discontinuity is encountered and only
the part containing the first element will have pressure loading applied.
Example
Tank load on set ABCD, hydrostatic pressure only.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-214
Loading Data
ASAS (Non-Linear) User Manual
TANK LOAD
ACCN
0.0
0.0
ABCD
END
100
1 20.0 1025.0
5.4.17
9.81 0.0
0.0
0.0
LOAD Functions
The load functions must follow all other other loading data.
Load functions provide a method for applying non-proportional loads. Two basic types are available; piecewise
linear and continuous. The piecewise linear type is defined as a series of ‘time-factor’ pairs. The value of the
load at time ‘time’ is the reference load multiplied by the value of ‘factor’. The continuous load function types
are defined in terms of mathematical functions. The value of the load at time ‘time’ is the reference load
multiplied by the value of the function. Load functions must not be used if pseudo-times have been used in
specifying the loading.
LOAD-FUN
lfunno
lfunno
time
factor
SINU
A
w
EXPO
a
b
POLY
c
d
RAOS
(t1)
(t2)
p
e
(t1)
(t2)
(t1)
(t2)
f
(t1)
(t2)
END
Parameters
LOAD-FUN
: compulsory header keyword to denote the start of the load function data
lfunno
: load function number. This corresponds to the load set number specified in the loading data.
(Integer)
time
: time. (Real)
factor
: multiplying factor for load at time time. (Real)
SINU
: keyword to denote continuous sinusoidal load function
A,w,p
: constants in the expression Asin(wt + p) where t is time. (Real). Note: (wt + p) is in radians
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-215
ASAS (Non-Linear) User Manual
Loading Data
t1
: time to start ramping up the load function (Real)
t2
: time to finish ramping up the load function (Real)
EXPO
: keyword to denote continuous exponential load function
a,b
: constants in the expression ae-bt where e is the base of the natural logarithm and t is time. (Real)
POLY
: keyword to denote continuous polynomial load function
c,d,e,f
: constants in the expression ct2 + dt3 + et4 + ft5 where t is time. (Real)
RAOS
: keyword to denote a RAO load function
END
: compulsory keyword to denote the end of the load function data
Notes
1.
Times must be in ascending order within each load function definition.
2.
Any number of lines may be used to identify a load function defined by time-factor pairs.
3.
The times in the list time do not have to be identical to the list of times specified with the SOLV
command. In such cases linear interpolation is used to calculate load multipliers corresponding to each
time specified with the SOLV command.
4.
Non-proportional loading cannot be used in conjunction with special solution techniques as defined by
the SOLU command.
5.
All constants (except the optional parameters t1 and t2) must be specified when using the continuous load
function types SINU, EXPO and POLY.
6.
For the special load function types, the load factor applied will be scaled by a ramping factor R. This
factor takes the following value:
R = 0.0
if t < t1
R = (t-t1) / (t2-t1) if t1 ≤ t ≤ t2
R = 1.0
if t > t2
R = 1.0 if both t1 and t2 are not specified
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-216
Additional Mass Data
ASAS (Non-Linear) User Manual
5.5
DIRECT Mass Input Data
To define mass on the structure in addition to that implied by the elements. The direct mass data consists of one
Direct Mass input header, followed by the mass data. The data consists of an input type header followed by the
appropriate data.
DIRE
LUMP
(mtype)
ADDED MA
mass
dof
nodes
END
Parameters
DIRE
: compulsory header keyword to denote the start of the Direct Mass data
LUMP
: keyword for lumped added mass input
END
: compulsory keyword to denote the end of each block of Direct Mass data
5.5.1
UNITS command
If global units have been defined using the UNITS command in the Preliminary Data (see Section 5.1.42), it is
possible to override the input units locally by the inclusion of UNITS command. The local units are only
operational for the data block concerned and will return to the default global units when the next END command
is encountered.
One or more UNITS commands may appear in a data block thus permitting the greatest flexibility in data input.
The form of the command is similar to that used in the Preliminary Data.
UNITS
unitnm
Parameters
UNITS
: keyword
unitnm
: name of unit to be utilised (see below)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-217
Additional Mass Data
ASAS (Non-Linear) User Manual
Notes
1.
The mass unit is not defined explicitly, but is derived from the force and length unit currently defined. In
order to determine the consistent mass unit the force and length terms must both be either metric or
imperial. Valid combinations are shown in Table 3.1.
2.
Force, length, and angular unit may be specified. Only those terms which are required to be modified
need to be specified, undefined terms will default to those supplied on the global units definition unless
previously overwritten in the current data block.
3.
For a list of valid unit names see Section 5.1.42.1.
5.5.2
LUMP ADDED MASS Data
To define the lumped mass input.
LUMP
ADDED MA
(mtype)
mass
RP
nrep
inode
RRP
nrrep
iinode
dof
//nodes//
END
Parameters
LUMP
ADDED MA
mtype
: compulsory header keyword to denote the start of lumped mass data
:
keyword to define that the following mass terms are to be added to any element mass
: optional keyword defining the mass usage
L
-
mass for load calculation only
M
-
mass for mass calculation only
If omitted (default), the mass will be included in all calculations.
mass
: value of the lumped mass. (Real)
dof
: freedom name to define the direction in which the mass is active. See Appendix -F
nodes
: list of node numbers to which the mass is applied. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-218
ASAS (Non-Linear) User Manual
Additional Mass Data
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: number of times the data is to be generated. (Integer)
inode
: node increment to be added each time the data is generated by the RP command. (Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: number of times the data is to be generated. (Integer)
iinode
: node increment to be added each time the data is generated by the RRP command. (Integer)
END
: compulsory keyword to denote the end of the lumped mass data block
Notes
1.
Whether or not the mass of any particular element is included depends on the setting of the mass flag in
the element topology data.
2.
Freedom name TRA may be used to assign the mass to the X, Y, Z freedoms at the nodes. Freedom
name ROT may be used to assign the mass to the RX, RY, RZ freedoms.
3.
If a node is skewed in Boundary Condition data, any added lumped mass terms input for that node are
assumed to be in the skewed directions.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-219
ASAS (Non-Linear) User Manual
5.6
Initial Conditions Data
Initial Conditions Data
These data blocks allow the user to define the initial residual stress state of the elements and the initial nodal
displacements and velocities for a transient dynamic analysis. This data is optional.
The following data blocks are available
Residual initial stresses ............ ................ ................ see Section 5.6.2
Residual initial stresses for stiffeners ........ ................ see Section 5.6.3
Initial conditions ...... ................ ................ ................ see Section 5.6.4
5.6.1
UNITS Command
If global units have been defined using the UNITS command in the Preliminary data (Section 5.1.42), it is
possible to override the input units locally by the inclusion of a UNITS command. The local units are only
operational for the data block concerned and will return to the default global units when the next END command
is encountered.
In general, one or more UNITS commands may appear in a data block thus permitting the greatest flexibility in
data input. The form of the command is similar to that used in the Preliminary data.
UNITS
unitnm
Parameters
UNITS
: keyword
unitnm
: name of unit to be utilised (see below)
Notes
1.
Force, length and angular unit may be specified. Only those terms which are required to be modified
need to be specified, undefined terms will default to those supplied on the global units definition unless
previously overwritten in the current data block.
2.
The default angular unit for all load types is radians
3.
Valid unit names are as defined in Section 5.1.42.1.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-220
Initial Conditions Data
ASAS (Non-Linear) User Manual
5.6.2
RESIDUAL Initial Stresses
This data defines a residual stress state from which the analysis is initiated. Optional.
RESI
ALL
rstv al
//elno//
inptno
RP
nrep
ielem
RRP
nrrep
iielem
END
Parameters
RESI
: compulsory header keyword to denote the start of the residual initial stress data
ALL
: keyword to indicate that all integration points for element elno have the same residual initial
stress values
inptno
: integration point number to which the following residual initial stresses apply. (Integer)
rstval
: residual initial stress values, the number of which depend upon the element type. See table below.
(Real)
elno
: element number to which the residual initial stress values apply. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: number of times the data is to be generated. (Integer)
ielem
: element number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: number of times the data is to be generated. (Integer)
iielem
: element number increment to be added each time the data is generated by the RRP command.
(Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-221
Initial Conditions Data
ASAS (Non-Linear) User Manual
END
: compulsory keyword to denote the end of the residual initial stress data
Notes
1.
The number of stress components (NST) for different element types and their orders are given in the
following table:
Element type
NST
Uniaxial
Location in vector
1
2
3
4
5
6
1
XX
-
-
-
-
-
Plane Stress
3
XX
YY
XY
-
-
-
Plane Strain
4
XX
YY
XY
ZZ
-
-
Axisymmetric
4
RR
ZZ
HH
RZ
-
-
3-D solids
6
XX
YY
ZZ
XY
YZ
ZX
Thick beams, STF4
3
XX
XY(XT)*
XZ(-)*
-
-
-
Shells
5
XX
YY
XY
XZ
YZ
* for tube or box sections, XT is the tangential shear stress component
2.
5.6.3
The stresses are defined in the stress output axis system as specified in Appendix -A.
RESIDUAL Initial Stresses for Stiffeners WST4 and SST4
This data defines the residual axial stress for stiffener elements. Optional.
The residual stress is read in for two end nodes of the element and all median points of the cross-section. For
details of median points see Geometric Property Data, see Section 5.2.5.1.
Stresses are interpolated from element end nodes to Gauss points and from median points to segment integration
points. A linear interpolation is used in both cases.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-222
Initial Conditions Data
ASAS (Non-Linear) User Manual
RESD
ND1
ND2
rstv al
//elno//
ALL
RP
nrep
ielem
RRP
nrrep
iielem
END
Parameters
RESD
: compulsory header keyword to denote the start of the residual initial stress data for stiffeners
WST4 and SST4
ND1
: keyword to indicate that the following residual stress values refer to node one
ND2
: keyword to indicate that the following residual stress values refer to node two
ALL
: keyword to indicate that the following residual stress values refer to both node one and node two
rstval
: list of residual initial axial stress values for each median point. (Real)
elno
: element number to which the residual initial axial stress values apply. (Integer)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: number of times the data is to be generated. (Integer)
ielem
: element number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: number of times the data is to be generated. (Integer)
iielem
: element number increment to be added each time the data is generated by the RRP command.
(Integer)
END
: compulsory keyword to denote the end of the residual initial stress data for stiffeners WST4 and
SST4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-223
Initial Conditions Data
ASAS (Non-Linear) User Manual
Notes
1.
The RESD data block must follow the RESI data block if both are present.
2.
If the same elements appear in both the RESD and the RESI data then the residual stress is the sum of
stress from both sets of data.
3.
Values of residual axial stress are assigned to cross-sectional median points in increasing number order.
The number of values should not exceed the number of median points for the element cross section.
Median points which are not assigned a stress value are assumed to have zero residual axial stress.
4.
Free format continuations (:) may be used but, if they are used, the keywords ND1, ND2 and ALL should
appear at the start of each new line.
5.
For any particular element, the residual axial stress values required for both ends and for all median
points must be defined at one point.
5.6.4
Initial Conditions
This data defines the initial conditions of the structure at the start of a transient dynamic or heat analysis.
Optional.
INIT
dof
disp
T
temp
//node//
v elo
//node//
RP
nrep
inode
RRP
nrrep
iinode
END
Parameters
INIT
: compulsory header keyword to define the start of the initial condition data for a transient dynamics
analysis
dof
: a freedom code. See Appendix -F
disp
: an initial displacement. (Real)
velo
: an initial velocity. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-224
ASAS (Non-Linear) User Manual
Initial Conditions Data
T
: freedom code for temperature (heat analysis only)
temp
: initial temperature
node
: list of node numbers at which the initial condition is applied. (Integer, 1-99999)
RP
: keyword to indicate the generation of data from the previous / symbol
nrep
: number of times the data is to be generated. (Integer)
inode
: node number increment to be added each time the data is generated by the RP command.
(Integer)
RRP
: keyword to indicate the generation of data from the previous // symbol
nrrep
: number of times the data is to be generated. (Integer)
iinode
: node number increment to be added each time the data is generated by the RRP command.
(Integer)
END
: compulsory word to define the end of the initial conditions
Notes
1.
If a node is skewed in the Boundary Condition data, any initial conditions specified will be assumed to be
in the skewed direction.
2.
If non-zero initial conditions are given, the first solution time must be time 0.0 for a new analysis and the
last static solution time if it is restarted from a static job.
3.
In a restart, the initial conditions specified may be total values or in addition to the previous solution. By
default, total values are assumed and Option DTRS should be set if incremental values are specified.
Example
This example gives the X freedom of nodes 1,2,3,4 an initial displacement of 0.0 and an initial velocity of 1.0.
INIT
/
X 0.0 1.0
RP 2 2
1
2
END
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-225
ASAS (Non-Linear) User Manual
5.7
STOP Data
STOP Command
To define the termination of the input data for this run.
STOP
Parameter
STOP
: compulsory keyword
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 5-226
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
STOP Data
Page 5-227
ASAS (Non-Linear) User Manual
6.
Running Instructions
6.1
DATA AREA Requirement
Running Instructions
The amount of workspace or DATA AREA specified with the SYSTEM command depends mainly on the
number of elements and nodes in the model. An analysis will abort if insufficient workspace is allocated. Some
of the data area (dependent on system parameters) is always reserved for the data-manager, (see next section).
The default value for DATA AREA is 1000000 but a higher value may be required for very large problems. The
size of the data area is defined in terms of Integer words (ie 1 word = 4 bytes). Note, the word freestore is often
used in place of data area, but both terms have the same meaning.
6.2
Data-Manager Parameters
Parameters that control the operation and efficiency of the data-manager are set by default. They are normally
adequate for most analyses, but may be insufficient for large analyses. In this case a re-analysis must be
performed and default system parameters re-set using the Preliminary Data SYSPAR command. Default values
for the system parameters are given in Table 6.1.
A certain amount of the workspace (LPGSIZ*MINPAG) is always reserved for the data-manager from the data
area allocation defined with the SYSTEM command. Both parameters MINPAG and LPGSIZ may be increased
to reduce the amount of ‘paging’ by the data-manager. This, however, will increase the demand of data area
required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-1
Running Instructions
ASAS (Non-Linear) User Manual
System
Parameter
1.
Default Size
Description
LPGSIZ
Data-manager pagesize
MINPAG
Minimum page reserve for datamanager
MANREC
Default length of sub-index
LTPAGE
Maximum length of page directory
NOPAG
Solution Blocking Factor
SMALL
MEDIUM
LARGE
256
512
1024
10
10
10
335
335
335
65535
65535
65535
10 1
10 1
10 1
NOPAG will be automatically reduced if there is insufficient freestore available.
Table 6.1 System Parameters
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-2
Running Instructions
ASAS (Non-Linear) User Manual
Default Name
Type
Description
Can Name be
Overwritten?
ZZZOARCH
External
Old Archive file
Yes
ZZZNARCH
External
New Archive file
Yes
ZZZOSTIF
External
Old Stiffness file
Yes
ZZZNSTIF
External
New Stiffness file
Yes
ZZZPORTF
External
Porthole file
Yes
ZZZMODEL
External
PATRAN/FEMVIEW Neutral
file
Yes
pnamJF**
External
Project journal file
No
INCRJF
External
Analysis journal file
No
Default Name
Default Status
Default Attribute
Deleted on
Successful
Completion?
May be
Overwritten?
ZZZOARCH
Unset
Append
No
Yes*
ZZZNARCH
New
Append
No
No
ZZZOSTIF
Old
Append
No
Yes*
ZZZNSTIF
New
Append
No
No
ZZZPORTF
New
Append
No
No
ZZZMODEL
New
Append
No
No
pnamJF**
Old
Append
No
No
INCRJF
Old
Append
No*
No
* Upon request by user
** pnam is the project name
Note
First three letters of each file name may vary from installation to installation.
Table 6.2 External Files
6.3
File Status
The names, types and contents and default attributes of all internal and external files are given in Table 6.2.
The user is cautioned that conflicts can arise if default names are used, due to files with the same name
remaining from previous runs. It is recommended that files are explicitly named.
The types, names and dispositions of all files used in an analysis are listed in the output files under the heading
FILE STATUS. Table 6.3 contains a list of possible dispositions.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-3
Running Instructions
ASAS (Non-Linear) User Manual
Mnemonic
Action
DEL
Deleted
OPEN
Open
CLSE
Closed, but not deleted
Table 6.3 Dispositions of Internal and External Files
6.4
Warnings and Errors
Errors resulting in unsuccessful analyses may result for a variety of reasons:
Data Errors
Insufficient Data Area Allocated to the Program
Backing Files Not Open Correctly
System Parameters Insufficient for Analysis
Most errors result in a controlled exit, a system abort message, a sub-routine traceback indicating the subroutine
in which the program halted and a message describing the error.
Data problems with the user may result in either error or warning messages. An error message indicates a
problem that prevents satisfactory execution of the analysis. In this case, the job will terminate after the stage
where errors are reported. Warnings indicate problems or inconsistencies with the data, but which can still allow
successful analysis. In this case the analysis will terminate before the main analysis unless the option GOON is
given with the preliminary data OPTION command.
Messages such as:
ERROR FOR UNIT 8 NAME ZZZOARCH, MODE 3, DISPOSITON 1, STATUS 0
indicate an error in opening a file (ZZZOARCH for example). Table 6.4 indicates the various possible values
for Mode, Disposition and Status.
Occasionally large analyses may fail because the default system parameters are insufficient for the analysis (see
Section 6.2).
Parameter
Value
MODE
1
3
DISPOSITION
1
2
3
STATUS
various
Description
Existing File
New File
Machine dependent error code.
See specific machine documentation
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-4
Running Instructions
ASAS (Non-Linear) User Manual
Table 6.4 Mode, Disposition and Status of Files
If a premature exit is made from ASAS-NL, then there will be an internal file called pnamJF (pnam is the project
name), created which indicates the stage the program had reached when the exit was made. The different stages
are given in Table 6.5.
Stage Number
Description
1
Read and echo data. Preliminary checking
2
Check and print data
3
Determine the parameters for solution process
4
Main analysis
Table 6.5 Stage Numbers for ASAS-NL
If a premature exit is made within the main analysis (i.e. stage 4), a journal file called INCRJF will also be saved
indicating the current increment and iteration being analysed when the exit was made.
6.5
Running Instructions
The program ASAS-NL is required to run an ASAS-NL analysis. In addition, if a restart is attempted, the datamanager oldarchive file and stiffness matrix oldarchive file must be present in the default directory (these files
are named with the FILE commands).
The instructions to run ASAS-NL have been kept to a minimum with all file assignments being initiated from
within the program as the run proceeds.
The PC version of ASAS-NL is run as a Windows process. The program is issued with an accompanying icon
which may be displayed on the main Windows desktop. There are three ways in which a program may be run
1. Click on the Program Icon
By clicking on the program icon, the following form will be displayed:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-5
ASAS (Non-Linear) User Manual
Running Instructions
The data file name may be identified by clicking on the Browse button. A file structure will be displayed from
which the data file may be identified. Double clicking on the file will place it in the Data File Name display box.
Alternatively, the data file name and its path may be typed in the display box. By default, the analysis will be run
in the directory defined by the path to the data file.
Command line parameters can be defined in this display box. The following parameters may be used to define
the location of files:
/DATA=
will define the name of the data file and, optionally, its location. By default .dat will be appended
if no file extension is given.
/OUT=
will define the name of the results file and, optionally, its location. By default this will be set to the
data file prefix appended with .out, e.g. for an input file of hull.dat the results file will be hull.out.
/PATH=
will define the path to the data and results file.
This will be used if there is no path defined on /DATA= or /OUT=
/BACK=
will define the directory in which the analysis is to be run.
This may be different from the location of the data and results files.
/CLEAR
will clear the dialog window. The default is for it to remain in position at the end of the run.
/LOCK
will write a lock file. This may be interrogated with the WAITLOCK process to determine when
the process has completed. See note below.
/EXPAND
will expand all @ files, resolves all IF/THEN/ELSE references, and carries out all data
replacements (see below). This generates a new data file with a .exp extension. Note that the use of
/EXPAND does not run the program itself, rather it is a pre-processor for generating expanded
data.
Parameters must be separated by a space on the command line.
To start the analysis, click on the OK button. This will display a dialog window similar to that shown below:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-6
ASAS (Non-Linear) User Manual
Running Instructions
At the end of the run a message is displayed that the analysis has completed and requests an Exit confirmation.
Clicking on ”Yes” or pressing the enter key on the keyboard will close the dialog window. Clicking on ”No” will
allow the window to be processed according to the command buttons. Note that the use of /CLEAR
automatically closes the dialog window when the analysis has completed.
2. Drag and Drop
Using Windows Explorer, a data file may be dragged and dropped on the program icon. This will automatically
initiate the analysis in the directory of the data file. To run ASASNL, drop the data file onto the ASASNL icon.
3. Using a Windows Command Prompt
The program can be run in a Windows Command Prompt using a command of the form:
asanl DataFileName
or
asasnl /DATA=DataFileName /OUT=ResultsFileName [/parameter]
assuming the directory where the program is installed (e.g. c:\asash) in on the path correctly. The optional
/parameter equates to any of the valid command line parameters given above e.g. /CLEAR, /PATH=c:\asash\test.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-7
Running Instructions
ASAS (Non-Linear) User Manual
Typing the program name on its own is equivalent to clicking on the program icon as described above.
It is not now possible on the PC to use the redirect symbols < and > to define data and results files.
Running ASAS-NL from batch files on PCs
As ASAS-NL now runs as a process, it may not be possible for a number of jobs to be run consecutively. This is
because when a command is issued to start an ASAS-NL run, the process begins and control may return
immediately to the DOS shell or the .BAT file. So, if a .BAT file is being used, as each process begins, control is
returned to the file and the next command is executed.
This has been overcome in the ASAS suite of programs with the use of a LOCK file. If the /LOCK parameter
(see above) is used, a file called $_$_LOCK is created. A program WAITLOCK has been written that can then
be run following an ASAS program. This program will wait until the LOCK file has been deleted, which occurs
when the preceding ASAS run completes. When the LOCK file has been deleted, WAITLOCK itself completes
and allows the next command to be executed.
Example Batch File
ASASNL
hull /LOCK
WAITLOCK
6.6
ASAS Initialisation File
The ASAS initialisation file allows the user to define the default file extensions to be used. The file is called
asas.ini. There are three locations in which the file may be stored. These are searched in the following order:
1.
In the current directory
2.
In a directory pointed to with the environmental variable ASAS_INI.
3.
In a directory pointed to with the environmental variable ASAS_SEC.
Currently, the following data items may be defined in the asas.ini file.
The first line must be [General] starting in column 1.
The next lines may be one or more of the following, all starting in column 1:
Default_input_extension=ext
where ext is the user’s preferred extension for the input file.
Default is .dat
Default_output_extension=ext
where ext is the user’s preferred extension for the output
file.
Default is .out
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-8
Running Instructions
ASAS (Non-Linear) User Manual
Noclobber=on (or ON or On)
prevents the output file from being overwritten if it already
exists in the current directory.
The two default extensions will only be used if no extension is given for either input or output files on the
command line, eg
asasnl.exe
hull
The output default extension will also be used if the input file name is specified with an extension and no output
file is specified on the command line, eg
asasnl.exe
6.7
hull.dat
Extended Syntax in Data Files
6.7.1
IF/THEN/ELSE
ASASNL data is often very similar for several runs. Differences can occur when data is used for linear and
dynamic analysis, when two similar components are being created or different loading is required in a series of
runs. These similarities will vary for each different user.
The IF/THEN/ELSE feature allows the user to create a path through a data file conditional upon one or more
pieces of key data on the command line or embedded within the data.
This feature is best described with an example of a linear and a natural frequency run.
The three columns below describe the two separate sets of data, and then how they can be merged together.
Static Data
Transient Data
Merged Data
job stat
job tran
if static then
job stat
else
job tran
endif
project test
project test
project test
options nobl
options nobl
options nobl
save new 1. 2. 3. 4.
if static then
else
save new 1. 2. 3. 4.
endif
coor, elem, mate, geom
coor, elem, mate, geom
coor, elem, mate, geom
supp, disp, load
supp, disp, load
supp, disp
resi
if static then
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-9
Running Instructions
ASAS (Non-Linear) User Manual
else
resi
endif
stop
stop
stop
Note: In this example, coor, elem, load, etc represent complete sets of data.
The command line to run this data would be either:
asasnl.exe
hull /static for a static run
asasnl.exe
hull /#static
or
for a transient run
Thus any parameter after a /, except the reserved parameters listed in section 6.5, is treated as a logical
parameter. This takes the value true if on its own, or false if preceded by #.
This has been extended to allow for testing against a value, as in the following example:
Static Data
Transient Data
Merged Data
job stat
job tran
if save#tran then
job stat
else
job tran
endif
project test
project test
project test
options nobl
options nobl
options nobl
save new 1. 2. 3. 4.
if save=tran then
save new 1. 2. 3. 4.
else
endif
etc
etc
etc
The command line to run this data would be either:
asasnl.exe hull
/save=tran for a transient run
or
asasnl.exe hull
for a static run
Thus the parameter following / may be of the form:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-10
Running Instructions
ASAS (Non-Linear) User Manual
/param
param is true when encountered in the data
/#param
param is false when encountered in the data
/param=value
param is true in the data if it equals value
/param#value
param is false in the data if it does not equal value
Any parameters not defined on the command line are assumed to be false.
Then in the data, the test following IF and ELSEIF is
IF param THEN
the lines of data following are used if param is true
IF #param THEN
the lines of data following are used if param is false
IF param=value THEN
the lines of data following are used if param equals value
IF param#value THEN
the lines of data following are used if param does not equal value
The full sequence of possible IF/THEN/ELSE statements is:
IF logical1 THEN
these lines are used if logical1 is true
ELSEIF logical2 THEN
these lines are used if logical2 is true
ELSEIF logical3 THEN
these lines are used if logical3 is true
ELSE
these lines are used if none of the above is true
ENDIF
The ELSE command is not mandatory, but if it is omitted, then there could be situations when none of the lines
is used between the IF and ENDIF.
There is no limit to the number of ELSEIF statements. Nesting up to five levels may be used.
Note that it is important that there must be no embedded spaces in the parameter test.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-11
ASAS (Non-Linear) User Manual
6.7.2
Running Instructions
DATA REPLACEMENT
Specified character strings in the data may be replaced with values defined on the command line.
Consider the following data file:
job stat
project %proj
options nobl
end
coor, elem, mate, geom, supp, disp decks
load 1
case 1 Point load of %load
nodal lo
z %load 200
end
stop
Then the command line would be, for example:
asasnl.exe hull %proj=a001 %load=5000
When interpreting the data, each time %proj was encountered, it would be replaced by the characters a001, and
%load replaced by the characters 5000.
To maintain compatibility between UNIX and the PC, the $ may be used instead of %. The two characters are
completely interchangeable and the existence of one implies also the existence of the other. Thus the command
line could be:
asasnl.exe hull $proj=a001 $load=5000
It should be noted that if any of the replacement strings is not satisfied in a data file a warning will occur for
each one. Processing will continue, but there will probably be errors in the data where the unsatisfied
replacement strings are being interpreted.
6.7.3
The DEFINE Command
The command line data may be embedded within the data file itself by using a DEFINE command. This has the
same effect as setting logical values on the command, but they can change during the processing of the file. For
example:
define %proj=a001
define %load=5000
job stat
project %proj
options nobl
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-12
ASAS (Non-Linear) User Manual
Running Instructions
end
etc
When the data is interpreted, the replacement strings would take the values as on the define lines. However, they
may be overridden by a different value on the command line. The command line value takes precedence if a
string replacement is used on a command line and also on a DEFINE command. Thus, if the command line had
been:
asasnl.exe hull %proj=a002
then the project would have been interpreted as project a002 instead.
The DEFINE commands do not have to be placed at the start of the data file. They may occur anywhere prior to
the first use of the parameter.
6.8
Secondary Data Files within ASAS-NL Data
The command @filename may appear anywhere in a data file. When such a command is encountered, the
input of data switches to the file filename and data continues to be read from that file until either the end-offile is reached or an @ command is encountered in the secondary file.
When the end of the secondary file is reached, that file is closed and input switches back to the previous data
file. If, however, an @ command is found in the secondary file, input switches to yet another file. This process
can continue until a maximum of 5 secondary files are open simultaneously.
6.8.1
Use of @filename command
There are many ways in which such a facility can be used, some examples of which are listed below.
(a)
The user may prepare each data block in a separate file and these files may then be referenced by a simple
main datafile which consists of @ commands only.
For example, hull.dat may contain the lines
@prelim.dat
@phase1.dat
@phase2.dat
@load.dat
phase1.dat may then contain
@coor.dat
@elem.dat
@mate.dat
@geom.dat
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-13
Running Instructions
ASAS (Non-Linear) User Manual
Finally,
coor.dat contains the coordinate data
elem.dat contains the element data
etc.
(b)
The user may prepare his data as in example (a) above but may have a number of variants of some of the
data blocks, for example, geometry data, support data and load data.
A number of small data files containing @ commands can be prepared to pull together the various data
blocks in whatever combinations may be required.
(c)
The user may have a block of data, such as some loading data which he needs to repeat in a number of
different loadcases. If these data are stored in a file, for example pressure.dat, they may be read at
any point by including a command @pressure.dat.
(d)
On some computers, the file editors may not handle very long files conveniently. In such cases the data
file may be split into convenient sections for editing without the need to recombine into one file before
the analysis run.
6.8.2
1.
Notes about the @ Command
The filename on the @ command line may be up to 79 characters long . This name may include the path
name to the directory as well as the filename.
Examples of the @ command
(a)
@coor.dat
-
(b)
@
- spaces are allowed between @ and filename
(c)
@/asasdata/coor.dat - an absolute path (/asasdata) is included
(d)
@bridge/coor
-
reference to a subdirectory (bridge) is included
(e)
@h:\data\coor
-
reference to a different drive and directory on a PC
(f)
@..\data\coor
-
reference to a directory relative to the current directory
coor.dat
switch to file coor.dat
2.
@ may be nested to a depth of 5 secondary files open at any one time in addition to the main data file.
3.
A secondary file is closed when the end-of-file is reached whereupon control returns to the line following
the @ command in the higher level data file.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-14
ASAS (Non-Linear) User Manual
4.
Running Instructions
Any one file may be opened several times in one run using @ commands, provided that it has been closed
before being accessed for a second time.
Conversely, no file may be opened more than once within a given nesting of @ commands. (Recursion is
not allowed).
5.
A secondary file which contains all or part of the preliminary data must not also contain any other data,
such as coordinates or elements. Such a secondary file must terminate at or before the END command for
the preliminary data.
6.9
Soft Halt Facility
There may be occasions when it is desirable to halt an analysis before all increments have been completed. This
may be achieved by creating a file named ZZZSHALT in the directory in which the program is running. At the
completion of each increment, ASASNL checks for the existence of this file and terminates accordingly.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page 6-15
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Running Instructions
Page 6-16
Appendix A
ASAS (Non-Linear) User Manual
Appendix - A
A.1
Element Description Sheets
Facilities Available for each Element Type
This Appendix contains a detailed description of each of the finite element types within ASAS-NL, arranged in
alphabetical order. They can be grouped as follows:
Stress/structural elements
Uniaxial
FLA2
Plane Strain/Plane Stress
TRM3, QUM4, TRM6, QUM8
Axisymmetric Solid
TRX3, QUX4, TRX6, QUX8
3-D Solid
BRK6, BRK8, BR15, BR20
3-D Laminated Solid
LB15, LB20
Shell/Plate
QUS4, TCS6, TCS8, TCS9
Beam/Stiffener
STF4, BEAM, BM2D, BM3D, TUBE
Beam/Stiffener of arbitrary
SST4, WST4
(open) cross-section
Gap
GAP2, GAPX, GAPR
Spring/Dashpot
SPR1, SPR2
Rigid surface interface
RGX3, RGX4, RG23, RG24
Linespring
LSP3, LSP6
Field elements
Uniaxial
FAT2, FAT3
2-D Plane
TMT3, QMT4, TMT6, QMT8
Axisymmetric Solid
TXT3, QXT4, TXT6, QXT8
3-D Solid
BRT6, BRT8, BT15, BT20
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-1
ASAS (Non-Linear) User Manual
Appendix A
The following chart summarises the facilities available to each element.
Following the chart is a description of rigid offsets for beams.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-2
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix A
Page A-3
ASAS (Non-Linear) User Manual
Material Models
Elem.
Type
Elastic
Iso.
Hype
.
Aniso/
Orth/
Wove
n
Plastic
Lami.
Field
von
Mises
Tresca
Mohr/Dru
c
Tension
Ivanov
Cut-off
Fail
Spring
Coul.
Frict.
Kine.
Hard.
Creep
von
Mises
Tangent
Stiffness
Large
Disp.
Geom.
Stiff
Cent.
Stiff
Press.
Stiff
Mass
Matrix
Skew
Sys.
BEAM
♦
♦
♦
♦
♦
♦
BM2D
♦
♦
♦
♦
♦
♦
BM3D
♦
♦
♦
♦
♦
♦
BRK6
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
BRK8
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
BRT6
1x1x2
2x2x2
1x1x2
♦
BRT8
Default
Int. Rule
2x2x2
BR15
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
BR20
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
1x3x2
2x2x2
BT15
♦
1x3x2
BT20
♦
2x2x2
FAT2
♦
1x1x1
FAT3
♦
♦
2x1x1
FLA2
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
GAP2
♦
GAPR
♦
♦
GAPX
♦
♦
♦
LB15
♦
♦
♦
♦
♦
♦
♦
1x3x1 per layer
LB20
♦
♦
♦
♦
♦
♦
♦
2x2x1 per layer
LSP3
♦
♦
3x1x1
LSP6
♦
♦
3x1x1
QMT4
♦
QMT8
♦
2x2
2x2
Page A-4
QUM4
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
QUM8
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
2x2
QUS4
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
1x1x3
QUX4
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
2x2
QUX8
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
2x2
♦
♦
♦
♦
♦
Table A.1 Facilities available to each element type
2x2
ASAS (Non-Linear) User Manual
Load Types
Elem.
Type
Nodal
Loads
Presc.
D,V,A
BEAM
♦
BM2D
♦
BM3D
Press.
Loads
Dist.
Loads
Temp
.
Loads
♦
♦
♦
♦
♦
♦
♦
BRK6
♦
♦
BRK8
♦
♦
Face
Temp
.
Cent.
Loads
Body
Force
s
Ang.
Acce.
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
Nodal
Flux
Presc.
Field
Flux
Dens.
BRT6
♦
♦
♦
BRT8
♦
♦
♦
BT15
♦
♦
♦
BT20
♦
♦
♦
FAT2
♦
♦
♦
♦
QMT4
♦
♦
♦
QMT8
♦
♦
♦
BR15
♦
♦
♦
♦
♦
♦
♦
BR20
♦
♦
♦
♦
♦
♦
♦
Tank
Loads
FAT3
FLA2
♦
♦
GAP2
♦
♦
GAPR
♦
♦
GAPX
♦
♦
LB15
♦
♦
LB20
♦
♦
LSP3
♦
♦
LSP6
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
Page A-5
QUM4
♦
♦
♦
♦
♦
♦
♦
♦
♦
QUM8
♦
♦
♦
♦
♦
QUS4
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
QUX4
♦
♦
♦
♦
♦
♦
♦
♦
QUX8
♦
♦
♦
♦
♦
♦
♦
♦
Table A.1 Facilities available to each element type (cont.)
ASAS (Non-Linear) User Manual
Material Models
Elem.
Type
Elastic
Iso.
Hype
.
Aniso/
Orth/
Wove
n
Plastic
Lami.
Field
QXT4
♦
QXT8
♦
von
Mises
Tresca
Mohr/Dru
c
Ivano
v
Fail
Spring
Coul.
Frict.
Kine.
Hard.
Creep
von
Mises
Tangent
Stiffness
Large
Disp.
Geom.
Stiff
Cent.
Stiff
Press
Stiff
Mass
Matrix
Skew
Sys.
Default
Int. Rule
2x2
2x2
RGX3
♦
♦
♦
♦
2x1x1
RGX4
♦
♦
♦
♦
3x1x1
RG23
♦
♦
♦
♦
2x1x1
RG24
♦
♦
♦
♦
3x1x1
SPR1
♦
SPR2
♦
SST4
♦
♦
STF4
♦
♦
♦
TCS6
♦
♦
♦
♦
♦
♦
♦
TCS8
♦
♦
♦
♦
♦
♦
♦
TCS9
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
2x3x3 Rect
2x8x1 Tube
2x12x1
Box
♦
♦
♦
♦
♦
♦
♦
♦
1x3x3
♦
♦
♦
♦
♦
♦
♦
♦
2x3x3
♦
♦
♦
♦
♦
♦
♦
♦
2x3x3
♦
♦
TMT3
1x1
♦
TMT6
1x3
TRM3
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
1x1
TRM6
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
1x3
TRX3
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
1x1
TRX6
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
1x3
TUBE
♦
♦
♦
♦
TXT3
♦
TXT6
♦
Page A-6
WST4
♦
♦
1x1
1x3
♦
♦
♦
♦
Table A.1 Facilities available to each element type (cont.)
♦
♦
ASAS (Non-Linear) User Manual
Load Types
Elem.
Type
Nodal
Flux
Presc.
Field
Flux
Dens.
QXT4
♦
♦
♦
QXT8
♦
♦
♦
TMT3
♦
♦
♦
TMT6
♦
♦
♦
TXT3
♦
♦
♦
TXT6
♦
♦
♦
RGX3
Nodal
Loads
♦
Presc.
D,V,A
♦
♦
RG23
♦
♦
RG24
♦
♦
SPR1
♦
♦
SPR2
♦
♦
SST4
♦
♦
STF4
♦
♦
TCS6
♦
♦
TCS8
♦
TCS9
♦
♦
Dist.
Loads
Temp.
Loads
Face
Temp.
Cent.
Loads
Body
Forces
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
♦
TRX3
♦
♦
♦
♦
♦
♦
♦
TRX6
♦
♦
♦
♦
♦
♦
♦
TUBE
♦
♦
♦
♦
♦
♦
♦
Tank
Loads
♦
♦
TRM6
WST4
Ang.
Acce.
♦
RGX4
TRM3
Press.
Loads
♦
♦
♦
♦
♦
Notes
Page A-7
1.
Elastic material data must be supplied.
2.
The geometric stiffness is invoked by directive LARGe with the Problem or Group Title commands. The centrifugal stiffness is included by default if the
structure is spinning. Symmetrized load stiffness is included by default if the structure is subject to pressure loading.
Table A.1 Facilities available to each element type (cont.)
ASAS (Non-Linear) User Manual
A.2
Appendix A
Element Axes Systems
All elements have some form of local element axes system associated with them. These are used for the purpose
of defining material axes and element related loading and also for the calculation and display of stress results. For
some elements the global axes system is used as the element local axis system. All other elements have a local
system (as defined in the element description sheets which follow) normally based on the order in which the
element nodes are specified in the element topology data. The general rules used for defining the local axes for
elements of certain types are outlined in the following sections.
It must be noted that adjacent elements not using the global axes system can have a completely different
orientation of local axes system. For this reason the nodal stress/force results on adjacent elements may not be
averaged directly but must be re-orientated into a consistent axes system first. This type of re-orientation may be
conducted for the shell elements by the post processor POSTNL.
A.2.1 Local Axes on Beam Elements
The beam elements have the local X direction along the axis of the beam from the first node towards the last node.
The local Y and Z axes are normal to the beam axis and defined according to element specific rules (as described
in the individual element description sheets). For beam element types BM3D and TUBE the local Y and Z
directions may be explicitly defined in the geometric property data for the element by specifying the plane
containing the local Y or Z direction. For a TUBE element, the local axis definition may be omitted, in which
case a default local axis system is used. See TUBE element description sheets.
The planes of the local Y and Z axes may be defined by one of the following methods:
COOR command (Default)
This gives the coordinates of a point in the local XY plane with the local Y axis positive towards this point
from end 1 of the element. If command XZ is also present, the point defines the local XZ plane with local
Z positive towards the point.
NODE command
This works in the same way as for COOR except that the node number of a point with the required
coordinates is given.
BETA command
This gives an angle through which the default local Y and Z axes are to be rotated about the element local
X axis. The default axes for BM3D assume the coordinate point in the local XY plane (XZ plane if
command XZ is present) to be the origin, and for the TUBE are as given when the coordinate point is
omitted.
GPOS, GNEG commands
This gives an axis X,Y or Z which will be taken as a vector lying in the required local XY plane. The
GPOS or GNEG keyword gives the positive or negative global direction as defining the positive direction
for the local Y axis so defined. If command XZ is also present, then the vector lies in the required local XZ
plane and the GPOS or GNEG defines the direction for the positive local Z axis.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-8
ASAS (Non-Linear) User Manual
Appendix A
SPOS, SNEG commands
This gives a skewed X,Y or Z axis, which will be taken as a vector lying in the required local XY plane.
The SPOS or SNEG keyword and the skew system integer gives the positive or negative skewed global
direction as defining the positive direction for the local Y axis so defined. If command XZ is also present,
then the vector lies in the required local XZ plane and the SPOS or SNEG defines the direction for the
positive local Z axis.
VECT command
This gives the coordinates of a point defining a vector from the origin, lying in the required local XY plane
with the local Y axis positive in the direction of the vector. If command XZ is also present, then the vector
defines the required local XZ plane with the local Z axis positive in the direction of the vector.
These are shown diagrammatically in the following table.
For a further description of data formats see Section 5.2.5.5.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-9
Appendix A
ASAS (Non-Linear) User Manual
X'
node2
X'
node2
Y'
(10,20,0)
node1
Z'
(10,20,0)
node1
Z'
Y'
COOR 10 20 0 [XY]
COOR 10 20 0 XZ
Z'
501
Y'
501
X'
node2
X'
node2
Y'
node1
node1
Z'
NODE 501 XZ
NODE 501 [XY]
Y'
node1
default Y'
Y'
X'
node2
Z'
node1
β=35°
β=35°
default Y'
β
default Z'
default Z'
BETA 35 [XY]
Z'
BETA 35 XZ
Y
Y
X
Y'
X'
node2
Y'
X'
node2
Z
X'
node2
X
Z
node1
node1
Y'
Z'
GP OS Y [XY]
Y
Y
Ys
Ys
Xs
X
Z
GNEG Y XZ
Z'
Zs
Y'
Z'
node1
X'
node2
Xs
X
Z
X'
node2
node1
Z'
node1
SNEG 1 Z [SY]
Y' |5,4,3|
Zs
Y'
Y'
Z'
X'
node2
SP OS 1 X XZ
|5,4,3|
X'
node2
node1
Z'
VECT 5 4 3 [XY]
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
VECT 5 4 3 XZ
Page A-10
Appendix A
ASAS (Non-Linear) User Manual
A.3
Beam Offsets
The element types BEAM, BM2D, BM3D, and TUBE can have rigid offsets defined at each node.
It is normally assumed that a beam member has its centroidal axes lying along the line joining the two end nodes
and that it is flexible throughout its length. Often, however, this is not the case. Sometimes the centroidal axis is
offset from this line. It may also be appropriate when modelling the intersection of two beams at a node to
consider the end portion of one of the beams to be rigid.
Rigid offsets may be defined by the OFFG, OFFS, OFSK or OFCO command in the Geometric Properties Data
(Section 5.2.5). The offset command for an element occurs after the Geometric Properties commands for that
element.
One command is required for each set of geometric property data which describes a member with offsets
An offset beam element has two local axis systems. Local X’,Y’,Z’ refer to the node points used to define the
element and X”,Y”,Z” refer to the physical ends of the element centroidal axis after the offsets have been taken
into account. If the member has no offsets then X’,Y’,Z’ and X”,Y”,Z” are coincident.
Y'
Y”
Node2
X'
Node1
Z'
End1
End 2
X”
Z”
Figure A.1 Local Axes for a Beam with Offsets
A.3.1 OFFS Command
For the OFFS command, the local offsets are defined as the distances from the physical ends of the member
centroidal axes to the nodes, measured in the local X’,Y’,Z’ axes system.
Positive values of the local offsets ex, ey, ez, are as shown:
Y'
Y”
Node1
ex
Y'
Node 2
X'
ey
ey
Node 1
Z'
ez
ey
ex
X”
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-11
Appendix A
ASAS (Non-Linear) User Manual
Figure A.2 Beam Offsets Defined using OFFS
Notes
1.
ex at node 2 is measured in the negative x’ direction such that a shortening at either end of the beam is
given by a positive ex value.
2.
The command has the keyword OFFS and the six offset values ex, ey, ez values for node 1 followed by ex,
ey, ez values for node 2.
3.
For BM2D element, 4 values of offset are required, ex, ey values for node 1 followed by ex ey for node 2
Example
Example of an Offset BM3D
175
BM3D
:
:
OFFS
17.5
145.0
97.3
0.0
225.0
1107.0
12.7
4.3
0.0
5.7
0.0
0.0
0.0
4.3
0.0
A.3.2 OFFG and OFSK Commands
For the OFFG and OFSK commands, the offsets are defined as the distances from the nodes to the physical ends
of the member centroidal axis, measured in the global or skewed global axes system.
Y
ex (-ve)
ey
Y
ex
Node 2
ez
ey
ey
Node1
Node 1
X
Z
Figure A.3 Beam Offsets Defined using OFFG or OFSK
Notes
(i)
The OFFG command has the keyword OFFG and the six offset values ex, ey, ez values for node 1 followed
by ex, ey, ez values for node 2.
(ii)
The OFSK command has the keyword OFSK followed by a skew system integer to identify the skewed
global axes system. This is then followed by 6 offset values as above.
(iii)
For BM2D element, 4 values of offset are required, ex, ey, values for node 1 followed by ex, ey for node 2.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-12
Appendix A
ASAS (Non-Linear) User Manual
Example
Example of offset beam elements.
175
BM3D
17.5
:
145.0
0.0
:
1
OFFG
BEAM
-5.0
64.2
:
OFSK
6
225.0
97.3
5.7
1107.0
0.0
2.0 0.0
1208.0 497.0
1.0
0.0
0.0
-8.0
23.0
0.0
0.0
6.0
-1.0
0.0
5.0
A.3.3 OFCO Command
For the OFCO command, the global coordinates of the physical ends of member centroidal axes are required.
Y
(x2,y2 ,z2 )
Node 2
(x1 ,y1 z1 )
Node1
X
Figure A.4 Beam Offsets Defined using OFCO
Notes
1.
The command has the keyword OFCO and the 6 coordinate values x,y,z for end 1 followed by x,y,z for
end2.
2.
For BM2D element, 4 values of coordinates are required, x,y for end 1 followed by x,y for end 2.
Example of offset BM3D
175
BM3D
17.5
OFCO
10.0
:
:
0.0
145.0
225.0
5.0
97.3
5.7
1107.0
8.0
0.0
12.0
0.0
3.0
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
20.0
Page A-13
Appendix A
ASAS (Non-Linear) User Manual
A.3.4 Finite Element Description Sheets
Beams/Bars
BEAM 2 node beam with constant cross section and rigid offset and special orientations for three
dimensional structures
BM3D 2 node beam with constant cross section and rigid offsets for three dimensional structures.
BM2D 2 node beam with constant cross section and rigid offsets for two dimensional structures.
FLA2
2 node axial element with varying cross section.
TUBE
2 node circular tube element with constant cross section and rigid offsets.
Solid Elements
BRK6
6 node straight edged wedge.
BRK8
8 node straight edged brick.
BR15
15 node wedge.
BR20
20 node brick.
LB15
15 node laminate wedge.
LB20
20 node laminate brick.
Axisymmetric Elements
QUX4
QUX8
Axisymmetric quadrilateral solid with straight or curved edges.
TRX3
Axisymmetric triangular solid with straight or curved edges.
TRX6
Membrane Elements
QUM4 4 node quadrilateral membrane with varying thickness and plane strain options.
QUM8 8 node isoparametric quadrilateral membrane with varying thickness and plane strain options.
TRM3 3 node triangular membrane with varying thickness and plane strain options.
TRM6 6 node isoparametric triangular membrane with varying thickness and plane strain options.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-14
Appendix A
ASAS (Non-Linear) User Manual
A.3.4
Finite Element Description Sheets
Gap Elements
GAP2
GAPX
GAPR
2D/3D node-to-node interface/gap element.
axisymmetric node-to-node interface/gap element.
node-to-node radial interface/gap element
Beam/Stiffener Elements
SST4
STF4
WST4
curved beam/stiffener element with thin-walled open section.
curved beam/stiffener with solid rectangular, tube and box section.
curved beam/stiffener element with thin-walled open section including warping.
Rigid Surface Interface Elements
RGX3
RGX4
RG23
RG24
rigid surface interface for use with axisymmetric elements TRX3 and QUX4.
rigid surface interface for use with axisymmetric elements TRX6 and QUX8.
rigid surface interface for use with plane elements TRM3 and QUM4.
rigid surface interface for use with plane elements TRM6 and QUM8.
Shell Elements
TCS6
TCS8
TCS9
6 node triangular element for modelling thick and thin shell applications.
8 node quadrilateral element for modelling thick and thin shell applications.
9 node quadrilateral element for modelling thick and thin shell applications.
QUS4
4 node quadrilateral shell element for modelling thick and thin shell applications.
Note all elements can have laminated composite material properties
Special Elements
SPR1
SPR2
Translational spring element between 2 nodes with damper.
Rotational spring element between 2 nodes with damper.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-15
Appendix A
ASAS (Non-Linear) User Manual
A.3.4
Finite Element Description Sheets
Linespring Elements
LSP3
elasto-plastic line-spring element for use with high order shell elements for
modelling surface flaws, symmetric boundary.
LSP6
elasto-plastic line-spring element for use with high order shell elements for
modelling surface flaws.
Uniaxial Field Elements
FAT2
2 node uniaxial field element with varying cross-section.
FAT3
3 node curved uniaxial field element with varying cross-section.
3-D Solid Field Elements
BRT6
6 node straight edged wedge.
BRT8
8 node straight edged brick.
BT15
15 node wedge.
BT20
20 node brick.
Axisymmetric Field Elements
QXT4
QXT8
Axisymmetric quadrilateral solid with straight or curved edges.
TXT3
TXT6
Axisymmetric triangular solid with straight or curved edges.
2-D Plane Field Elements
QMT4 4 node quadrilateral membrane with varying thickness.
QMT8 8 node isoparametric quadrilateral membrane with varying thickness.
TMT3 3 node triangular membrane with varying thickness.
TMT6 6 node isoparametric triangular membrane with varying thickness.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-16
BEAM
Appendix A
ASAS (Non-Linear) User Manual
BEAM
Three-dimensional Beam Bending Element with Uniform Cross-section and Special
Orientation of the Local Axes
1
NUMBER OF NODES
2
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ at each node
GEOMETRIC PROPERTIES
(uniform)
A
Iz”z”
Cross-sectional area (≥ 0.0)
Principal moment of inertia about the local Z” axis (≥ 0.0)
Iy”y”
Principal moment of inertia about the local Y” axis (≥ 0.0)
J
Torsion constant (≥ 0.0)
2
OFFSETS
The OFFG, OFFS, OFSK, OFCO commands can be used to define rigid offsets
at each end. For further details see Section 5.2.5.5 and Appendix A.3.
MATERIAL MODEL
ELASTIC
-
Isotropic
PLASTIC
-
Stress resultant model based on generalised plastic hinge
theory. Note that hinges can only form at nodes.
See Appendix -B for details.
Material properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements
Temperature loads
Distributed load patterns
BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
GL1, GL4, GL5, GL6, GL7
GP1, GP4, GP6, GP7
Body Forces
Centrifugal Loads
Angular Acceleration
Wave load
MASS MODELLING
Consistent Mass
Lumped Mass (used by default)
FORCE OUTPUT
The forces are exerted by the nodes on the element and related to the centroidal
local axes.
Axial Force X”X” at each end
Transverse shears QY” and QZ” at each end
Torque X”X” at each end
Bending Moments Y”Y” and Z”Z” at each end
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-17
BEAM
ASAS (Non-Linear) User Manual
INTEGRATION RULES
Appendix A
There are no integration points for the element, all the necessary element
matrices being formed explicitly.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-18
BEAM
Appendix A
ASAS (Non-Linear) User Manual
LOCAL AXES
A beam element has two local axes systems. The X’Y’Z’ local axes are
associated with end nodes of the element. The X”Y”Z” local axes are
associated with the end points of the centroidal axis of the element, taking
account of any non-zero rigid offsets.
If all offsets are zero, X’Y’Z’ and X”Y”Z” are coincident.
Geometric properties, distributed loads and output forces are all referred to the
X”Y”Z” local axes.
Local X” lies along the centroidal axis from end 1 towards end 2. Local Z”
must lie in the global XY plane with +ve local Y” on the +ve side of the global
XY plane. In the special case where local Y” is also in the global XY plane,
local Y” must lie in the global Y direction. BM3D should be used for a beam
with general orientation of local Z”.
See also Section 5.2.5.5 and Appendix A.2.1.
SIGN CONVENTIONS
Axial force
Shear force
Torque
positive for tension
positive for end 2 sagging relative to end 1
positive for clockwise rotation of end 2
relative to end 1, looking from end 1
towards end 2
Bending moment
Shear QY”
+ve
Moment Z”Z”
Positive for sagging
Shear QZ”
+ve
Moment Y”Y”
Y''
+ve
+ve
Z''
1
2
1
X''
LIMITATIONS
Length must be >0.0
REFERENCE
A.1
DATA EXAMPLES
ELEM
MATP
BEAM
BEAM
END
1
9
10
3
10
11
2
2
X''
GEOM
2
3
BEAM
BEAM
27.1
39.2
1469.7
2006.3
1614.1
1987.0
2766.9
3124.8
END
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-19
BM2D
Appendix A
ASAS (Non-Linear) User Manual
Two-dimensional Beam Bending Element with Uniform Cross-section,
Lying in the Global XY Plane
Y
NUMBER OF NODES
2
NODAL COORDINATES
x, y
2
1
Option TWOD must be specified
DEGREES OF FREEDOM
X, Y, RZ at each node
GEOMETRIC PROPERTIES
A
Cross-sectional area (> 0.0)
(uniform) Iz”z”
X
Principal moment of inertia about the local Z” axis (> 0.0) Asy”Effective shear
area (shear strain is neglected if Asy” is blank)
OFFSETS
The OFFG, OFFS, OFSK, OFCO commands may be used to define rigid
offsets at each end. For further details see Appendix A.3 and Section 5.2.5.
MATERIAL MODEL
ELASTIC
-
Isotropic
PLASTIC
-
Stress resultant model based on generalised plastic hinge
theory. Note that hinges can only form at nodes.
See Appendix -B for details.
Material properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements
Temperature loads
Distributed load patterns
BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
GL1, GL4, GL5, GL6, GL7
GP1, GP4, GP6, GP7
Body Forces
Centrifugal Loads
Angular Acceleration
MASS MODELLING
Consistent Mass
Lumped Mass (used by default)
FORCE OUTPUT
The forces are exerted by the nodes on the element, and related to the local
axes. Note that for an offset beam the forces output are related to the member
centroidal axes.
INTEGRATION RULES
There are no integration points for the element, all the necessary element
matrices being formed explicitly.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-20
BM2D
Appendix A
ASAS (Non-Linear) User Manual
LOCAL AXES
The X’Y’ local axes are associated with the end nodes of the member. The
X”Y” local axes are associated with the physical ends of the centroid of the
member after taking account of any non-zero rigid offsets. If the offsets are all
zero then X’Y’ and X”Y” are coincident.
Local X’ (X”) lies along the element from node 1 (end1) towards node 2
(end2). Local Z’ (Z”) must lie in the global Z direction. Local Y” forms a
right handed set with local X” and local Z”
The geometric properties Iz”z” and Asy” are related to X”Y” system. Distributed
loads are also in the X”Y” system.
See also section 5.2.5 and Appendix A.2.1
SIGN CONVENTIONS
Axial force
Shear force
Bending moment
+ve for tension
+ve for node 2 sagging relative to node 1
+ve for sagging
Y'
1
2
X'
LIMITATIONS
Length must be >0.0
REFERENCE
A. 1
DATA EXAMPLE
ELEM
MATP
BM2D
1
9
10
3
/
BM2D 10
11
2
RP 6
END
Shear QY”
+ve
Moment Z”Z”
+ve
1
GEOM
2
3
BM2D
BM2D
27.1
39.2
1469.7
2006.3
32.8
END
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-21
BM3D
Appendix A
ASAS (Non-Linear) User Manual
Three-dimensional Beam Bending Element with Uniform Cross-section and any
Orientation of the Local Axes
1
NUMBER OF NODES
2
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ at each node
GEOMETRIC PROPERTIES
A
Cross-sectional area (> 0.0)
(uniform)
Iz”z”
Iy”y”
Principal moment of inertia about the local Z” axis (> 0.0)
Principal amount of inertia about the local Y” axis (> 0.0)
2
J
Torsion constant (> 0.0)
Local Axis Definition - see Section 5.2.5.5 and Appendix A.2.1.
Asy”
Effective shear area for forces in Y” direction
Asz”
(Y” shear strain is neglected if Asy” is blank)
Effective shear area for forces in Z” direction
(Z” shear strain is neglected if Asz” is blank)
OFFSETS
The OFFG, OFFS, OFSK, OFCO commands may be used to define rigid
offsets at each end. For further details see Appendix A.3 and Section 5.2.5.
MATERIAL MODEL
ELASTIC
-
Isotropic
PLASTIC
-
Stress resultant model based on generalised plastic hinge
theory. Note that hinges can only form at nodes.
See Appendix -B for details.
Material properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements
Temperature loads
Distributed load patterns
BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
GL1, GL4, GL5, GL6, GL7
GP1, GP4, GP6, GP7
Body Forces
Centrifugal Loads
Angular Acceleration
Wave load
MASS MODELLING
Consistent Mass
Lumped Mass (used by default)
FORCE OUTPUT
The forces are exerted by the nodes on the element, and related to the local
axes. Note that for an offset beam the forces output are related to the element
centroidal axes.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-22
BM3D
ASAS (Non-Linear) User Manual
INTEGRATION RULES
Appendix A
There are no integration points for the element, all the necessary element
matrices being formed explicitly.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-23
BM3D
Appendix A
ASAS (Non-Linear) User Manual
LOCAL AXES
The X’Y’Z’ local axes are associated with the end nodes of the member. The
X”Y”Z” local axes are associated with the physical ends of the centroid of the
member after taking account of any non-zero rigid offsets. If the offsets are all
zero then X’Y’Z’ and X”Y”Z” are coincident.
Local X’ (X”) lies from node 1 (end1) towards node 2 (end2). Local Y’ (Y”)
lies in the plane defined by the two nodes (ends) and a third point defined in
the Geometric Properties list. This third point must not lie on the X’ or X”
axes. Local Y’ (Y”) lies from node 1 (end1) and is +ve towards the third point.
Local Z’ (Z”) forms a right-handed set with local X’ (X”) and local Y’ (Y”).
The geometric properties A, Iy”y”, Iz”z”, Asy”, Asz” and J all refer to the X”Y”Z”
system. Distributed loads are also in the X”Y”Z” system.
If a local axis definition is not supplied, a 3rd point with coordinates of 0.0,
0.0, 0.0 is assumed.
See also Section 5.2.5.5 and Appendix A.2.1
SIGN CONVENTIONS
Axial force
Shear force
+ve for tension
+ve for node 2 sagging relative to node 1
Torque
+ve for anti-clockwise rotation at node
1 and clockwise rotation at node 2
looking from node 1 towards node 2
Bending moment
Shear QY”
Moment Z”Z”
+ve for sagging
+ve
+ve
Shear QZ”
Moment Y”Y”
Y''
+ve
+ve
Z''
1
2
1
2
X''
LIMITATIONS
Length must be >0.0
REFERENCE
A. 1
DATA EXAMPLE
ELEM
MATP 1
BM3D
/
9
10
3
BM3D 10
RP 6 1
11
2
X''
END
GEOM
3 BM3D
:
END
39.2
2006.3
1987.0
-18.1
32.8
13.7
3124.8
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
-1.4
2.3
Page A-24
BRK6
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Brick Element with Quasi-linear Strain Variation
1
2
NUMBER OF NODES
6
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
X, Y, Z at each node
3
4
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
ELASTIC
-
Isotropic
Orthotropic
-
Woven
Anisotropic
5
6
Anisotropic matrix (C or C-1) - referred to axis system
selected for output (global by default)
σxx
σyy
σzz
σxy
σyz
σzx
=
C1 C2
. C3
.
.
.
.
.
.
.
.
C4
C5
C6
.
.
.
C7
C8
C9
C10
.
.
C11
C12
C13
C14
C15
.
C16
C17
C18
C19
C20
C21
εxx
εyy
εzz
εxy
εyz
εzx
6 coefficients of thermal expansion αxx, αyy, αzz, αxy, αyz, αzx,
referred to axis system selected for output.
-
Hyperelastic
PLASTIC
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager, Tension
cut, yield criteria.
Isotropic, Kinematic (Prager or Ziegler) or Combined
CREEP
-
von Mises.
Hardening.
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-25
BRK6
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal loads
Prescribed displacements
Pressure loads (on any face, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
Angular accelerations
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points related to either global or
local axes (global by default)
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
a triangular face
INTEGRATION RULES
1x1x2 Gauss quadrature by default. Higher order rules by request.
Appendix -G gives positions of integration points.
LOCAL AXES
At any point local X’ coincides with the (straight) line L1=0 +ve in the
direction 1, 2. Local Y’ lies in the triangular plane L1L2L3 +ve towards node 3.
Local Z’ forms a right-handed set with local X’ and local Y’. See Appendix -
SIGN CONVENTIONS
G for explanation of curvilinear axes.
+ve for tension
Direct stresses σxx, σyy, σzz
Shear stresses σxy, σyz, σzx
REFERENCE
+ve as shown
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-26
BRK8
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Brick Element with
Quasi-linear Strain Variation
2
1
NUMBER OF NODES
8
3
4
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
X, Y, Z at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
ELASTIC
6
5
-
Isotropic
Orthotropic
Woven
-
Anisotropic
7
8
Anisotropic matrix (C or C-1) - referred to axis system
selected for output (global by default)
σxx
σyy
σzz
σxy
σyz
σzx
=
C1 C2
. C3
.
.
.
.
.
.
.
.
C4
C5
C6
.
.
.
C7
C8
C9
C10
.
.
C11
C12
C13
C14
C15
.
C16
C17
C18
C19
C20
C21
εxx
εyy
εzz
εxy
εyz
εzx
6 coefficients of thermal expansion αxx, αyy, αzz, αxy, αyz, αzx,
referred to axis system selected for output.
PLASTIC
-
Hyperelastic
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
Tension cut, yield criteria.
Isotropic, Kinematic (Prager or Ziegler) or Combined
Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-27
BRK8
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal loads
Prescribed displacements
Pressure loads (on any face, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
Angular accelerations
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points related to either global or
local axes (global by default)
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
a triangular face
INTEGRATION RULES
2x2x2 Gauss quadrature by default. Higher order rules by request.
Appendix -G gives positions of integration points.
LOCAL AXES
At any point local X’ is coincident with curvilinear ξ. Local Y’ lies in the
curvilinear ξη plane, +ve in the +ve η direction. Local Z’ forms a righthanded set with local X’ and local Y’. See Appendix -G for explanation of
SIGN CONVENTIONS
REFERENCE
curvilinear axes.
Direct stresses σxx, σyy, σzz
+ve for tension
Shear stresses σxy, σyz, σzx
+ve as shown
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-28
BR15
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Brick Element with Quasi-quadratic Strain Variation
NUMBER OF NODES
15 (6 corner, 9 mid-side)
NODAL COORDINATES
x, y, z
(may be omitted for mid-side nodes on
straight edges). The position of each
mid-side node has a tolerance of sidelength/10
position.
about the
DEGREES OF FREEDOM
X, Y, Z at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
ELASTIC
true
-
Isotropic
Orthotropic
-
Woven
Anisotropic
mid-side
Anisotropic matrix (C or C-1) - referred to axis system
selected for output (global by default)
σxx
σyy
σzz
σxy
σyz
σzx
=
C1 C2
. C3
.
.
.
.
.
.
.
.
C4
C5
C6
.
.
.
C7
C8
C9
C10
.
.
C11
C12
C13
C14
C15
.
C16
C17
C18
C19
C20
C21
εxx
εyy
εzz
εxy
εyz
εzx
6 coefficients of thermal expansion αxx, αyy, αzz, αxy, αyz, αzx,
referred to axis system selected for output.
PLASTIC
-
Hyperelastic
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager Tension
cut, yield criteria
Isotropic, Kinematic (Prager or Ziegler) or Combined
Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-29
BR15
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal loads
Prescribed displacements
Pressure loads (on any face, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
Angular accelerations
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points related to either global or
local axes (global by default)
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
a triangular face at a corner node
INTEGRATION RULES
1x3x2 Gauss quadrature by default. Higher order rules by request.
Appendix -G gives positions of integration points.
LOCAL AXES
At any point local X’ is tangential to curvilinear L1 = constant +ve in the
direction 1 to 2. Local Y’ is tangential to the curvilinear L1L2L3 surface, +ve
towards node 5. Local Z’ forms a right-handed set with local X’ and local Y’.
SIGN CONVENTIONS
See Appendix -G for explanation of curvilinear axes.
+ve for tension
Direct stresses σxx, σyy, σzz
Shear stresses σxy, σyz, σzx
REFERENCE
+ve as shown
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-30
BR20
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Brick Element with Quasi-quadratic Strain Variation
NUMBER OF NODES
20 (8 corner, 12 mid-side)
NODAL COORDINATES
x, y, z
(may be omitted for mid-side nodes on
straight edges). The position of each
mid-side node has a tolerance of sidelength/10
position.
about the
DEGREES OF FREEDOM
X, Y, Z at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
ELASTIC
true
-
Isotropic
Orthotropic
-
Woven
Anisotropic
mid-side
Anisotropic matrix (C or C-1) - referred to axis system
selected for output (global by default)
σxx
σyy
σzz
σxy
σyz
σzx
=
C1 C2
. C3
.
.
.
.
.
.
.
.
C4
C5
C6
.
.
.
C7
C8
C9
C10
.
.
C11
C12
C13
C14
C15
.
C16
C17
C18
C19
C20
C21
εxx
εyy
εzz
εxy
εyz
εzx
6 coefficients of thermal expansion αxx, αyy, αzz, αxy, αyz, αzx,
referred to axis system selected for output.
PLASTIC
-
Hyperelastic
-
von Mises, Tresca, Mohr-Coulomb,
Tension cut, yield criteria.
Drucker-Prager
Isotropic, Kinematic (Prager or Ziegler) or Combined
Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-31
BR20
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal loads
Prescribed displacements
Pressure loads (on any face, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
Angular accelerations
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points related to either global or
local axes (global by default)
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at a
corner node
INTEGRATION RULES
2x2x2 Gauss quadrature by default. Higher order rules by request.
Appendix -G gives positions of integration points.
LOCAL AXES
At any point local X’ is tangential to and in the direction of curvilinear ξ.
Local Y’ is tangential to the curvilinear ξη surface, +ve in the +ve η direction.
Local Z’ forms a right-handed set with local X’ and local Y’.
SIGN CONVENTIONS
See Appendix -G for explanation of curvilinear axes.
+ve for tension
Direct stresses σxx, σyy, σzz
Shear stresses σxy, σyz, σzx
REFERENCE
+ve as shown
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-32
BRT6
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Field Brick Element with Quasi-linear Variation
of Field Variable
1
NUMBER OF NODES
6
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
T at each node
2
3
4
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
FIELD
5
6
PIER
Material properties can be temperature dependent if required
LOAD TYPES
Nodal value related to field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradient
(analogous to strains) are available at integration points related to either global
or local axes (global by default)
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
a triangular face
INTEGRATION RULES
1x1x2 Gauss quadrature by default. Higher order rules by request.
Appendix -G gives positions of integration points.
LOCAL AXES
At any point local X’ coincides with the (straight) line L1=0 +ve in the
direction 1, 2. Local Y’ lies in the triangular plane L1L2L3 +ve towards node 3.
Local Z’ forms a right-handed set with local X’ and local Y’. See Appendix G for explanation of curvilinear axes.
SIGN CONVENTIONS
Fluxes and gradients positive when in the positive axis direction.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-33
BRT6
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4A. 4A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-34
BRT8
ASAS (Non-Linear) User Manual
Appendix A
Isoparametric Field Brick Element with Quasi-linear Variation
of Field Variable
NUMBER OF NODES
8
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
T at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
FIELD
PIER
Material properties can be temperature dependent if required
LOAD TYPES
Nodal values related to the field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at the integration points related to either the
local or global axes (global by default)
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at a
corner node
INTEGRATION RULES
2x2x2 Gauss quadrature by default. Higher order rules by request.
Appendix -G gives positions of integration points.
LOCAL AXES
At any point local X’ is coincident with curvilinear ξ. Local Y’ lies in the
curvilinear ξη plane, +ve in the +ve η direction. Local Z’ forms a righthanded set with local X’ and local Y’. See Appendix -G for explanation of
curvilinear axes.
SIGN CONVENTIONS
Fluxes and gradients are positive when in the positive axis direction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-35
BRT8
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-36
BT15
ASAS (Non-Linear) User Manual
Appendix A
Isoparametric Field Brick Element with Quasi-quadratic Variation
of Field Variable
NUMBER OF NODES
15 (6 corner, 9 mid-side)
NODAL COORDINATES
x, y, z
(may be omitted for mid-side nodes on
straight edges). The position of each
mid-side node has a tolerance of sidelength/10 about the true mid-side
position.
DEGREES OF FREEDOM
T at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
FIELD
PIER
Material properties can be temperature dependent if required
LOAD TYPES
Nodal values related to the field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at the integration points related to either the
local or global axes (global by default)
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
a triangular face at a corner node
INTEGRATION RULES
1x3x2 Gauss quadrature by default. Higher order rules by request.
Appendix -G gives positions of integration points.
LOCAL AXES
At any point local X’ is tangential to curvilinear L1 = constant +ve in the
direction 1 to 2. Local Y’ is tangential to the curvilinear L1L2L3 surface, +ve
towards node 5. Local Z’ forms a right-handed set with local X’ and local Y’.
See Appendix -G for explanation of curvilinear axes.
SIGN CONVENTIONS
Fluxes and gradients are positive when in the positive axis direction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-37
BT15
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-38
BT20
ASAS (Non-Linear) User Manual
Appendix A
Isoparametric Field Brick Element with Quasi-quadratic Variation
of Field Variable
NUMBER OF NODES
20 (8 corner, 12 mid-side)
NODAL COORDINATES
x, y, z
(may be omitted for mid-side nodes on
straight edges). The position of each
mid-side node has a tolerance of sidelength/10 about the true mid-side
position.
DEGREES OF FREEDOM
T at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
FIELD
PIER
Material properties can be temperature dependent if required
LOAD TYPES
Nodal values related to the field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at the integration points related to either the
local or global axes (global by default)
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at a
corner node
INTEGRATION RULES
2x2x2 Gauss quadrature by default. Higher order rules by request.
Appendix -G gives positions of integration points.
LOCAL AXES
At any point local X’ is tangential to and in the direction of curvilinear ξ.
Local Y’ is tangential to the curvilinear ξη surface, +ve in the +ve η direction.
Local Z’ forms a right-handed set with local X’ and local Y’.
See Appendix -G for explanation of curvilinear axes.
SIGN CONVENTIONS
Fluxes and gradients positive when in the positive axis direction.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-39
BT20
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-40
FAT2
Appendix A
ASAS (Non-Linear) User Manual
Straight Field Axial Element with Linear Variation
of Field Variable
2
NUMBER OF NODES
2
1
NODAL COORDINATES
x, y, z
z should be omitted for 2D problems
DEGREES OF FREEDOM
T at each node.
GEOMETRIC PROPERTIES
A1
A2
Cross-sectional area at node 1
Cross-sectional area at node 2
(The cross-sectional area varies linearly between node 1 and node 2.
The value A2 may be omitted for an element with uniform area A1).
MATERIAL MODELS
FIELD
PIER
CVEC
RADI
Material properties can be temperature dependent if required
LOAD TYPES
Nodal values related to the field variable type
Prescribed field variable
Temperature
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at the integration points related to the local
axes
INTEGRATION RULE
Not appropriate, explicit integration assuming constant field variable is used.
LOCAL AXES
Local X’ lies along the element from node 1 towards node 2.
SIGN CONVENTIONS
Fluxes and gradients positive when in the positive axis direction.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-41
FAT2
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
4.
For heat conduction analysis, this element may be used to model convection by specifying directive FLNS
in the PROB/TITL or GROUP commands. In this case, the first material property specified will have the
meaning of a heat transfer (or film) coefficient and the length of an element will not enter into the heat flow
calculations. All FAT2 elements in the same group are so treated.
5.
The convective and radiant heat transfer can be modelled directly using the CVEC and RADI material
models, respectively. The length of an element will not enter into the calculations with these 2 models.
6.
The area required for the RADI model is the direct interchange area. This is defined to the product of the
geometric view factor and the emitting surface area.
REFERENCE
A. 1, A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-42
FAT3
Appendix A
ASAS (Non-Linear) User Manual
Curved Axial Field Element with Quadratic Variation
of Field Variable
NUMBER OF NODES
3
NODAL COORDINATES
x, y, z
z should be omitted for 2D problems
2
3
1
DEGREES OF FREEDOM
T at each node.
GEOMETRIC PROPERTIES
A1
A2
Cross-sectional area at node 1
Cross-sectional area at node 2
A3
Cross-sectional area at node 3
(The cross-sectional area varies quadratically between node 1,
node 2 and node 3. The values A2 and A3 may be omitted for an
element with uniform area A1).
MATERIAL MODELS
FIELD
PIER
Material properties can be temperature dependent if required
LOAD TYPES
Nodal values related to the field variable type
Prescribed field variable
Temperature
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at the integration points related to the local
axes
INTEGRATION RULE
2 point integration assuming linear variation of the field variable
LOCAL AXES
Local X’ lies along the element axis from node 1 towards node 3.
SIGN CONVENTIONS
Fluxes and gradients positive when in the positive axis direction.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-43
FAT3
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 1, A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-44
FLA2
Appendix A
ASAS (Non-Linear) User Manual
Straight Axial Element with Constant Strain
NUMBER OF NODES
2
NODAL COORDINATES
x, y, z
z should be omitted
2
1
2D problems
DEGREES OF FREEDOM
X, Y, (Z) at each node.
Option TWOD converts to 2-D form, freedoms X, Y only.
GEOMETRIC PROPERTIES
There are two types of geometric properties available:
(a)
Cross-sectional areas at nodes 1 and 2, no keyword required with
geometric property data
A1 Cross-sectional area at node 1
A2 Cross-sectional area at node 2
(The cross-sectional area varies linearly between node 1 and
node 2. The value A2 may be omitted for an element with
uniform area A1).
(b)
Cross-sectional areas at nodes 1 and 2 plus keyword CABL on
a continuation line to invoke the conversion to a tension only
(cable formulation)
A1 Cross-sectional area at node 1
A2 Cross-sectional area at node 2
(The cross-sectional area varies linearly between node 1 and
node 2. The value A2 may be omitted for an element with
uniform area A1).
The geometric property data required following the keyword CABL
are:
Te
m
-
erection tension
mass unit per length
g
-
acceleration due to gravity
Cd
ρa
-
coefficient of drag
mass per unit volume for air
d
V
-
cable diameter
magnitude of wind velocity
α
-
bearing of V from the global XZ plane
β
a
-
bearing of V from the global XY plane
load stiffness
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-45
FLA2
Appendix A
ASAS (Non-Linear) User Manual
MATERIAL MODELS
ELASTIC
PLASTIC
-
CREEP
-
Isotropic
Hyperelastic
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager,
Tension cut, yield criteria
Isotropic, Kinematic (Prager or Ziegler) or Combined
Hardening.
von Mises.
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements
Temperature loads (Not valid with CABL properties)
Body forces
Centrifugal loads
Angular accelerations
MASS MODELLING
Lumped mass (used by default)
Consistent mass
OUTPUT
Stresses and strains are available for the centre of the element
(in local axes).
INTEGRATION RULE
Not appropriate, explicit integration assuming constant stress is used.
LOCAL AXES
Local X’ lies along the element from node 1 towards node 2.
SIGN CONVENTION
Axial stress +ve for tension.
NOTES
1.
Any group containing FLA2 elements must contain only FLA2 elements.
2.
The stiffness E(A1 + A2)/2L of the element can be set to E(A1 + A2)/2, thereby allowing the elastic (natural)
stiffness to be unchanged by large deformations. This is accomplished by directive FLNS using the
PROB/TITL or GROUP commands. All FLA2 elements in the same group are so treated.
REFERENCE
A. 1, A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-46
GAP2
Appendix A
ASAS (Non-Linear) User Manual
Interface/Gap Element with Sliding Capacity
2
NUMBER OF NODES
2
NODAL COORDINATES
x, y, z
z should be omitted for 2D problems
DEGREES OF FREEDOM
X, Y, (Z) at each node.
Option TWOD converts to 2-D form, freedoms X, Y only.
GEOMETRIC PROPERTIES
GAP
1
The initial size of the gap. (GAP ≤ 0.0 assumes an initial
gap closed condition and GAP will be reset to zero internally)
MUY
Coefficient of friction in local Y’-direction
MUZ
XG
Coefficient of friction in local Z’-direction, zero for TWOD
X component of vector defining the gap reference axis
YG
ZG
Y component of vector defining the gap reference axis
Z component of vector defining the gap reference axis
KN
KT
Normal contact stiffness factor (see note 4)
Tangential stick stiffness factor (see note 5)
KR
Gap residual stiffness factor (see note 6)
C
Damping coefficient
MATERIAL MODELS
Elastic only. K - the effective contact stiffness is given in the material
property data (see note 3)
LOAD TYPES
Nodal loads
Prescribed displacements
OUTPUT
The gap size, GAP, in the X’-direction and sliding displacements SLIDE-Y
and SLIDE-Z are related to local axes. Force across the gap, Fx’x’, and
frictional forces Fy’y’ and Fz’z’ are related to the local axes. STATUS refers to
the status of the element at the last iteration.
Both STRS and STRN should be specified using the corresponding BLOC
command to obtain gap output.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-47
GAP2
ASAS (Non-Linear) User Manual
LOCAL AXES
Appendix A
Local X’ lies along the gap reference axis (see note 1). Local Y’ lies in the
global xy plane, perpendicular to local X’. (If local X’ is parallel to global z,
then local Y’ lies in the global xy plane in the negative x direction). Local Z’
forms a right-handed set with local X’ and local Y’.
SIGN CONVENTIONS
Force Fx’x’ tending to open gap is positive.
GAP is positive if gap is open.
NOTES
1.
The gap reference axis defines the direction of the gap surface, which is assumed to be in a plane
perpendicular to this axis. If this is specified as {0.0, 0.0, 0.0}, the gap reference axis will be assumed to
lie along the element from node 1 to node 2. In this case, nodes 1 and 2 must not be coincident.
2.
GAP elements cannot be placed with other types of element in the same group.
3.
The effective stiffness (K) required in the material property data can be estimated as E√A, where E is the
elastic modulus and A is the effective area at the contact node.
4.
When the gap is closed, the normal stiffness between the two nodes is computed as KN*K. If KN ≤ 0.0 is
specified, it will be set equal to the value of the parameter GAPSTF in the PARA command (default 1000).
5.
When the gap is closed and stick, the tangential stick stiffness betweeen the two nodes is computed as
KT*K. If KT ≤ 0.0 is specified, it will be set equal to the value of the parameter GAPSTF in the PARA
command (default 1000).
6.
When the gap is open, a residual stiffness is used in order to maintain numerical stability. This is given by
KR*K. If KR < 0.0 is specified, it will be set equal to the value of the parameter GAPSMA in the PARA
command (default 10-8).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-48
GAPR
Appendix A
ASAS (Non-Linear) User Manual
Radial Gap Element with Sliding Capacity
GAP > 0.0
NUMBER OF NODES
2
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
X, Y, Z
MATERIAL MODELS
Elastic only -
GAP < 0.0
2
2
1
the effective stiffness, K
(see note 4)
GEOMETRIC PROPERTIES
GAP
MUY
Gap parameter (see note 2)
Coefficient of friction in local Y’ direction
MUZ
Coefficient of friction in local Z’ direction
XG
YG
X component of vector defining the gap reference axis
Y component of vector defining the gap reference axis
ZG
KN
Z component of vector defining the gap reference axis
Normal contact stiffness factor (see note 5)
KT
KR
Tangential stick stiffness factor (see note 6)
Gap residual stiffness factor (see note 7)
C
Damping coefficient
LOAD TYPES
Nodal loads
Prescribed displacements
OUTPUT
The gap size, GAP in the X’ direction and sliding displacements SLIDE-Y and
SLIDE-Z are related to the local axes. Forces across the gap Fx’x’ and frictional
forces Fy’y’ and Fz’z’ are related to the local axes. STATUS refers to the status
of the element at the last iteration. STATUS = 1 for no contact, = 2 for contact
and stick, = 5 for contact and slide. Both STRS and STRN should be specified
using the corresponding BLOC command to obtain gap output.
LOCAL AXES
Local Z’ axis is the gap reference axis (see note 3). Local X’ lies from node 1
to node 2 and on the normal plane to local Z’. Local Y’ is also on the normal
plane to local Z’ and perpendicular to local X’.
SIGN CONVENTIONS
Force Fx’x’ tending to open gap is positive. GAP is positive if gap is open.
Notes
1.
Gap elements cannot be placed with other types of element in the same group.
2.
The gap parameter is used to define the position and diameter of the tubes (plus any non-structural
coatings, etc).
a) Tube in Tube configuration.
The parameter is used to define the distance (gap) between the outer diameter of the inner tube and the
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-49
GAPR
ASAS (Non-Linear) User Manual
Appendix A
inner diameter of the outer tube. Hence the value entered ought to equal the outer tube’s inner radius less
the inner tube’s outer radius. Allowance will be automatically be made if the nodes are not coincident.
b) Two separate tubes configuration.
To indicate that this is the case, the sign of this parameter must be negative. The magnitude of the
parameter is used to define the distance (gap) between nodes below which contact will occur. Hence the
the value will be equal to the sum of the two outer radii.
3.
The gap reference axis defines the direction that is normal to the contact plane. If this is specified as {0.0,
0.0, 0.0}, the gap reference axis will be assumed to be in the global Z direction (i.e. the contact plane is the
global X-Y plane).
4.
The effective stiffness (K) required in the material property data can be estimated as E√A, where E is the
elastic modulus and A is the effective area at the contact node.
5.
When the gap is closed, the normal stiffness between the two nodes is computed as KN*K. If KN ≤ 0.0 is
specified, it will be set equal to the value of the parameter GAPSTF in the PARA command (default 1000).
6.
When the gap is closed and stick, the tangential stick stiffness betweeen the two nodes is computed as
KT*K. If KT ≤ 0.0 is specified, it will be set equal to the value of the parameter GAPSTF in the PARA
command (default 1000).
7.
When the gap is open, a residual stiffness is used in order to maintain numerical stability. This is given by
KR*K. If KR < 0.0 is specified, it will be set equal to the value of the parameter GAPSMA in the PARA
command (default 10-8).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-50
GAPX
Appendix A
ASAS (Non-Linear) User Manual
Axisymmetric Interface/Gap Element with Sliding Capacity
2
NUMBER OF NODES
2
NODAL COORDINATES
r, z
(Note that r and z occupy the first and third
1
Z
fields with coordinate data using an
unnamed cartesian system).
R
DEGREES OF FREEDOM
R, Z at each node.
Any skew system must be 2-D.
GEOMETRIC PROPERTIES
GAP
The initial size of the gap. (GAP ≤ 0.0 assumes an initial
MUY
gap closed condition and GAP will be reset to zero internally)
Coefficient of friction in local Y’-direction
MUZ
XG
Coefficient of friction in local Z’-direction (always ignored)
X component of vector defining the gap reference axis
YG
Y component of vector defining the gap reference axis (always
assumed zero)
ZG
Z component of vector defining the gap reference axis
KN
KT
Normal contact stiffness factor (see note 4)
Tangential stick stiffness factor (see note 5)
KR
C
Gap residual stiffness factor (see note 6)
Damping coefficient
MATERIAL MODELS
Elastic only. K - the effective contact stiffness is given in the material property
data (see note 3)
LOAD TYPES
Nodal loads
Prescribed displacements
OUTPUT
The gap size, GAP, in the X’-direction and sliding displacements SLIDE-Y are
related to local axes. Force across the gap, Fx’x’, and frictional force Fy’y’ are
related to the local axes. STATUS refers to the status of the element at the last
iteration. Both STRS and STRN should be specified using the corresponding
BLOC command to obtain gap output.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-51
GAPX
ASAS (Non-Linear) User Manual
Appendix A
LOCAL AXES
Local X’ lies along the gap reference axis (see note 1). Local Y’ lies in the
global rz plane, perpendicular to local X’.
SIGN CONVENTIONS
Force Fx’x’ tending to open gap is positive. GAP is positive if gap is open.
NOTES
1.
The gap reference axis defines the direction of the gap surface, which is assumed to be in a plane
perpendicular to this axis. If this is specified as {0.0, 0.0, 0.0}, the gap reference axis will be assumed to
lie along the element from node 1 to node 2. In this case, nodes 1 and 2 must not be coincident.
2.
GAP elements cannot be placed with other types of element in the same group.
3.
The effective stiffness (K) required in the material property data can be estimated as E√A, where E is the
elastic modulus and A is the effective area at the contact node.
4.
When the gap is closed, the normal stiffness between the two nodes is computed as KN*K. If KN ≤ 0.0 is
specified, it will be set equal to the value of the parameter GAPSTF in the PARA command (default 1000)
5.
When the gap is closed and stick, the tangential stick stiffness between the two nodes is computed as
KT*K. If KT ≤ 0.0 is specified, it will be set equal to the value of the parameter GAPSTF in the PARA
command (default 1000).
6.
When the gap is open, a residual stiffness is used in order to maintain numerical stability. This is given by
KR*K. If KR < 0.0 is specified, it will be set equal to the value of the parameter GAPSMA in the PARA
command (default 10-8).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-52
LB15
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Laminated Brick Element with Quasi-quadratic
Strain Variation
NUMBER OF NODES
15 (6 corner, 9 mid-side)
NODAL COORDINATES
x, y, z
(may be omitted for mid-side nodes on
straight edges). The position of each
mid-side node has a tolerance of sidelength/10 about the true mid-side
position.
DEGREES OF FREEDOM
X, Y, Z at each node
GEOMETRIC PROPERTIES
Lay up data. See Section 5.2.5.3.
The layers are stacked from the bottom surface
up. The bottom surface is defined as the first face
formed by the local node numbering (the face formed
by nodes 1-6 in this case).
MATERIAL MODELS
ELASTIC
-
Laminated
FAIL
-
Lamina failure law for composites.
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements
Pressure loads (on any face, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
Angular accelerations
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points related to the principal
material axes of each layer
For failure analysis, the equivalent stress at each integration point is also
available. This is defined as:
SEQ=10*mode+f
where f is the failure function value and mode is the failure mode integer.
mode
= 0, elastic
= 4, fibre failure
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-53
LB15
Appendix A
ASAS (Non-Linear) User Manual
= 5, matrix failure
= 6, lamina failure
= 7, transverse shear/normal stress failure
= 8, modes 5 and 7
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting on
a triangular face at a corner node
INTEGRATION RULES
1x3x1 Gauss quadrature for each layer by default. If the element contains one
single layer only, then the default is 1x3x3, where Gauss quadrature is used for
the in-plane integration and Newton-Coates for through thickness integration.
Other rules by request.
Appendix -G gives positions of integration points.
Note that the integration order specified in the preliminary data is the rule
adopted for each layer.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-54
LB15
Appendix A
ASAS (Non-Linear) User Manual
SIGN CONVENTIONS
Direct stresses σxx, σyy, σzz
Shear stresses σxy, σyz, σzx
REFERENCE
A. 2
+ve for tension
+ve as shown
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-55
LB20
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Laminated Brick Element with Quasi-quadratic
Strain Variation
NUMBER OF NODES
20 (8 corner, 12 mid-side)
NODAL COORDINATES
x, y, z (may be omitted for midside nodes on straight edges).
The position of each mid-side
node has a tolerance of side/10
about the true mid-side position.
DEGREES OF FREEDOM
X, Y, Z at each node
GEOMETRIC PROPERTIES
Lay up data. See Section 5.2.5.3.
The layers are stacked from the bottom surface
up. The bottom surface is defined as the first face
formed by the local node numbering (the face formed
by nodes 1-8 in this case).
MATERIAL MODELS
ELASTIC
-
Laminated
FAIL
-
Lamina failure law for composites
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements
Pressure loads (on any face, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
Angular accelerations
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points related to the principal
material axes of each layer.
For failure analysis, the equivalent stress at each integration point is also
available. This is defined as:
SEQ=10*mode+f
where f is the failure function value and mode is the failure mode integer.
mode
= 0, elastic
= 4, fibre failure
= 5, matrix failure
= 6, lamina failure
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-56
LB20
Appendix A
ASAS (Non-Linear) User Manual
= 7, transverse shear/normal stress failure
= 8, modes 5 and 7
NODE NUMBERING
The nodes are listed in a screw sense, clockwise or anti-clockwise, starting at a
corner node
INTEGRATION RULES
2x2x1 Gauss quadrature for each layer by default. If the element contains one
single layer only, then the default is 2x2x3, where Gauss quadrature is used for
the in-plane integration and Newton-Coates for through thickness integration.
Other rules by request.
Appendix -G gives positions of integration points.
Note that the integration order specified in the preliminary data is the rule
adopted for each layer.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-57
LB20
Appendix A
ASAS (Non-Linear) User Manual
SIGN CONVENTIONS
Direct stresses σxx, σyy, σzz
Shear stresses σxy, σyz, σzx
REFERENCE
A. 2
+ve for tension
+ve as shown
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-58
LSP3
Appendix A
ASAS (Non-Linear) User Manual
Line-Spring Element Compatible with Quadratic Shell Elements for
Modelling Surface Flaws with Symmetry Boundary
NUMBER OF NODES
3
NODAL COORDINATES
x, y, z
2
DEGREES OF FREEDOM
3
X, Y, Z, RX, RY, RZ
1
GEOMETRIC PROPERTIES
d1
t1
d2
Crack depth at node 1
Shell thickness at node 1
Crack depth at node 2
t2
d3
Shell thickness at node 2
Crack depth at node 3
t3
Shell thickness at node 3
x1, y1, z1 Orientation node coordinates for node 1
x2, y2, z2 Orientation node coordinates for node 2
x3, y3, z3 Orientation node coordinates for node 3
The orientation node is a node in the plane of the crack, pointing in the
direction of the surface from which the crack originates.
(Note - d is +ve if a flaw lies on the +ve Z’ side and vice versa)
MATERIAL MODELS
ELASTIC
-
Isotropic only
PLASTIC
-
von Mises yield criterion
Isotropic hardening only
LOAD TYPES
Nodal loads
Prescribed displacements
MASS MODELLING
No mass
OUTPUT
Forces and moments per unit length of flaw for fracture modes I, II and III and
the associated relative displacements and rotations are available at all
integration points. In addition, the mode I, II and III stress intensity factors,
the plastic part of the J-integral and the total J are also printed at each
integration point.
INTEGRATION RULES
3 point Simpson’s rule along the flaw (i.e. 3x1x1) and this cannot be changed.
LOCAL AXES
Local X’ axis is tangential to the curvilinear ξ axis, positive in the direction of
node 1 to node 3. The local Y’ axis lies in the plane through the orientation
node and the local X’ axis, positive towards the orientation node. Local Z’
forms a right handed set with local X’ and local Y’.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-59
LSP3
Appendix A
ASAS (Non-Linear) User Manual
NOTES
1.
The element is written for small displacement analysis only, i.e. large displacement effects are not included
and should not be specified.
2.
Thermal strain effects are not included.
3.
Plasticity is included for mode I response only, so that elasto-plastic analysis should only be carried out
with LSP3 or with LSP6 when mode I behaviour dominates. Significant approximations have been made
in the plasticity model and therefore this should be used with care.
4.
The amount of plastic work of the numerical model can be adjusted using the PARA command FACLSP
(default 0.4) to provide a matching to the experiment results for an edge-cracked specimen.
REFERENCE
A. 6
, A. 7
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-60
LSP6
Appendix A
ASAS (Non-Linear) User Manual
Line-Spring Element Compatible with Quadratic Shell Elements for
Modelling Surface Flaws
NUMBER OF NODES
6
6
5
NODAL COORDINATES
x, y, z
4
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ
GEOMETRIC PROPERTIES
d1
t1
Crack depth at node 1
Shell thickness at node 1
d2
Crack depth at node 2
t2
d3
Shell thickness at node 2
Crack depth at node 3
2
1
t3
Shell thickness at node 3
x1, y1, z1 Orientation node coordinates for node 1
x2, y2, z2 Orientation node coordinates for node 2
x3, y3, z3 Orientation node coordinates for node 3
The orientation node is a node in the plane of the crack, pointing in the
direction of the surface from which the crack originates.
(Note - d is +ve if a flaw lies on the +ve Z’ side and vice versa)
MATERIAL MODELS
ELASTIC
-
Isotropic only
PLASTIC
-
von Mises yield criterion
Isotropic hardening only
LOAD TYPES
Nodal loads
Prescribed displacements
MASS MODELLING
No mass
OUTPUT
Forces and moments per unit length of flaw for fracture modes I, II and III and
the associated relative displacements and rotations are available at all
integration points. In addition, the mode I, II and III stress intensity factors,
the plastic part of the J-integral and the total J are also printed at each
integration point.
INTEGRATION RULES
3 point Simpson’s rule along the flaw (i.e. 3x1x1) and this cannot be changed.
LOCAL AXES
Local X’ axis is tangential to the curvilinear ξ axis, positive in the direction of
node 1 to node 3. The local Y’ axis lies in the plane through the orientation
node and the local X’ axis, positive towards the orientation node. Local Z’
forms a right handed set with local X’ and local Y’.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-61
3
LSP6
Appendix A
ASAS (Non-Linear) User Manual
NOTES
1.
The element is written for small displacement analysis only, i.e. large displacement effects are not included
and should not be specified.
2.
Thermal strain effects are not included.
3.
Plasticity is included for mode I response only, so that elasto-plastic analysis should only be carried out
with LSP3 or with LSP6 when mode I behaviour dominates. Significant approximations have been made
in the plasticity model and therefore this should be used with care.
4.
The amount of plastic work of the numerical model can be adjusted using the PARA command FACLSP
(default 0.4) to provide a matching to the experiment results for an edge-cracked specimen.
REFERENCE
A. 6
, A. 7
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-62
QMT4
Appendix A
ASAS (Non-Linear) User Manual
Quadrilateral Membrane Field Element with Quasi-linear Variation
of Field Variable
NUMBER OF NODES
4
NODAL COORDINATES
x, y, (z)
z should be omitted for 2-D problems.
DEGREES OF FREEDOM
T at each node.
GEOMETRIC PROPERTIES
ti Thickness at node i (i=1,4),
t2 to t4 may be omitted for an element with
uniform thickness t1.
No geometric property required with PLSN option. In this case, the geometric
property integer in the topology data should also be omitted.
MATERIAL MODELS
FIELD
PIER
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal values related to field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at integration points related to either global
or local axes (local by default).
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise.
INTEGRATION RULES
2x2 Gauss quadrature by default. Other rules by request. Appendix -G gives
position of integration points.
3
Y'
LOCAL AXES
Invariant throughout element. Local
X’ lies along the straight line from
σx'y'
4
node 1 towards node 2. Local Y’ is
σx'x'
in the plane of the element
perpendicular to local X’ and +ve
towards node 3. Local Z’ forms a
right-handed set with local X’ and
σy'y'
1
X'
2
local Y’.
SIGN CONVENTION
Fluxes and gradients are positive when in the positive axis direction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-63
QMT4
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-64
QMT8
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Quadrilateral Membrane Field Element with Quasi-quadratic Variation
of Field Variable
NUMBER OF NODES
8
NODAL COORDINATES
x, y, (z)
z should be omitted for 2D problems.
6
7
5
Coordinates may be omitted for midside nodes on straight edges, but if
4
8
given each node must be within side/10
of the true mid-side.
3
1
DEGREES OF FREEDOM
T at each node.
GEOMETRIC PROPERTIES
ti Thickness at node i (i=1,8)
2
t2 to t8 may be omitted for an element with uniform thickness t1.
No geometric property required with PLSN option. In this case, the geometric
property integer in the topology data should also be omitted.
MATERIAL MODELS
FIELD
PIER
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal values related to field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at integration points related to either global
or local axes (local by default).
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
corner node.
INTEGRATION RULES
2x2 Gauss quadrature by default. Other rules by request. Appendix -G gives
position of integration points.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-65
QMT8
Appendix A
ASAS (Non-Linear) User Manual
LOCAL AXES
Local X’ lies on the element surface. For
flat elements, it is a straight line parallel to
a line through nodes 1 and 3.
For
elements curved out-of-plane, it is the
intersection of the element surface with
the plane containing the surface normal
and the straight line through nodes 1 and
3.
Local Y’ is in the surface,
perpendicular to local X’ and +ve towards
node 5. Local Z’ forms a right-handed set
with local X’ and local Y’.
SIGN CONVENTION
Fluxes and gradients are positive when in the positive axis direction
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-66
QUM4
Appendix A
ASAS (Non-Linear) User Manual
Quadrilateral Membrane Element with Quasi-linear Strain Variation
This element can be used for both plane strain and plane stress applications in two and three dimensions.
REQUIRED OPTIONS
PLSN
- 2-D Classical Plane Strain (εz = 0.0)
EPSN
- 2-D Engineering Plane Strain (εz = const.)
TWOD - 2-D Plane Stress
none
- 3-D Plane Stress
3
4
NUMBER OF NODES
4
NODAL COORDINATES
x, y, (z)
z should be omitted for plane strain
and 2-D plane stress forms.
DEGREES OF FREEDOM
X Y, for Plane Strain and 2-D plane
stress forms.
2
1
X,Y,Z for 3-D Plane stress.
Deformations out-of-plane must be suppressed or restrained by adjacent
elements.
GEOMETRIC PROPERTIES
MATERIAL MODELS
Plane strain
-
None (the geometric property integer with the element
topology data should also be omitted)
Plane stress
-
ti Thickness at node i (i=1,4),
t2 to t4 may be omitted for an element with uniform
thickness t1.
ELASTIC
-
Isotropic
Orthotropic
-
Woven
Anisotropic
Anisotropic matrix C (or C-1) defined in axis system
selected for output.
σxx
σyy
σxy
σzz
=
C1 C2
.
C3
.
.
.
.
C4
C5
C6
.
C7
C8
C9
C10
εxx
εyy
εxy
εzz
4 coefficients of thermal expansion αxx, αyy, αxy, αzz,
referred to axis system selected for output
-
Hyperelastic
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-67
QUM4
Appendix A
ASAS (Non-Linear) User Manual
PLASTIC
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
criteria
yield
Isotropic, Kinematic (Ziegler) or Combined Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal Loads
Prescribed displacements
Edge pressure loads (on any side, +ve towards the element centre)
Normal pressure loads (+ve for +ve local z’ direction)
Distributed load patterns ML1, ML2, ML3
Temperature loads
Body forces
Centrifugal loads
Angular accelerations
Tank Loads
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points referred to either global
or element local axes (local by default). Note global should not be used with
elements in the 3-D Plane stress form.
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise.
INTEGRATION RULES
2x2 Gauss quadrature by default. Other rules by request. Appendix -G gives
position of integration points.
LOCAL AXES
Invariant throughout element. Local
X’ lies along the straight line from
node 1 towards node 2. Local Y’ is
in the plane of the element
perpendicular to local X’ and +ve
towards node 3. Local Z’ forms a
right-handed set with local X’ and
local Y’.
SIGN CONVENTION
Direct stresses σxx, σyy, σzz
+ve for tension
Shear stress σxy
+ve as shown
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-68
QUM4
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
With the EPSN option, one extra node, with number MAXND+1 (MAXND is the maximum node number
on the structure), is automatically added to the structure. The node has εz as its only freedom, which is
reported in the displacement output. As this extra node is common to all elements, εz is constant for the
entire structure.
2.
2-D elements with global stress output must be used if fracture mechanics processing in POSTNL is
required.
REFERENCE
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-69
QUM8
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Quadrilateral Membrane with Quasi-quadratic Strain Variation
This element can be used for both plane strain and plane stress applications in two and three dimensions.
REQUIRED OPTIONS
PLSN
- 2-D Classical Plane Strain (εz = 0.0)
EPSN - 2-D Engineering Plane Strain (εz = const.)
TWOD - 2-D Plane Stress
none
- 3-D Plane Stress
6
7
NUMBER OF NODES
8
NODAL COORDINATES
x, y, (z)
z should be omitted for plane strain and
5
4
8
2-D plane stress forms.
Coordinates may be omitted for midside nodes on straight edges, but if
given each node must be within side/10
3
2
1
of the true mid-side.
DEGREES OF FREEDOM
X, Y for Plane strain and 2-D Plane stress forms
X, Y, Z for 3-D Plane stress.
Deformations out-of-plane must be suppressed or restrained by adjacent
elements.
GEOMETRIC PROPERTIES
Plane strain
- None (the geometric property integer with the topology
data should also be omitted).
Plane stress
- ti Thickness at node i (i=1,8), t2 to t8 may be omitted for
an element with uniform thickness t1.
MATERIAL MODELS
ELASTIC
-
Isotropic
-
Orthotropic
Woven
-
Anisotropic
Anisotropic matrix C (or C-1) defined in axis system
selected for output
σxx
σyy
σxy
σzz
=
C1 C2
.
C3
.
.
.
.
C4
C5
C6
.
C7
C8
C9
C10
εxx
εyy
εxy
εzz
4 coefficients of thermal expansion αxx, αyy, αxy, αzz,
referred to axis system selected for output.
-
Hyperelastic
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-70
QUM8
Appendix A
ASAS (Non-Linear) User Manual
PLASTIC
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
criteria
yield
Isotropic, Kinematic (Ziegler) or Combined Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal Loads
Prescribed displacements
Edge pressure loads (on any side, +ve towards the element centre)
Normal pressure loads (+ve for +ve local z’ direction)
Distributed load patterns ML1, ML2, ML3
Temperature loads
Body forces
Centrifugal forces
Centrifugal loads
Angular accelerations
Tank Loads
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points referred to either global
or element local axes (local by default). Note global should not be used with
elements in the 3-D Plane stress form.
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise.
INTEGRATION RULES
2x2 Gauss quadrature by default. Other rules by request. Appendix -G gives
position of integration points.
LOCAL AXES
Local X’ lies on the element surface.
For flat elements, it is a straight line
parallel to a line through nodes 1 and 3.
For elements curved out-of-plane, it is
the intersection of the element surface
with the plane containing the surface
normal and the straight line through
nodes 1 and 3.
Local Y’ is in the
surface, perpendicular to local X’ and
+ve towards node 5. Local Z’ forms a
right-handed set with local X’ and local
Y’.
SIGN CONVENTION
Direct stresses σxx, σyy, σzz
Shear stress σxy
+ve for tension
+ve as shown
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-71
QUM8
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
With the EPSN option, one extra node, with number MAXND+1 (MAXND is the maximum node number
on the structure), is automatically added to the structure. The node has εz as its only freedom, which is
reported in the displacement output. As this extra node is common to all elements, εz is constant for the
entire structure.
2.
2-D elements with global stress output must be used if fracture mechanics processing in POSTNL is
required.
REFERENCE
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-72
QUS4
Appendix A
ASAS (Non-Linear) User Manual
Quadrilateral Element with Linearly Varying Thickness
for Modelling Thin or Thick Shells
NUMBER OF NODES
4
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ at each node.
GEOMETRIC PROPERTIES
ti Thickness at node i (i = 1,4),
t2 to t4 may be omitted for an element with
3
4
uniform thickness t1. Additional lay-up data is
required for laminated material option.
See Section 5.2.5.3 for the LAMI command.
MATERIAL MODELS
ELASTIC
Nx’x’
Νy’y’
Νx’y’
Mx’x’
My’y’
Mx’y’
Qx’z’
Qy’z’
2
1
-
Isotropic
Orthotropic
Woven
-
Anisotropic
Anisotropic matrix C (not C-1) defined in element
material axes. (see Appendix B.1.2)
Coefficients C1-C24 required. Note that they do not
contain the thickness.
C1t C2t C4t
.
C3t C5t
.
. C6t
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
=
C7t2
C8t2
C9t2
C10t3
.
.
.
.
C11t2
C12t2
C13t2
C14t3
C15t3
.
.
.
C16t2 0
0
C17t2 0
0
C18t2 0
0
3
C19t 0
0
C20t3 0
0
C21t3 0
0
. C22t C23t
.
. C24t
εx’x’
εy’y’
εx’y’
yx’x’
yy’y’
yx’y’
εx’z’
εy’z’
3 coefficients of thermal expansion αxx, αyy, αxy referred to
local axes.
PLASTIC
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
criteria.
yield
Isotropic, Kinematic (Ziegler) or Combined Hardening.
Ivanov yield criterion with Isotropic hardening.
CREEP
-
von Mises
FAIL
-
lamina failure law for composites
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-73
QUS4
ASAS (Non-Linear) User Manual
LOAD TYPES
Appendix A
Nodal loads
Prescribed displacements
Pressure loads (+ve for +ve local Z’ direction)
Distributed load patterns ML1, ML2, ML3
Temperature loads
Face temperature loads (Face 1 is on the -ve local Z’ side)
Body forces
Centrifugal loads
Angular accelerations
Tank Loads
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-74
QUS4
ASAS (Non-Linear) User Manual
Appendix A
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses, strains and stress resultants are available at all integration points
referred to element local axes. For Ivanov (full section) models only stress and
strain resultants are available. In addition, the stress indicators are printed for
plastic points.
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise.
INTEGRATION RULES
1 point Gaussian integration in the plane and 3 point Newton-Cotes through
thickness by default. 2x2 Gauss rule in the plane by request. Other in-plane
rules not recommended. See Appendix -G for positions of integration points.
LOCAL AXES
Local X’,Y’,Z’ form a right- handed
orthogonal system which, in general,
varies in orientation from point to
point within the element. At any
point P in the element, X’ and Y’ lie
in the tangent plane at P. The
tangent plane is the plane containing
the vectors PR and PS which are
vectors tangent to the curvilinear ξ
and η directions respectively. X’
and Y’ are positioned in the tangent
plane such that the angle between
PR and X’ equals the angle between
PS and Y’.
SIGN CONVENTIONS
REFERENCE
Direct forces/unit width Νx’x’, Νy’y’, Νx’y’
+ve as shown.
Bending moments/unit width Μx’x’, Μy’y’, Μx’y’
Shear forces/unit width Qx’z’, Qy’z’
+ve as shown.
+ve as shown.
A. 3
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-75
QUX4
Appendix A
ASAS (Non-Linear) User Manual
Axisymmetric Quadrilateral Element With Straight Sides
Z
NUMBER OF NODES
4
NODAL COORDINATES
r, z
(Note that r and z occupy the first and
4
third fields with coordinate data using
1
3
2
an unnamed cartesian system)
DEGREES OF FREEDOM
R, Z at each node
(Any skew system must be 2-D. Of the six direction cosines R’R, R’θ, R’Z,
Z’R, Z’θ, Z’Z, the values R’θ and Z’θ must be zero).
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
ELASTIC
-
Isotropic
Orthotropic
-
Woven
Anisotropic
Anisotropic matrix C (or C-1) - referred to axis system
selected for output (global by default)
σrr
σzz
σθθ
σrz
=
C1 C2
.
C3
.
.
.
.
C4
C5
C6
.
C7
C8
C9
C10
εrr
εzz
εθθ
εrz
4 coefficients of thermal expansion αrr, αzz, αθθ, αrz,
referred to axis system selected for output
PLASTIC
-
Hyperelastic
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
Isotropic, Kinematic (Prager or Ziegler) or Combined
Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-76
QUX4
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal Loads (must be defined per radian)
Prescribed displacements
Pressure loads (on any side, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points in global or local element
axes (global by default)
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise.
INTEGRATION RULES
2x2 rule used by default. Higher order rules by request. Appendix -G gives
position of integration points.
LOCAL AXES
Invariant throughout the element. Local R’ lies along the line from node 1 to
node 2. Local Z’ is perpendicular to local R’, in the global rz plane, and lies
counter clockwise from R’.
SIGN CONVENTIONS
Direct stresses σrr, σzz, σθθ
Shear stress σrz
+ve for tension
+ve as shown
z
r
NOTE
Global stress output must be used if fracture mechanics processing in POSTNL
is required.
REFERENCE
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-77
QUX8
Appendix A
ASAS (Non-Linear) User Manual
Axisymmetric Isoparametric Quadrilateral Element
Z
NUMBER OF NODES
8
NODAL COORDINATES
r, z
(may be omitted for mid-side nodes
7
on a straight edge). Note that r and z
8
occupy the first and third fields with
coordinate data using an unnamed
1
6
5
4
2
3
cartesian system.
DEGREES OF FREEDOM
R, Z at each node
(Any skew system must be 2-D. Of the six direction cosines R’R, R’θ, R’Z,
Z’R, Z’θ, Z’Z, the values R’θ and Z’θ must be zero)
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
ELASTIC
-
Isotropic
Orthotropic
-
Woven
Anisotropic
Anisotropic matrix C (or C-1) - referred to axis system
selected for output (global by default)
σrr
σzz
σθθ
σrz
=
C1 C2
.
C3
.
.
.
.
C4
C5
C6
.
C7
C8
C9
C10
εrr
εzz
εθθ
εrz
4 coefficients of thermal expansion αrr, αzz, αθθ, αrz,
referred to axis system selected for output
PLASTIC
-
Hyperelastic
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
Isotropic, Kinematic (Prager or Ziegler) or Combined
Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-78
QUX8
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal Loads (must be defined per radian)
Prescribed displacements
Pressure loads (on any side, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses and strains are available at integration points in global or local element
axes (global by default)
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
corner node.
INTEGRATION RULES
2x2 rule used by default. Higher order rules by request. Appendix -G gives
position of integration points.
LOCAL AXES
Invariant throughout the element. Local R’ lies along the line from node 1 to
node 2. Local Z’ is perpendicular to local R’, in the global rz plane, and lies
counter clockwise from R’.
SIGN CONVENTIONS
Direct stresses σrr, σzz, σhh
Shear stress σrz
+ve for tension
+ve as shown
z
r
NOTE
Global stress output must be used if fracture mechanics processing in POSTNL
is required.
REFERENCE
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-79
QXT4
ASAS (Non-Linear) User Manual
Appendix A
Axisymmetric Quadrilateral Field Element with Quasi-linear Variation
of Field Variable
NUMBER OF NODES
4
NODAL COORDINATES
r, z
(Note that r and z occupy the first and
third fields with coordinate data using
Z
4
3
1
an unnamed cartesian system)
DEGREES OF FREEDOM
T at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
FIELD
2
PIER
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal values related to field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at integration points related to either global
or local axes (global by default).
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise.
INTEGRATION RULES
2x2 rule used by default. Higher order rules by request. Appendix -G gives
position of integration points.
LOCAL AXES
Invariant throughout the element. Local R’ lies along the line from node 1 to
node 2. Local Z’ is perpendicular to local R’, in the global rz plane, and lies
counter clockwise from R’.
SIGN CONVENTION
Fluxes and gradients are positive when in the positive axis direction
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-80
ASAS (Non-Linear) User Manual
3.
Appendix A
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-81
QXT8
ASAS (Non-Linear) User Manual
Appendix A
Axisymmetric Isoparametric Quadrilateral Field Element with Quasi-quadratic
Variation of Field Variable
Z
NUMBER OF NODES
8
NODAL COORDINATES
r, z
(may be omitted for mid-side nodes
on a straight edge). Note that r and z
7
6
5
4
8
1
occupy the first and third fields with
2
3
coordinate data using an unnamed
cartesian system.
DEGREES OF FREEDOM
T at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
FIELD
PIER
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal values related to field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at integration points related to either global
or local axes (global by default).
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
corner node.
INTEGRATION RULES
2x2 rule used by default. Higher order rules by request. Appendix -G gives
position of integration points.
LOCAL AXES
Invariant throughout the element. Local R’ lies along the line from node 1 to
node 2. Local Z’ is perpendicular to local R’, in the global rz plane, and lies
counter clockwise from R’.
SIGN CONVENTION
Fluxes and gradients are positive when in the positive axis direction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-82
QXT8
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-83
RGX3
Appendix A
ASAS (Non-Linear) User Manual
Linear Axisymmetric Rigid Surface Contact Element
2
NUMBER OF NODES
3
NODAL COORDINATES
r, z
DEGREES OF FREEDOM
R, Z
1
3
GEOMETRIC PROPERTIES
No basic geometric property.
RIGS required to define the geometry of rigid surface.
(See Section 5.2.5.4)
MATERIAL MODELS
ELASTIC
PLASTIC
-
K is the normal contact stiffness (stress/penetration)
Coulomb friction
Frictionless surface is assumed if no plastic material data.
LOAD TYPES
OUTPUT
Nodal loads,
Prescribed displacements
The gap size, GAP in the X’-direction and sliding displacement SLIDE-Y are
related to local axes. Stress across the gap, STRESS-XX and frictional stress,
STRESS-YY are related to the local axes.
INTEGRATION RULES
LOCAL AXES
2 point Newton-Cotes (Trapezoidal rule) along the interface at nodes 1 and 2
(i.e. 2x1x1)
Local X’ lies normal to the rigid surface and passes through the integration
point. Local Y’ lies in the global rz plane, perpendicular to local X’ (ie
tangential to the rigid surface).
2
1
X'
Y'
SIGN CONVENTIONS
σx’x’
σy’y’
+ve direction of
rigid surface
is positive when compressive.
is positive when it acts in negative y’ direction
GAP is positive when penetrated
SLIDE-
Yis positive when sliding in the +ve Y’ direction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-84
RGX3
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Node 3 is the rigid body reference node and should always be either suppressed or prescribed. Nodes 1 and
2 should be on the deforming body.
2.
It is always assumed that the structure is separated from the rigid surface at the beginning of an analysis
and therefore care must be taken to ensure that singularity is not present at time t=0.0. If the structure is
not properly supported initially, the user will have to put in sufficient boundary conditions to avoid the
singularity. These boundary conditions can then be removed once the contact condition with the rigid
surface is established.
3.
If contact is made at the very first step, it is assumed that no sliding or frictional stress will be developed
during this step. Because of this restriction, it is advisable to solve at t=0.0 first before proceeding the
analysis further.
4.
Augmented Lagrangian procedure is invoked by specifying the maximum number of augmentation steps
required, MXAUGM, in the PARA command. See also Appendix C.6.
REFERENCE
A. 8
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-85
RGX4
Appendix A
ASAS (Non-Linear) User Manual
Quadratic Axisymmetric Rigid Surface Contact Element
NUMBER OF NODES
4
NODAL COORDINATES
r, z
3
2
1
DEGREES OF FREEDOM
R, Z
4
GEOMETRIC PROPERTIES
No basic geometric property.
RIGS required to define the geometry of rigid surface.
(See Section 5.2.5.4)
MATERIAL MODELS
ELASTIC
PLASTIC
-
K is the normal contact stiffness (stress/penetration)
Coulomb friction
Frictionless surface is assumed if no plastic material data
LOAD TYPES
Nodal loads,
Prescribed displacements
OUTPUT
The gap size, GAP in the X’-direction and sliding displacement SLIDE-Y are
related to local axes. Stress across the gap, STRESS-XX and frictional stress,
STRESS-YY are related to the local axes.
INTEGRATION RULES
3 point Newton-Cotes (Simpson’s rule) along the interface at nodes 1, 2 and 3
(i.e. 3x1x1)
LOCAL AXES
Local X’ lies normal to the rigid surface and passes through the integration
point. Local Y’ lies in the global rz plane, perpendicular to local X’ (ie
tangential to the rigid surface).
3
2
1
X'
Y'
SIGN CONVENTIONS
+ve direction of
rigid surface
σx’x’
σy’y’
is positive when compressive.
is positive when it acts in negative y’ direction
GAP
is positive when penetrated
SLIDE-Y
is positive when sliding in the +ve Y’ direction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-86
RGX4
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Node 4 is the rigid body reference node and should always be either suppressed or prescribed. Nodes 1, 2
and 3 should be on the deforming body.
2.
It is always assumed that the structure is separated from the rigid surface at the beginning of an analysis
and therefore care must be taken to ensure that singularity is not present at time t=0.0. If the structure is
not properly supported initially, the user will have to put in sufficient boundary conditions to avoid the
singularity. These boundary conditions can then be removed once the contact condition with the rigid
surface is established.
3.
If contact is made at the very first step, it is assumed that no sliding or frictional stress will be developed
during this step. Because of this restriction, it is advisable to solve at t=0.0 first before proceeding the
analysis further.
4.
Augmented Lagrangian procedure is invoked by specifying the maximum number of augmentation steps
required, MXAUGM, in the PARA command. See also Appendix C.6.
REFERENCE
A. 8
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-87
RG23
Appendix A
ASAS (Non-Linear) User Manual
Linear 2-D Rigid Surface Contact Element
2
NUMBER OF NODES
3
NODAL COORDINATES
x, y
Option TWOD must be specified
DEGREES OF FREEDOM
X, Y
GEOMETRIC PROPERTIES
(i)
3
Basic Properties
Plane stress -
Plane strain (ii)
MATERIAL MODELS
1
ti thickness at node i (i=1,2) (>0.0)
t2 may be omitted for an element with uniform
thickness t1.
no basic geometric property
RIGS required to define the geometry of the rigid surface
(see Section 5.2.5.4)
ELASTIC
PLASTIC
-
K is the normal contact stiffness (stress/penetration)
Coulomb friction
Frictionless surface is assumed if no plastic material data
LOAD TYPES
Nodal loads,
Prescribed displacements
OUTPUT
The gap size, GAP in the X’-direction and sliding displacement SLIDE-Y are
related to local axes. Stress across the gap, STRESS-XX and frictional stress,
STRESS-YY are related to the local axes.
INTEGRATION RULES
LOCAL AXES
2 point Newton-Cotes (Trapezoidal rule) along the interface at nodes 1 and 2
(i.e. 2x1x1)
Local X’ lies normal to the rigid surface and passes through the integration
point. Local Y’ lies in the global xy plane, perpendicular to local X’ (ie
tangential to the rigid surface).
2
1
X'
Y'
SIGN CONVENTIONS
σx’x’
σy’y’
+ve direction of
rigid surface
is positive when compressive.
is positive when it acts in negative Y’ direction
GAP
is positive when penetrated
SLIDE-Y
is positive when sliding in the +ve Y’ direction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-88
RG23
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Node 3 is the rigid body reference node and should always be either suppressed or prescribed. Nodes 1 and
2 should be on the deforming body.
2.
It is always assumed that the structure is separated from the rigid surface at the beginning of an analysis
and therefore care must be taken to ensure that singularity is not present at time t=0.0. If the structure is
not properly supported initially, the user will have to put in sufficient boundary conditions to avoid the
singularity. These boundary conditions can then be removed once the contact condition with the rigid
surface is established.
3.
If contact is made at the very first step, it is assumed that no sliding or frictional stress will be developed
during this step. Because of this restriction, it is advisable to solve at t=0.0 first before proceeding the
analysis further.
4.
Augmented Lagrangian procedure is invoked by specifying the maximum number of augmentation steps
required, MXAUGM, in the PARA command. See also Appendix C.6.
REFERENCE
A. 8
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-89
RG24
Appendix A
ASAS (Non-Linear) User Manual
Quadratic 2-D Rigid Surface Contact Element
NUMBER OF NODES
4
NODAL COORDINATES
x, y
Option TWOD must be specified
DEGREES OF FREEDOM
X, Y
GEOMETRIC PROPERTIES
(i)
Basic Properties
Plane strain -
MATERIAL MODELS
1
4
Plane stress -
(ii)
3
2
ti thickness at node i (i=1,3) (>0.0)
t2 and t3 may be be omitted for an element with
uniform thickness t1.
no basic geometric property
RIGS required to define the geometry of the rigid surface
(see Section 5.2.5.4)
ELASTIC
PLASTIC
-
K is the normal contact stiffness (stress/penetration)
Coulomb friction
Frictionless surface is assumed if no plastic material data
LOAD TYPES
Nodal loads,
Prescribed displacements
OUTPUT
The gap size, GAP in the X’-direction and sliding displacement SLIDE-Y are
related to local axes. Stress across the gap, STRESS-XX and frictional stress,
STRESS-YY are related to the local axes.
INTEGRATION RULES
LOCAL AXES
3 point Newton-Cotes (Simpson’s rule) along the interface at nodes 1, 2 and 3
(i.e. 3x1x1)
Local X’ lies normal to the rigid surface and passes through the integration
point. Local Y’ lies in the global xy plane, perpendicular to local X’ (ie
tangential to the rigid surface).
3
2
1
X'
Y'
SIGN CONVENTIONS
+ve direction of
rigid surface
σx’x’
σy’y’
is positive when compressive.
is positive when it acts in negative Y’ direction
GAP
SLIDE-Y
is positive when penetrated
is positive when sliding in the +ve Y’ direction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-90
RG24
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Node 4 is the rigid body reference node and should always be either suppressed or prescribed. Nodes 1, 2
and 3 should be on the deforming body.
2.
It is always assumed that the structure is separated from the rigid surface at the beginning of an analysis
and therefore care must be taken to ensure that singularity is not present at time t=0.0. If the structure is
not properly supported initially, the user will have to put in sufficient boundary conditions to avoid the
singularity. These boundary conditions can then be removed once the contact condition with the rigid
surface is established.
3.
If contact is made at the very first step, it is assumed that no sliding or frictional stress will be developed
during this step. Because of this restriction, it is advisable to solve at t=0.0 first before proceeding the
analysis further.
4.
Augmented Lagrangian procedure is invoked by specifying the maximum number of augmentation steps
required, MXAUGM, in the PARA command. See also Appendix C.6.
REFERENCE
A. 8
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-91
SPR1
Appendix A
ASAS (Non-Linear) User Manual
Translational Spring/Dashpot Element
2
NUMBER OF NODES
2
NODAL COORDINATES
x, y, (z)
z should be omitted for TWOD option
C
K
1
DEGREES OF FREEDOM
X, Y, (Z), at each node
GEOMETRIC PROPERTIES
(i)
(ii)
(iii)
MATERIAL PROPERTIES
ELASTIC - Isotropic (Not used but material integer must be specified.)
PLASTIC - Inelastic spring, SPRG
LOAD TYPES
Nodal loads
Prescribed displacements.
MASS MODELLING
No mass (use added mass).
OUTPUT
Spring force, relative displacement, damping force and relative velocity in
Global coordinates of a point defining line of action of spring
Linear stiffness K or tabulated values of displacement and force
Linear damping factor C or tabulated values of velocity and force
spring direction.
LOCAL AXES
If the global coordinates P specified in the geometric properties data are all
zero, local X’ lies along the element from node 1 to node 2. For other cases,
local X’ is defined by the position vector OP, where O is the origin of the
global axes.
SIGN CONVENTIONS
Forces are positive in tension.
Displacements are positive when node 2 moves positively relative to node1.
NOTES
1.
If the coordinates of P are all zero, nodes 1 and 2 must not be coincident.
2.
Elastic behaviour is always assumed for damping.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-92
SPR2
Appendix A
ASAS (Non-Linear) User Manual
Rotational Spring/Dashpot Element
NUMBER OF NODES
2
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
RX, RY, RZ, at each node
GEOMETRIC PROPERTIES
(i)
(ii)
Global coordinates of a point, P, defining line of action of spring
Linear rotational stiffness K or tabulated values of moment and rotation
and moment.
(iii)
Linear damping factor C or tabulated values of moment and
angular velocity and moment.
MATERIAL PROPERTIES
ELASTIC - Isotropic (Not used but material integer must be specified.)
PLASTIC - Inelastic spring, SPRG.
LOAD TYPES
Nodal loads
Prescribed displacements.
MASS MODELLING
No mass (use added mass).
OUTPUT
Spring moment, relative rotation, damping moment and relative angular
velocity.
LOCAL AXES
If the global coordinates P specified in the geometric properties data are all
zero, local X’ lies along the element from node 1 to node 2. For other cases,
local X’ is defined by the position vector OP, where O is the origin of the
global axes.
SIGN CONVENTIONS
Rotations are positive when node 2 rotates positively relative to node 1.
NOTES
1.
If the coordinates of P are all zero, nodes 1 and 2 must not be coincident.
2.
Elastic behaviour is always assumed for damping.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-93
SST4
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Beam/Stiffener Element having Thin-walled
Open Cross-sections of Arbitrary Shape (no warping)
NUMBER OF NODES
4 (2 end, 1 mid-length and 1 auxiliary node).
NODAL COORDINATES
X, Y, Z (may be omitted for mid-length
node on a straight element). The mid-
2
4
3
length node has tolerance of length/10
about the true mid-length. The auxiliary
node is only used to define the local axes
s
1
(see below).
r
t
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ.
GEOMETRIC PROPERTIES
The element can have any open thin-walled cross-section made up of straight
sided segments, connected at median points.
The element has special
geometric properties (see Geometric Property Section 5.2.5.1).
RMUL
-
Rigidity multiplier (= 1.0 - to represent full
cross-section, or = 0.5 to represent half symmetric
cross-section).
Repeat this
for each
segment
s,t
- Local coordinates to define median points in plane of
cross-section.
IA,IB
-
Local connectivity.
NSTAT
NLAY
-
Number of integration stations along the segment.
Number of integration layers through segment thickness.
T
-
Segment thickness.
The cross-section of the element is assumed constant along the length
(Geometric Properties at nodes 2 and 3 need not be supplied).
MATERIAL MODEL
ELASTIC
PLASTIC
-
Isotropic
von-Mises
Isotropic Hardening
Material properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-94
SST4
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal loads
Prescribed displacements.
Body forces
Centrifugal loads
Angular accelerations
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Direct stress σrr, shear stress σrm, (referred to segment axes) and stress
resultants (in element local axes) are available as follows.
STRS:
stresses at all integration points on element
SSTR:
smoothed stresses for all integration points at 2 cross-sections
corresponding to 2 point Gauss rule on length.
ESTR:
smoothed stresses for top and bottom layers at end of each
segment (ie extreme fibrepoints) at 2 cross-sections
corresponding to 2 point Gauss rule on length.
SRES:
stress resultants at all 4 Gauss points along the length
SSRE:
smoothed stress resultants at 2 cross-sections corresponding
to 2 point Gauss rule on length
Strains and strain resultants are not available
For elastic analysis, only stress resultants (i.e. SRES or SSRE) are available.
INTEGRATION RULES
4 Point Gauss Quadrature along length (invariant and independent of stress
output). User defined trapezoidal rule for each segment. (NO DEFAULT) see Geometric Properties Data. As a guide the following are suggested:
Elastic - 2 stations, 1 layer
Plastic - 5 stations, 4 layers
NODE NUMBERING
Node 3 is always the MID-LENGTH node and 4 the auxiliary node.
LOCAL AXES r, s, t
Independent of cross-sectional shape - ie s, t do not have to coincide with
principal axes of the cross-section. Local r is tangential to the curvilinear
nodal axis, positive in the direction node 1 to node 2. s is normal to the plane
containing the r-axis and node 4. t is orthogonal to r and s and points away
from node 4, ie positive t and the auxiliary node are on opposite sides of the r
axis.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-95
SST4
Appendix A
ASAS (Non-Linear) User Manual
SIGN CONVENTIONS
Axial force
Axial stress
+ve tension
+ve tension
Generalised stress resultants, +ve as shown
Fr
Qrs
-
axial force
shear along s
Qrt
Ms
-
shear along t
moment about s
Mt
Tsv
-
moment about t
St. Venant Torque
Mt
Qrt
Ms
t
Qrs
s
r
Fr
T sv
NOTES
1.
This element requires special Geometry Property and Residual stress input data (see Sections 5.2.5.1 and
5.6.3).
2.
Note that the element topology definition and local axes are not the same as the STF4 beam stiffener.
3.
Segment number 1 must start at free edge of the beam cross-section. Each subsequent segment must start
from the end of any previously numbered segment.
4.
Stress and stress resultant outputs always correspond to the full cross-section.
REFERENCE
A. 5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-96
STF4
Appendix A
ASAS (Non-Linear) User Manual
Curved Beam Element with Transverse Shear and Offset Nodes
for use with the TCS Family of Thick Shell Elements
NUMBER OF NODES
4 (2 end, 1 mid-length and 1
auxiliary node, see Note).
NODAL COORDINATES
3
4
Y'
2
x, y, z (may be omitted for midlength node on a straight element).
The mid-length node has a tolerance
length. The auxiliary node defines
the local axes.
Z'
1
of length/10 about the true mid-
X'
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ at nodes 1, 2, 3.
GEOMETRIC PROPERTIES
There are three types of cross sections available:
(a) Solid rectangular cross-section RECT (or blank) with the
geometric property data
For nodes 1, 2 and 3, in turn:
aY’ cross-sectional dimension of
local Y’ direction
Y'
aY'
Z'
aZ’
cross-sectional dimension of
local Z’ direction
eX’
nodal offset in local X’ direction
aZ'
eY’
eZ’
nodal offset in local Y’ direction
nodal offset in local Z’ direction
X' axis into paper
(b) Thin tubular cross-section TUBE - with the geometric
property data
For nodes 1, 2 and 3, in turn:
outer radius
ro
t
wall thickness (ro/t should be ≥ 10)
eX’
eY’
nodal offset in local X’ direction
nodal offset in local Y’ direction
eZ’
nodal offset in local Z’ direction
Note that +ve θ is the rotation from local Y’ towards local Z’.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-97
STF4
Appendix A
ASAS (Non-Linear) User Manual
(c) Thin hollow rectangular cross-section (Box-section) BOX - with
geometric property data.
the
Y'
For nodes 1, 2 and 3, in turn:
ao outer dimension of box in
local Y’ axis.
bo
outer dimension of box in
t1
local Z’ axis.
thickness of segment 1
t2
t3
thickness of segment 2
thickness of segment 3
t4
thickness of segment 4
eX’
eY’
nodal offset in local X’ direction
nodal offset in local Y’ direction
eZ’
nodal offset in local Z’ direction
1
t1
t2
4
ao
t4
t3
2
3
Z'
bo
X' axis into paper
In this case again thin section assumption is made, ao/(t2 or t4)>10 and
bo/(t1 or t3)>10. The hollow section is divided into four segments for
integration purposes. Numbering of segments is shown above. Segment 1 is
numbered where positive Y’ axis crosses the segment and segment 3 is
numbered where the negative Y’ axis crosses. Similarly segments 2 and 4 are
numbered where +ve and -ve Z’ axis crosses respectively.
MATERIAL MODEL
ELASTIC
PLASTIC
-
Isotropic
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
CREEP
-
Isotropic, Kinematic (Ziegler) or Combined Hardening.
von Mises
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements
Distributed load pattern CB1
Temperature loads
Body forces
Centrifugal loads
Angular acceleration
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses, strains and stress resultants are available at integration points referred
to element local axes. Stress point indicators for plastic points are also printed.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-98
STF4
Appendix A
ASAS (Non-Linear) User Manual
INTEGRATION RULES
(1) Rectangular cross-section.
2 point Gauss quadrature along length and 3 x 3 Newton-Cotes rules on crosssection by default (2 x 3 x 3). Other rules, by request, using the INTEgration
command in Preliminary data. Newton-Cotes points are equally spaced and
Appendix -G gives the positions of the Gauss integration points.
Examples
Y'
7
Y'
8
9
5
1
2
6
15
10
11
12
7
8
9 Z'
4
5
6
Z'
1 2 3 4
3
3x3=9
(default)
5
1
1x5=5
Y'
14
13
Z'
4
Y'
2
5x3=15
3
25
26
27
22
23
24
19
16
13
20
17
14
21
18
15
10
11
12
7
8
9
4
5
6
1
2
3
Z'
9x3=27
From the above examples it may be noted that the numbering of integration
points always start from the negative quadrant of Y’ Z’ axis.
Points are
numbered in the local Z’ axis direction (from -ve to +ve direction) first. Then
points are numbered in the local Y’ axis direction (from -ve to +ve direction)
as shown above.
(2) Tube cross-section
2 point Gauss quadrature along length and 8 points (Trapezoidal) equally
spaced around the tube periphery by default (ie 2x8x1 = NGX*NGY*NGZ).
Other rules, by request, using the INTEgration command in Preliminary data.
(Note that NGZ must be given but is not used) NGY should be a multiple of 4.
Examples
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-99
STF4
Appendix A
ASAS (Non-Linear) User Manual
The numbering of the integration points always start from the negative
quadrant of the Y’ Z’ axes as shown above. The points are equally spaced on
the circumference.
(3) Box cross-section
2 point Gauss quadrature along length and 12 point Newton-Cotes on crosssection by default (2x12x1). Other orders, by request, using the INTEgration
command in Preliminary data. NGY must be a multiple of 4 with a minimum
of 12.
Examples
Take NGY = 4n ; n = number of integration points for each segment
CL
Y'
Y'
Z'
5
5
1
3
2
4
5
4
4
CL
3
3
CL
CL
2
2
Z'
1
1
1
2
3
4
5
NGY = 20, n = 5
For the box section, there are the two stresses at each point on the segment.
These are the normal stress and the shear stress along the segment.
NODE NUMBERING
Node 2 is always the mid-length node and node 4 is the auxiliary node.
LOCAL AXES
Local X’ axis is tangential to the curvilinear centroidal axis, positive in the
direction of node 1 to node 3. The local Y’ axis lies in the plane through node
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-100
ASAS (Non-Linear) User Manual
Appendix A
4 and the local X’ axis, positive towards node 4. Local Z’ forms a righthanded set with local X’ and local Y’.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-101
STF4
Appendix A
ASAS (Non-Linear) User Manual
SIGN CONVENTIONS
OFFSETS
Axial force
+ve for tension
Axial stress
+ve for tension
Torque
+ve in positive direction of local axis
Bending Moment
+ve for sagging
Shear force
+ve in the local axes Y’ Z’ +ve direction
Offsets eX’, eY’, eZ’ +ve as shown. Note that the mid-length node cannot be
offset in the local X’ direction.
4
4
eX'
eX'
eZ'
Y'
1
Z'
X'
1
NOTE
2
3
eY'
The auxiliary node must be a dummy node and NOT a node on the structure.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-102
TCS6
Appendix A
ASAS (Non-Linear) User Manual
Generally Curved Degenerate Triangular Thick Shell Element
with Varying Thickness and Transverse Shear Capable of
Modelling Discontinuities in Curvature and Thickness
NUMBER OF NODES
6 (3 corner, 3 mid-side)
NODAL COORDINATES
x, y, z (may be omitted for mid-side nodes
on straight edges). Each mid-side node has
tolerance of side/10 about the true mid-side.
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ at each node.
GEOMETRIC PROPERTIES
ti Thickness at node i (i = 1,6),
t2 to t6 may be omitted for an element with uniform thickness.
Additional lay-up data is required for laminated material option.
See Section 5.2.5.3 for the LAMI command.
MATERIAL MODELS
ELASTIC
Nx’x’
Νy’y’
Νx’y’
Mx’x’
My’y’
Mx’y’
Qx’z’
Qy’z’
-
Isotropic
Orthotropic
Woven
-
Laminated
-
Anisotropic
Anisotropic matrix C (not C-1) defined in element
material axes. (See Appendix B.1.2)
Coefficients C1-C24 required. Note that they do not
contain the thickness.
=
C1t C2t C4t
.
C3t C5t
.
. C6t
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
C7t2
C8t2
C9t2
C10t3
.
.
.
.
C11t2
C12t2
C13t2
C14t3
C15t3
.
.
.
C16t2 0
0
C17t2 0
0
C18t2 0
0
3
C19t 0
0
C20t3 0
0
C21t3 0
0
. C22t C23t
.
. C24t
εx’x’
εy’y’
εx’y’
yx’x’
yy’y’
yx’y’
εx’z’
εy’z’
3 coefficients of thermal expansion αxx, αyy, αxy referred to
PLASTIC
-
CREEP
-
local axes.
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
Isotropic, Kinematic (Ziegler) or Combined Hardening.
Ivanov yield criterion with Isotropic hardening.
von Mises
FAIL
-
lamina failure law for composites
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-103
TCS6
ASAS (Non-Linear) User Manual
LOAD TYPES
Appendix A
Nodal Loads
Prescribed displacements
Pressure loads (+ve for +ve local Z’ direction)
Distributed load patterns ML1, ML2, ML3
Temperature loads
Face temperature loads (Face 1 is on the -ve local Z’ side)
Body forces
Centrifugal loads
Angular accelerations
Tank Loads
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-104
TCS6
Appendix A
ASAS (Non-Linear) User Manual
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses, strains and stress resultants are available at all integration points
referred to element local axes. For Ivanov (full section) models only stress and
strain resultants are available. In addition, the stress indicators are printed for
plastic points.
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
corner node.
INTEGRATION RULES
3 point triangular rule in plane and 3 point Newton-Cotes rule through
thickness (1x3x3) by default. Other rules by request, but only the through
thickness integration rule may be altered. See Appendix -G for positions of
integration points.
LOCAL AXES
Local X’, Y’, Z’ form a righthanded orthogonal system which, in
general, varies in orientation from
point to point within the element.
At any point P in the element, X’
and Y’ lie in the tangent plane at P.
The tangent plane is the plane
containing the vectors PR and PS
which are vectors tangent to the
curvilinear ξ
respectively.
and η directions
X’ and Y’ are
positioned in the tangent plane such
that the angle between PR and X’
equals the angle between PS and Y’.
SIGN CONVENTIONS
Direct forces/unit width Νx’x’, Νy’y’, Νx’y’
Bending moments/unit width Μx’x’, Μy’y’, Μx’y’
Shear forces/unit width Qx’z’, Qy’z’
REFERENCE
A. 2, A. 4, A. 5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
+ve as shown.
+ve as shown.
+ve as shown.
Page A-105
TCS8
Appendix A
ASAS (Non-Linear) User Manual
Generally Curved 8-Node Quadrilateral Thick Shell Element
with Varying Thickness and Transverse Shear,
Capable of Modelling Discontinuities in Curvature and Thickness
NUMBER OF NODES
8 (4 corner, 4 mid-side).
NODAL COORDINATES
x, y, z (may be omitted for mid-side nodes
on straight edges). Each mid-side node has
tolerance of side/10 about the true mid-side.
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ at each node.
GEOMETRIC PROPERTIES
ti Thickness at node i (i = 1,8),
t2 to t8 may be omitted for an element with uniform thickness t1.
Additional lay-up data is required for laminated material option.
See Section 5.2.5.3 for the LAMI command.
MATERIAL MODELS
ELASTIC
Nx’x’
Νy’y’
Νx’y’
Mx’x’
My’y’
Mx’y’
Qx’z’
Qy’z’
-
Isotropic
Orthotropic
-
Woven
-
Laminated
Anisotropic
Anisotropic matrix C (not C-1) defined in element
material axes. (See Appendix B.1.2)
Coefficients C1-C24 required. Note that they do not
contain the thickness.
C1t C2t C4t
.
C3t C5t
.
. C6t
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
=
PLASTIC
-
CREEP
FAIL
-
C7t2
C8t2
C9t2
C10t3
.
.
.
.
C11t2
C12t2
C13t2
C14t3
C15t3
.
.
.
C16t2 0
0
C17t2 0
0
2
C18t 0
0
C19t3 0
0
C20t3 0
0
C21t3 0
0
. C22t C23t
.
. C24t
εx’x’
εy’y’
εx’y’
yx’x’
yy’y’
yx’y’
εx’z’
εy’z’
3 coefficients of thermal expansion αxx, αyy, αxy referred to
local axes.
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
Isotropic, Kinematic (Ziegler) or Combined Hardening.
Ivanov yield criterion with Isotropic hardening.
von Mises
lamina failure law for composites
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-106
TCS8
ASAS (Non-Linear) User Manual
LOAD TYPES
Appendix A
Nodal Loads
Prescribed displacements
Pressure loads (+ve for +ve local Z’ direction)
Distributed load patterns ML1, ML2, ML3
Temperature loads
Face temperature loads (Face 1 is on the -ve local Z’ side)
Body forces
Centrifugal loads
Angular accelerations
Tank Loads
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-107
TCS8
ASAS (Non-Linear) User Manual
Appendix A
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses, strains and stress resultants are available at all integration points
referred to element local axes. For Ivanov (full section) models only stress and
strain resultants are available. In addition, the stress indicators are printed for
plastic points.
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
corner node.
INTEGRATION RULES
2x2 Gauss quadrature in plane and 3 point Newton-Cotes through thickness
(2x2x3) by default. Other rules by request, but only the through thickness
integration rule may be altered. See Appendix -G for positions of integration
points.
LOCAL AXES
Local X’, Y’, Z’ form a right
handed orthogonal system which,
in general, varies in orientation
from point to point within the
element. At any point P in the
element, X’ and Y’ lie in the
tangent plane at P. The tangent
plane is the plane containing the
vectors PR and PS which are
vectors tangent to the curvilinear ξ
and η directions respectively. X’
and Y’ are positioned in the
tangent plane such that the angle
between PR and X’ equals the
angle between PS and Y’.
SIGN CONVENTIONS
Direct forces/unit width Νx’x’, Νy’y’, Νx’y’
Bending moments/unit width Μx’x’, Μy’y’, Μx’y’
Shear forces/unit width Qx’z’, Qy’z’
REFERENCE
A. 2, A. 4, A. 5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
+ve as shown.
+ve as shown.
+ve as shown.
Page A-108
TCS9
Appendix A
ASAS (Non-Linear) User Manual
Generally Curved 9-Node Quadrilateral Thick Shell Element
with Varying Thickness and Transverse Shear,
Capable of Modelling Discontinuities in Curvature and Thickness
NUMBER OF NODES
9 (4 corner, 4 mid-side, 1 centre).
NODAL COORDINATES
x, y, z (may be omitted for mid-side nodes
on straight edges). Each mid-side node has
tolerance of side/10 about the true mid-side.
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ at each node.
GEOMETRIC PROPERTIES
ti Thickness at node i (i = 1,9),
t2 to t9 may be omitted for an element with uniform thickness t1.
Additional lay-up data is required for laminated material option.
See Section 5.2.5.3 for the LAMI command.
MATERIAL MODELS
ELASTIC
Nx’x’
Νy’y’
Νx’y’
Mx’x’
My’y’
Mx’y’
Qx’z’
Qy’z’
-
Isotropic
-
Orthotropic
Woven
-
Laminated
-
Anisotropic
Anisotropic matrix C (not C-1) defined in element
material axes. (See Appendix B.1.2)
Coefficients C1-C24 required. Note that they do not
contain the thickness.
=
C1t C2t C4t
.
C3t C5t
.
. C6t
.
.
.
.
.
.
.
.
.
.
.
.
.
.
.
C7t2
C8t2
C9t2
C10t3
.
.
.
.
C11t2
C12t2
C13t2
C14t3
C15t3
.
.
.
C16t2 0
0
C17t2 0
0
C18t2 0
0
3
C19t 0
0
C20t3 0
0
C21t3 0
0
. C22t C23t
.
. C24t
εx’x’
εy’y’
εx’y’
yx’x’
yy’y’
yx’y’
εx’z’
εy’z’
3 coefficients of thermal expansion αxx, αyy, αxy referred to
PLASTIC
-
CREEP
-
local axes.
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
Isotropic, Kinematic (Ziegler) or Combined Hardening.
Ivanov yield criterion with Isotropic hardening.
von Mises
FAIL
-
lamina failure law for composites
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-109
TCS9
Appendix A
ASAS (Non-Linear) User Manual
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal Loads
Prescribed displacements
Pressure loads (+ve for +ve local Z’ direction)
Distributed load patterns ML1, ML2, ML3
Temperature loads.
Face temperature loads (Face 1 is on the -ve local Z’ side)
Body forces
Centrifugal loads
Angular accelerations
Tank Loads
MASS MODELLING
Consistent mass (used by default)
Lumped mass
OUTPUT
Stresses, strains and stress resultants are available at all integration points
referred to element local axes. For Ivanov (full section) models only stress and
strain resultants are available. In addition, the stress indicators are printed for
plastic points.
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
corner node.
INTEGRATION RULES
2x2 Gauss quadrature in plane and 3 point Newton-Cotes through thickness
(2x2x3) by default. Other in-plane rules not recommended although 3x3 rule
may be adopted in special circumstances. Other through thickness rules by
request. See Appendix -G for positions of integration points.
LOCAL AXES
Local X’, Y’, Z’ form a right
handed orthogonal system which,
in general, varies in orientation
from point to point within the
element. At any point P in the
element, X’ and Y’ lie in the
tangent plane at P. The tangent
plane is the plane containing the
vectors PR and PS which are
vectors tangent to the curvilinear ξ
and η directions respectively. X’
and Y’ are positioned in the
tangent plane such that the angle
between PR and X’ equals the
angle between PS and Y’.
SIGN CONVENTIONS
Direct forces/unit width Νx’x’, Νy’y’, Νx’y’
Bending moments/unit width Μx’x’, Μy’y’, Μx’y’
+ve as shown.
+ve as shown.
Shear forces/unit width Qx’z’, Qy’z’
+ve as shown.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-110
TCS9
ASAS (Non-Linear) User Manual
REFERENCE
Appendix A
A. 2, A. 4, A. 5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-111
TMT3
Appendix A
ASAS (Non-Linear) User Manual
Triangular Membrane Field Element with Linear Variation
of Field Variable
NUMBER OF NODES
3
NODAL COORDINATES
x, y, (z)
z should be omitted for 2-D problems.
DEGREES OF FREEDOM
T at each node
GEOMETRIC PROPERTIES
ti Thickness at node i (i=i,3)
t2, t3 may be omitted for an element with
uniform thickness t1
No geometric property required with PLSN option. In this case, the geometric
property integer in the topology data should also be omitted.
MATERIAL MODELS
FIELD
PIER
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal values related to field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at integration points related to either global
or local axes (local by default).
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise.
INTEGRATION RULES
Single point rule by default (1x1). 3 point rule by request. Appendix -G gives
position of integration points.
Y'
LOCAL AXES
Local X’ lies along the straight line
from node 1 towards node 2. Local
σy'y'
Y’ is in the plane, perpendicular to
X’ and positive towards node 3.
Local Z’ forms a right-handed set
with local X’ and local Y’.
3
σx'y'
σx'x'
2
1
X'
SIGN CONVENTION
Fluxes and gradients are positive when in the positive axis direction
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-112
TMT3
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-113
TMT6
ASAS (Non-Linear) User Manual
Appendix A
Isoparametric Triangular Membrane Field Element with Quasi-quadratic
Variation of Field Variable
NUMBER OF NODES
6
NODAL COORDINATES
x, y, (z)
z should be omitted for 2-D problems.
Coordinates of mid-side nodes may be
omitted for straight edges but, if given,
each node must be within side/10 of the
true mid-side.
DEGREES OF FREEDOM
T at each node.
GEOMETRIC PROPERTIES
ti Thickness at node i (i=1,6)
t2, to t6 may be omitted for an element with
uniform thickness t1.
No geometric property required with PLSN option. In this case, the geometric
property integer in the topology data should also be omitted.
MATERIAL MODELS
FIELD
PIER
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal values related to field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at integration points related to either global
or local axes (local by default).
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
corner node.
INTEGRATION RULES
3 point rule by default (1x3). One point rule by request. See Appendix -G for
positions of integration points.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-114
TMT6
Appendix A
ASAS (Non-Linear) User Manual
LOCAL AXES
Local X’ lies on the element surface.
For flat elements it is a straight line
parallel to a line, through nodes 1
5
Y'
and 3. For elements curved out-ofplane, it is the intersection of the
element surface with the plane
containing the surface normal and
6
the straight line through nodes 1 and
3. Local Y’ is in the surface,
perpendicular to local X’ and +ve
4
σy'y'
σx'x'
X'
σx'y'
1
3
2
towards node 5. Local Z’ forms a
right-handed set with local X’ and
local Y’.
SIGN CONVENTION
Fluxes and gradients are positive when in the positive axis direction
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-115
TRM3
Appendix A
ASAS (Non-Linear) User Manual
Triangular Membrane Element with Constant Strain
This element can be used for both plane strain and plane stress applications in two and three dimensions.
REQUIRED OPTIONS
PLSN
- 2-D Classical Plane Strain (εz = 0.0)
EPSN
- 2-D Engineering Plane Strain (εz = const.)
TWOD - 2-D Plane Stress
none
- 3-D Plane Stress
NUMBER OF NODES
3
NODAL COORDINATES
x, y, (z)
z should be omitted for plane strain and
2-D plane stress forms.
DEGREES OF FREEDOM
X, Y, for Plane strain and 2-D Plane
stress forms (see note 2)
X, Y, Z for 3-D Plane stress. Deformations out-of-plane must be suppressed or
restrained by adjacent elements
GEOMETRIC PROPERTIES
MATERIAL MODELS
Plane strain
-
None (the geometric property integer with the element
topology data should also be omitted)
Plane stress
-
ti Thickness at node i (i=i,3)
t2, t3 may be omitted for an element with uniform
thickness t1
ELASTIC
-
Isotropic
Orthotropic
-
Woven
Anisotropic
Anisotropic matrix C (or C-1) defined in axis system
selected for output
σxx
σyy
σxy
σzz
=
C1 C2
.
C3
.
.
.
.
C4
C5
C6
.
C7
C8
C9
C10
εxx
εyy
εxy
εzz
4 coefficients of thermal expansion αxx, αyy, αxy, αzz,
referred to axis system selected for output
PLASTIC
-
Hyperelastic
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
Isotropic, Kinematic (Ziegler) or Combined Hardening.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-116
TRM3
Appendix A
ASAS (Non-Linear) User Manual
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements
Edge pressure loads (on any side, +ve towards the element centre)
Normal pressure load (+ve local z’ direction)
Distributed load patterns ML1, ML2, ML3
Temperature loads
Y'
Body forces
Centrifugal loads
3
σy'y'
Angular accelerations
Tank Loads
σx'y'
σx'x'
2
1
X'
MASS MODELLING
Consistent Mass (used by default)
Lumped Mass
OUTPUT
Stresses and strains are available at integration points referred to either global
or element local axes (local by default). Note global should not be used with
elements in the 3-D Plane stress form.
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise.
INTEGRATION RULES
Single point rule by default (1x1). 3 point rule by request. Appendix -G gives
position of integration points.
LOCAL AXES
Local X’ lies along the straight line
from node 1 towards node 2. Local
Y’ is in the plane, perpendicular to
X’ and positive towards node 3.
Local Z’ forms a right-handed set
with local X’ and local Y’.
SIGN CONVENTIONS
Direct stresses σxx, σyy, σzz
+ve for tension
Shear stress σxy
+ve as shown
NOTES
1.
With the EPSN option, one extra node, with number MAXND+1 (MAXND is the maximum node number
on the structure), is automatically added to the structure. This node has εZ as its only freedom, which is
reported in the displacement output. As this extra node is common to all elements, εZ is constant for the
entire structure.
2.
2-D elements with global stress output must be used if fracture mechanics processing in POSTNL is
required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-117
TRM3
ASAS (Non-Linear) User Manual
REFERENCE
Appendix A
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-118
TRM6
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Triangular Membrane Element
with Linear Strain Variation
This element can be used for both plane strain and plane stress applications in two and three dimensions.
REQUIRED OPTIONS
PLSN
- 2-D Classical Plane Strain (εz = 0.0)
EPSN
- 2-D Engineering Plane Strain (εz = const.)
TWOD - 2-D Plane Stress
none
NUMBER OF NODES
6
NODAL COORDINATES
x, y, (z)
- 3-D Plane Stress
z should be omitted for plane strain and 2-D
plane stress forms. Coordinates of mid-side
nodes may be omitted for straight edges but,
if given, each node must be within side/10 of
the true mid-side.
DEGREES OF FREEDOM
X, Y, for Plane strain and 2-D Plane
stress forms (see note 2)
X, Y, Z for 3-D Plane stress. Deformations out-of-plane must be suppressed or
restrained by adjacent elements
GEOMETRIC PROPERTIES
Plane strain
-
None (the geometric property integer with the element
topology data should also be omitted)
Plane stress
-
ti Thickness at node i (i=1,6)
t2, t3 may be omitted for an element with uniform
thickness t1
MATERIAL MODELS
ELASTIC
-
Isotropic
Orthotropic
Woven
-
Anisotropic
Anisotropic matrix C (or C-1) defined in axis system
selected for output
σxx
σyy
σxy
σzz
=
C1 C2
.
C3
.
.
.
.
C4
C5
C6
.
C7
C8
C9
C10
εxx
εyy
εxy
εzz
4 coefficients of thermal expansion αxx, αyy, αxy, αzz,
referred to axis system selected for output
-
Hyperelastic
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-119
TRM6
Appendix A
ASAS (Non-Linear) User Manual
PLASTIC
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
Isotropic, Kinematic (Ziegler) or Combined Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-120
TRM6
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal loads
Prescribed displacements
Edge pressure loads (on any side, +ve towards the element centre)
Normal pressure load (+ve for +ve local z’ direction)
Distributed load patterns ML1, ML2, ML3
Temperature loads
Body forces
Centrifugal loads
Angular accelerations
Tank Loads
MASS MODELLING
Consistent Mass (used by default)
Lumped Mass
OUTPUT
Stresses and strains are available at integration points referred to either global
or element local axes (local by default). Note global should not be used with
elements in the 3-D Plane stress form.
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise.
INTEGRATION RULES
3 point rule by default (1x3). One point rule by request. See Appendix -G for
positions of integration points.
LOCAL AXES
Local X’ lies on the element surface.
For flat elements it is a straight line
parallel to a line, through nodes 1
and 3. For elements curved out-ofplane, it is the intersection of the
element surface with the plane
containing the surface normal and
the straight line through nodes 1 and
3. Local Y’ is in the surface,
perpendicular to local X’ and +ve
towards node 5. Local Z’ forms a
right-handed set with local X’ and
local Y’.
SIGN CONVENTIONS
Direct stresses σxx, σyy, σzz
Shear stress σxy
+ve for tension
+ve as shown
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-121
TRM6
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
With the EPSN option, one extra node, with number MAXND+1 (MAXND is the maximum node number
on the structure), is automatically added to the structure. This node has εZ as its only freedom, which is
reported in the displacement output. As this extra node is common to all elements, εZ is constant for the
entire structure.
2.
2-D elements with global stress output must be used if fracture mechanics processing in POSTNL is
required.
REFERENCE
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-122
TRX3
Appendix A
ASAS (Non-Linear) User Manual
Axisymmetric Triangular Element with Straight Sides
Z
NUMBER OF NODES
3
NODAL COORDINATES
r, z
(Note that r and z occupy the first and
3
third fields on lines using an unnamed
cartesian system. The second field must
1
2
be input as zero.)
DEGREES OF FREEDOM
R, Z at each node
(Any skew system must be defined by the six direction cosines R’R, R’θ, R’Z,
Z’R, Z’θ, Z’Z. The values R’θ and Z’θ must be zero)
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
ELASTIC
-
Isotropic
Orthotropic
Woven
-
Anisotropic
Anisotropic matrix C (or C-1) defined in axis system
selected for output
σrr
σzz
σθθ
σrz
=
C1 C2
.
C3
.
.
.
.
C4
C5
C6
.
C7
C8
C9
C10
εrr
εzz
εθθ
εrz
4 coefficients of thermal expansion αrr, αzz, αθθ, αrz,
referred to axis system selected for output
PLASTIC
-
Hyperelastic
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
Isotropic, Kinematic (Prager or Ziegler) or Combined
Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-123
TRX3
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal loads (must be defined per radian)
Prescribed displacements
Pressure loads (on any side, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
MASS MODELLING
Consistent Mass (used by default)
Lumped Mass
OUTPUT
Stresses and strains are available at integration points either in global or local
element axes (global by default).
NODE NUMBERING
The nodes may be listed either clockwise or anti-clockwise.
INTEGRATION RULES
Single point rule used by default. Higher order rules by request. Appendix -G
gives position of integration points.
LOCAL AXES
Local R’ is a straight line from node 1 to node 2.
Local Z’ is perpendicular to local R’ in the RZ plane and lies counter
clockwise from R’.
SIGN CONVENTION
Direct stresses σrr, σzz, σθθ
Shear stress σrz
+ve for tension
+ve as shown
z
r
NOTE
Global stress output must be used if fracture mechanics processing in POSTNL
is required.
REFERENCE
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-124
TRX6
Appendix A
ASAS (Non-Linear) User Manual
Axisymmetric Isoparametric Triangular Element
NUMBER OF NODES
6
NODAL COORDINATES
r, z
(may be omitted for mid-side nodes on
Z
a straight edge). Each mid-side node
has a tolerance of side/10 about the true
5
4
6
mid-side. Note that r and z occupy the
3
1
first and third fields with coordinate
data using an unnamed cartesian
2
system.
DEGREES OF FREEDOM
R,Z at each node
(Any skew system must be 2-D. Of the six direction cosines R’R, R’θ, R’Z,
Z’R, Z’θ, Z’Z. The values R’θ and Z’θ must be zero)
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
ELASTIC
-
Isotropic
-
Orthotropic
Woven
-
Anisotropic
Anisotropic matrix C (or C-1) defined in axis system
selected for output
σrr
σzz
σθθ
σrz
=
C1 C2
.
C3
.
.
.
.
C4
C5
C6
.
C7
C8
C9
C10
εrr
εzz
εθθ
εrz
4 coefficients of thermal expansion αrr, αzz, αθθ, αrz,
referred to axis system selected for output
PLASTIC
-
Hyperelastic
-
von Mises, Tresca, Mohr-Coulomb, Drucker-Prager
yield criteria.
Isotropic, Kinematic (Prager or Ziegler) or Combined
Hardening.
CREEP
-
von Mises.
Material Properties may be temperature dependent if required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-125
TRX6
Appendix A
ASAS (Non-Linear) User Manual
LOAD TYPES
Nodal loads
Prescribed displacements
Pressure loads (on any side, +ve towards the element centre)
Temperature loads
Body forces
Centrifugal loads
MASS MODELLING
Consistent Mass (used by default)
Lumped Mass
OUTPUT
Stresses and strains are available at integration points either in global or local
element axes (global by default).
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
corner.
INTEGRATION RULES
3 point rule used by default (1x3). Single point rule by request.
Appendix-G gives positions of integration points.
LOCAL AXES
Invariant throughout the element. Local R’ is a straight line parallel to a line
through nodes 1 and 3. Local Z is perpendicular to local R’ in the global RZ
plane, and lies counter clockwise from R’.
SIGN CONVENTION
Direct stresses σrr, σzz, σθθ
Shear stress σrz
+ve for tension
+ve as shown
z
r
NOTE
Global stress output must be used if fracture mechanics processing in POSTNL
is required.
REFERENCE
A. 2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-126
TUBE
Appendix A
ASAS (Non-Linear) User Manual
Three-dimensional Beam Bending Element
with Uniform Circular Cross-section
NUMBER OF NODES
2
NODAL COORDINATES
x, y, z
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ at each node
GEOMETRIC PROPERTIES
D
External diameter (>0.0)
(uniform)
Wall thickness (D/2>t>0.0)
t
Local Axis definition -May be omitted. See Section 5.2.5.5 and Appendix
A.2.1.
OFFSETS
The OFFG, OFFS, OFSK, OFCO commands may be used to define rigid
offsets at each end. For further details see Appendix A.3 and Section 5.2.5.
MATERIAL MODEL
ELASTIC
-
Isotropic
PLASTIC
-
Stress resultant model based on generalised plastic hinge
theory. Note that hinges can only form at nodes.
See Appendix -B for details.
Material properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements
Temperature loads
Distributed load patterns
BL1, BL2, BL3, BL4, BL5, BL6, BL7, BL8
GL1, GL4, GL5, GL6, GL7
GP1, GP4, GP6, GP7
Body Forces
Centrifugal Loads
Angular Acceleration
Wave load
MASS MODELLING
Consistent Mass
Lumped Mass (used by default)
FORCE OUTPUT
The forces are exerted by the nodes on the element, and related to the local
axes. Note that for an offset beam the forces output are related to the element
centroidal axes.
INTEGRATION RULES
There are no integration points for the element, all the necessary element
matrices being formed explicitly.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-127
TUBE
Appendix A
ASAS (Non-Linear) User Manual
LOCAL AXES
A beam element has two local axes systems. The X’Y’Z’ local axes are
associated with end nodes of the element. The X”Y”Z” local axes are
associated with the end points of the centroidal axis of the element, taking
account of any non-zero rigid offsets.
If all offsets are zero, X’Y’Z’ and X”Y”Z” are coincident.
If local axis data is supplied, local X” lies along the centroidal axis from end 1
towards end 2. Local Y” lies in the plane defined by the two nodes (ends) and
a third point defined in the geometric properties list. Local Z” forms a right
handed set with local X” and localY”.
If local axis data is not supplied, local X” lies along the centroidal axis from
end 1 towards end 2. Local Z” must lie in the global XY plane with +ve local
Y” on the +ve side of the global XY plane. In the special case where local Y”
is also in the global XY plane, local Y” must lie in the global Y direction.
BM3D should be used for a beam with general orientation of local Z”.
See also Section 5.2.5 and Appendix A.2.1.
SIGN CONVENTIONS
Axial force
Shear force
positive for tension
positive for end 2 sagging relative to end 1
Torque
positive for clockwise rotation of end 2 relative to
end 1, looking from end 1 toward end 2
Bending moment
positive for sagging
Shear QY”
+ve
Shear QZ”
+ve
Moment Z”Z”
+ve
Moment Y”Y”
+ve
Y''
Z''
1
2
1
X''
DATA EXAMPLES
2
X''
ELEM
MATP 4
TUBE
4
1
17
END
GEOM
17 TUBE
20000.0
17.5
END
REFERENCE
A. 1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-128
TXT3
ASAS (Non-Linear) User Manual
Appendix A
Axisymmetric Triangular Field Element with Linear Variation
of Field Variable
NUMBER OF NODES
3
NODAL COORDINATES
r, z
(Note that r and z occupy the first and
third fields on lines using an unnamed
Z
3
cartesian system. The second field must
be input as zero.)
DEGREES OF FREEDOM
T at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
FIELD
1
2
PIER
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal values related to field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at integration points related to either global
or local axes (global by default).
NODE NUMBERING
The nodes may be listed either clockwise or anti-clockwise.
INTEGRATION RULES
Single point rule used by default. Higher order rules by request. Appendix -G
gives position of integration points.
LOCAL AXES
Local R’ is a straight line from node 1 to node 2.
Local Z’ is perpendicular to local R’ in the RZ plane and lies counter
clockwise from R’.
SIGN CONVENTION
Fluxes and gradients are positive when in the positive axis direction
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-129
ASAS (Non-Linear) User Manual
3.
Appendix A
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-130
TXT6
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Axisymmetric Triangular Field Element with Quasi-quadratic
Variation of Field Variable
Z
NUMBER OF NODES
6
NODAL COORDINATES
r, z
(may be omitted for mid-side nodes on
a straight edge). Each mid-side node
5
4
6
3
1
2
has a tolerance of side/10 about the true
mid-side. Note that r and z occupy the
first and third fields with coordinate
data using
system.
an
DEGREES OF FREEDOM
T at each node
GEOMETRIC PROPERTIES
None
MATERIAL MODELS
FIELD
unnamed
cartesian
PIER
Material Properties may be temperature dependent if required.
LOAD TYPES
Nodal values related to field variable type
Prescribed field variable
Temperature
Flux density - surface or internal
OUTPUT
Fluxes per unit area (analogous to stresses) and field variable gradients
(analogous to strains) are available at integration points related to either global
or local axes (global by default).
NODE NUMBERING
The nodes are listed in cyclic order, clockwise or anti-clockwise, starting at a
corner.
INTEGRATION RULES
3 point rule used by default (1x3). Single point rule by request.
Appendix-G gives positions of integration points.
LOCAL AXES
Invariant throughout the element. Local R’ is a straight line parallel to a line
through nodes 1 and 3. Local Z is perpendicular to local R’ in the global RZ
plane, and lies counter clockwise from R’.
SIGN CONVENTION
Fluxes and gradients are positive when in the positive axis direction.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-131
TXT6
ASAS (Non-Linear) User Manual
Appendix A
NOTES
1.
Temperature loading does not produce thermal loading and does not imply prescribed temperature but
simply allows temperature dependent material properties to be specified. This is not required for heat
conduction analysis.
2.
The element allows linear analysis only except for heat conduction analysis.
3.
Field elements allow a variety of field problems to be analysed eg. heat conduction, fluid seepage and
electrical conduction.
See Reference A. 4, Chapter 7 for full details
REFERENCE
A. 2, A. 4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-132
WST4
Appendix A
ASAS (Non-Linear) User Manual
Isoparametric Beam/Stiffener Element having Thin-walled
Open Cross-sections of Arbitrary Shape (allowing warping)
NUMBER OF NODES
4 (2 end, 1 mid-length and 1 auxiliary node).
NODAL COORDINATES
X, Y, Z (may be omitted for mid-length
node on a straight element). The mid-
2
4
3
length node has tolerance of length/10
about the true mid-length. The auxiliary
node is only used to define the local axes
s
(see below).
1
DEGREES OF FREEDOM
X, Y, Z, RX, RY, RZ, WRR.
GEOMETRIC PROPERTIES
The element can model any open thin-walled cross-section made up of straight
r
sided segments, connected at median points.
t
The element has special
geometric properties (see Geometric Property Section 5.2.5.1).
Repeat this
for each
segment
ISEC
-
Median point number to be used as warping origin
RMUL
-
Rigidity multiplier (= 1.0 - to represent full
cross-section, or = 0.5 to represent half symmetric
cross-
section).
s,t
-
Local coordinates to define median points in plane of cross-
section.
IA,IB
-
Local connectivity.
NSTAT
-
Number of integration stations along the segment.
NLAY
T
-
Number of integration layers through segment thickness.
Segment thickness.
The cross-section of the element is assumed constant along the length
(Geometric Properties at nodes 2 and 3 need not be supplied).
MATERIAL MODEL
ELASTIC
-
Isotropic
PLASTIC
-
von-Mises Isotropic Hardening.
Material properties may be temperature dependent if required.
LOAD TYPES
Nodal loads
Prescribed displacements.
Body forces
Centrifugal loads
Angular accelerations
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-133
WST4
Appendix A
ASAS (Non-Linear) User Manual
MASS MODELLING
OUTPUT
Consistent mass (used by default)
Lumped mass
Direct stress σrr, shear stress σrm, (referred to segment axes) and stress
resultants (in element local axes) are available as follows.
STRS:
stresses at all integration points on element
SSTR:
smoothed stresses for all integration points at 2 cross-sections
corresponding to 2 point Gauss rule on length.
ESTR:
smoothed stresses for top and bottom layers at end of each
segment (ie extreme fibrepoints) at 2 cross-sections
corresponding to 2 point Gauss rule on length.
SRES:
stress resultants at all 4 Gauss points along the length
SSRE:
smoothed stress resultants at 2 cross-sections corresponding
to 2 point Gauss rule on length
Strains and strain resultants are not available
For elastic analysis, only stress resultants (i.e. SRES or SSRE) are available.
INTEGRATION RULES
4 Point Gauss Quadrature along length (invariant and independent of stress
output). User defined trapezoidal rule for each segment. (NO DEFAULT) see Geometric Properties Data. As a guide the following are suggested:
Elastic - 2 stations, 1 layer
Plastic - 5 stations, 4 layers
NODE NUMBERING
Node 3 is always the MID-LENGTH node and 4 the auxiliary node.
LOCAL AXES r, s, t
Independent of cross-sectional shape - ie s, t do not have to coincide with
principal axes of the cross-section. Local r is tangential to the curvilinear
nodal axis, positive in the direction node 1 to node 2. s is normal to the plane
containing the r-axis and node 4. t is orthogonal to r and s and points away
from node 4, ie positive t and the auxiliary node are on opposite sides of the r
axis.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-134
WST4
Appendix A
ASAS (Non-Linear) User Manual
SIGN CONVENTIONS
Axial force
Axial stress
+ve tension
+ve tension
Generalised stress resultants, +ve as shown
Fr
Qrs
-
axial force
shear along s
Qrt
Ms
-
shear along t
moment about s
Mt Mw -
moment about t
warping moment
Tsv
St. Venant torque
-
Tw Twag -
warping torque
Wagner torque
T
T
Tsv + Tw + Twag
total torque
=
-
Mt
Qrt
Ms
t
Qrs
s
Mw
r
Fr
Tsv
NOTES
1.
This element requires special Geometry Property and Residual stress input data (see Sections 5.2.5.1 and
5.6.3).
2.
Note that the element topology definition and local axes are not the same as the STF4 beam stiffener.
3.
Segment number 1 must start at free edge of the beam cross-section. Each subsequent segment must start
from the end of any previously numbered segment.
4.
Stress and stress resultant outputs always correspond to the full cross-section.
REFERENCE
A. 5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-135
ASAS (Non-Linear) User Manual
A.4
Appendix A
References
A. 1
Przemieniecki, J.S., Theory of Matrix Structural Analysis, McGraw-Hill, 1968.
A. 2
Zienkiwicz, O.C and Taylor, R.L., The Finite Element Method, 4th Edn., Volumes 1 and 2, McGraw-Hill,
1989.
A. 3
Kebari, H., A one point integrated assumed strain 4-node Mindlin plate element. Eng. Comp. 1990, Vol. 7,
December, pp 284-290.
A. 4
Bathe, K-J., Finite Element Procedures in Engineering Analysis, Prentice-Hall, 1982.
A. 5
Bates, D.N., The Mechanics of Thin Walled Structures with Special Reference to Finite Rotations. PhD
Thesis, University of London, 1987.
A. 6
Rice, J.R., The Line-Spring Model for Surface Flaws, in the Surface Crack: Physical Problems and
Computational Solutions, ed. J.L. Swedlow, ASME, 1972.
A. 7
Parks, D.M., and White, C.S., Elastic-Plastic Line-Spring Finite Elements for Surface-Cracked Plates and
Shells, Trans ASME, Journal of Pressure Vessel Technology, Vol. 104, 1982, pp287-292.
A. 8
Laursen, T.A. and Simo, J.C., On the Formulation and Numerical Treatment of Finite Deformation
Frictional Contact Problems, in Non-linear Computational Mechanics - State of the Art, ed. Wriggers, P.
and Wagner, W., Springer-Verlag, 1991, pp716-736.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-136
ASAS (Non-Linear) User Manual
Appendix A
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page A-137
ASAS (Non-Linear) User Manual
Appendix - B
B.1
Appendix B
Material Models
Linear Elasticity
B.1.1 Isotropic Material
An isotropic, linear elastic material is characterised by two independent elastic constants, namely the Young’s
modulus and the Poisson’s ratio. As the material properties are invariant under coordinate transformation, the
choice of material reference axis system becomes irrelevant. Explicit forms of the elastic material matrix for an
isotropic material can be found in Ref B.1.
B.1.2 Anisotropic Material
For a completely anisotropic material, 21 independent elastic constants are necessary to define the 3-dimensional
stress-strain relationship. For finite element types other than 3-D solids, the number of constants required will
be different. The exact forms of the anisotropic material matrix for individual elements are given in Appendix A.
Unlike isotropic material, the coefficients of the material matrix for anisotropic materials are strongly dependent
on the choice of material reference axis system. The specification of material coefficients that are consistent
with the definition of material axis system are important to ensure the correct modelling of the material
behaviour.
By default, the material axis system coincides with the stress output axis system defined in Appendix -A. The
only exception is for shell elements where the default material Xm–axis is defined as the projection of global Xaxis onto the shell surface with Ym lying on the tangent plane of the shell and orthogonal Xm. The user can
override this default by specifying a material skew integer in the material properties data. In this case, the
material constants should be provided with respect to the skew system.
For bricks, plane stress/strain
membranes and axisymmetric solids, the skew axis system should be defined relative to the output axis system,
ie the direction cosines are those between the skew axes and the output axes. For shells, however, a different
definition of the skew system is adopted. The skew system is defined relative to the global axis system instead,
and Xm will become the projection of the skew X-axis onto the shell surface. Since the procedure for defining
the default material axis system will fail when the shell surface is normal to the global X, a skewed material
system must be specified in this situation.
B.1.3 Orthotropic Material
Orthotropic material is a special form of the general anisotropic material. It is completely defined by the
Young’s modulii, shear modulii and Poisson’s ratio in 3 principal material directions. From the 9 principal
elastic constants specified, the program will internally convert them into the equivalent anisotropic material
matrix format as described in Appendix -A. Because of the different numbers of stress components for each
element type, the conversion process is element dependent. As an example, the anisotropic matrix for a shell
element is given by:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-1
Appendix B
ASAS (Non-Linear) User Manual
where
and
C11 =
E11
1 -ν 12ν 21
,
C12 =
ν 12 E 22
1 -ν 12ν 21
,
C22 =
E 22
1 -ν 12ν 21
ν 12 E 22 = ν 21 E11
The default material axis system is defined in the same way as for anisotropic materials. Again, the user can
specify a material skew system to provide more general orientation of the material. Refer to B.1.2 for definitions
of the material axis system with and without skewing.
B.1.4 Laminated Material for Shell Elements
Laminated material is available to model shell structures constructed by assembling several layers of materials
with different properties such as fibre reinforced composites. Detailed discussion of laminated material and
composite analysis can be found in Ref B.2.
Based on the layup configuration specified, the equivalent anisotropic material properties for the laminate are
then obtained by integrating the properties for each individual layer through the thickness. This computation is
automatically carried out in PRENL and the results stored. The terms in the processed material matrix for a
composite laminate are defined as follows:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-2
ASAS (Non-Linear) User Manual
where
Q =
Appendix B
3x3 in-plane material stiffness matrix calculated for each lamina in the laminate reference
axis system
S
=
2x2 transverse shear material stiffness matrix in the laminate reference system
t
=
thickness of the laminate
z
=
axis of the laminate reference system normal to the plane of the laminate
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-3
Appendix B
ASAS (Non-Linear) User Manual
The laminate reference axes are defined such that the 0° fibre direction is parallel to the material Xm–axis and the
90° fibre direction is parallel to the material Ym–axis. By default, the material Xm–axis is defined as the
projection of global X-axis onto the shell surface with Ym lying on the tangent plane of the shell and orthogonal
to Xm. When skew system is specified, Xm will become the projection of the skew Xonto the shell surface.
Since the procedure for defining the default material axis system will fail when the shell surface is normal to the
global X, a skewed material system must be specified in this situation.
Unlike isotropic material where a single transverse shear correction factor of 5/6 can be applied throughout, the
shear correction factors for a laminated shell depend on both the layup sequence and the material properties of
each constitutive layer. Herein, the procedure outlined in Ref B.3 for orthotropic laminate has been adopted for
determining the shear correction factors.
The transverse shear constitutive relations for orthotropic laminates take the form
2
k1 T11
Qxz
0
εxz
2
εyz
=
0
Qyz
where
2
2
k1 , k 2 =
From Ref 0,
k 2 T 22
shear correction factors
T11
=
C22t
T22
=
C24t
2
k1 is evaluated from
-1
t


i
k = T11 ∫ -2t g1 (z) dz 
2
i
2




1
Q
i
where
g1 (z) = i G1i + 11 (2 B11 - A11 z)
2 Dx

S11 
2
1
and
i
=
i
G1 =
for all layers in the laminate
constants determined from interface continuity conditions and the requirement that
shear stresses σxz’s vanish on the bottom surface of the plate.
Dx = (D11A11-B112)
with
Similarly,
A11=C1t ,
B11=C7t2
and
D11=C10t3
2
k 2 can be determined with all suffix 1 replaced by 2.
B.1.5 Woven Material
The woven material considered is of 2-dimensional plain weave structure only. Thus, the fabric is assumed to be
composed of two sets of interlacing, mutually orthogonal yarns of the same material. The equivalent anisotropic
material properties of a woven layer are determined from the yarn properties (orthotropic) using the parallel
mosaic model (Ref B.8). The key simplification of the mosaic model is the omission of the fibre undulation and
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-4
Appendix B
ASAS (Non-Linear) User Manual
continuity that exist in the actual fabric. Effectively, a woven layer is treated as an assemblage of cross-ply
unidirectional laminae. The equivalent properties obtained can in general be written as:
D = ν0C0 + ν90C90
where ν
=
the volume fraction
C
=
the material stiffness of the unidirectional sub-lamina
subscripts 0 and 90
=
the yarn orientation
The definitions of the material axis system with and without skewing are identical to those for anisotropic
material. Refer to B.1.2 for details.
B.2
Non-Linear Elasticity
B.2.1 Hyperelastic Material
Hyperelastic material is used to model rubber-like materials which have high elastic deformability and near
incompressible behaviour. The material behaviour is characterised by a single scalar strain energy density
function in terms of the strain components. In ASAS-NL, a modified form of the classical Mooney-Rivlin
model has been implemented. The strain energy density, U, for this model can be written as:
U = C10 (J1 - 3) + C01 (J 2 - 3) + f(J3)
where C10, C01
=
J1 , J2, J3
Mooney-Rivlin material constants
=
1
1 3 3
J1 = I I
a set of modified invariants defined by
2
2 3 3
, J2 = I I
1
∧ J 3 = I3 2
I1 , I2 and I3 are, respectively, the first, second and third invariants of the left Cauchy-Green stretch tensor, b=F·Ft
, and F is the deformation gradient. These invariants are given by:
I1 =
Tr (b)
I2 =
1 2
[I1 - Tr(b . b)]
2
I3 =
Det (b)
The first two terms on the r.h.s. of the expression for U correspond to the deviatoric part of the strain energy
density while f(J3) corresponds to the volumetric part which allows the near incompressible behaviour to be
modelled. The function f(J3) is given by:
f(J3) =
where K
=
[
1
K (J3 - 1 )2 + ln(J3 )2
2
]
the bulk modulus
Stresses and material stiffnesses are obtained by differentiating U with respect to strains, ie
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-5
Appendix B
ASAS (Non-Linear) User Manual
σ=
B.3
δU
δU
, D=
δε
δεδε
Plasticity
B.3.1 Yield Criteria
The yield criterion in a hypothesis which defines the limit of elasticity under any combination of stresses. The
following yield criteria are available.
B.3.1.1 Von Mises
Yield occurs when the elastic distortional energy reaches a critical value (Ref B.4), ie in terms of the equivalent
stress when
σ = σy where σy is the uniaxial yield stress in tension
The equivalent stress, reported in the output, is calculated as
σ = 3 J2
where J2, the second invariant of the deviatoric stress, is given as
(
1
(σ xx - σ yy )2 + (σ yy - σ zz )2 + (σ zz - σ xx )2 + 6 σ 2xy + 6 σ 2yz + 6 σ 2zx
6
J2 =
)
B.3.1.2 Tresca
Yield occurs when the maximum shear stress reaches a critical value (Ref 0), ie in terms of principal stresses σ1,
σ2, σ3, with
σ1 > σ2 > σ3 then
σ =σ1-σ3=σy
where σy
=
the uniaxial yield stress in tension and σ the equivalent stress reported in the output
B.3.1.3 Ivanov
This (approximate) principle is based on the instantaneous plastification of the shell section (rather than
examining individual layers as for the other criteria) (Ref B.5). The stress resultants (direct forces and moments)
of the mid-plane are used directly in the yield criterion in conjunction with the flow rule. The criterion, which
does not include the effect of transverse shear stress resultants, has the form
(
)
2
1
 1 Qt Qm - Qtm
1
f = Q t + Qm +  Q2m + Q2tm  =1
2
 4 (Qt + 0.48 Qm )
4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-6
Appendix B
ASAS (Non-Linear) User Manual
where Qt, Qm, Qtm
Qt =
=
N
N
2
0
; Qm =
functions of the stress resultants as follows:
M
M
2
0
; Qtm =
MN
M0 N0
where
N = N 2x + N 2y - N x N y + 3 N 2xy
M = M 2x + M 2y - M x M y + 3 M 2xy
1
1
MN = M x N x + M y N y - M x N y - M y N x + 3 M xy N xy
2
2
N0 = σ 0 t = uniaxial yield force / unit width
M0 =
σ 0 t2
σ0 =
4
= uniaxial yield moment / unit width
yield stress in tension
t = thickness of shell section
The modified Ivanov criterion is simply the Ivanov criterion with M0 replaced by αM0, thus giving a better
approximation for the uniaxial moment/plastic curvature relationship with increasing equivalent plastic
curvature. The multiplier α is defined as:
α = 1.0 - 0.4 e-2.6
( χ ps )
where χps is the non-dimensional plastic curvature. This is obtained by summing the incremental equivalent
plastic curvatures;
2
2
∆ χ 2pxy 
 Et 
 Et  4 
2
2
2

∆ χ ps = 
 ∆ χ ps = 
 • ∆ χ px + ∆ χ py + ∆ χ px ∆ χ py +


3
3
3
4
 σo
 σo


2
In which E is the Youngs Modulus and ∆χpx, ∆χpy, ∆χpxy are the incremental plastic curvatures.
In the program the yield function f is converted to an equivalent stress σ reported by the program as
σ =σ0f
(where σ0 is the initial yield stress as before)
B.3.1.4 Mohr-Coulomb
This criterion is based on a generalisation of Coulomb’s failure theory for soils, and may be viewed as resulting
from the addition of a dependence on the mean stress into the Tresca yield criterion. Failure occurs when (Ref
B.4)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-7
ASAS (Non-Linear) User Manual
Appendix B
(σ 1 - σ 3) = 2 c cos φ - (σ 1 + σ 3) sin φ
where σ1, σ3 =
c
φ
maximum and minimum principal stresses
=
the cohesion
=
angle of friction
In this case the equivalent stress reported by the program is:
σ = (σ 1 - σ 3) + (σ 1 + σ 3) sin φ
B.3.1.5 Drucker-Prager
The Drucker-Prager yield criterion is a generalisation of the von Mises yield criterion into which a dependence
on mean stress has been added. Failure occurs at an equivalent stress given by (Ref B.4)
σ = α I1 + J 2 = k
where I1
=
σ1 + σ2 + σ3 (the 1st stress invariant)
where J2
=
2nd invariant of the deviatoric stress defined in Section B.1.1
where c, φ
α =
2 sin φ
3 (3 - sin φ )
k =
6 c cos φ
3 (3 - sin φ )
=
the cohesion and angle of friction respectively as before
B.3.1.6 Stress Resultant Plasticity for Beams
The stress resultant plasticity models BEM2, BEM3 and BEAM are only available with engineering beam
elements BM2D, BM3D and TUBE. The theory assumes that the whole beam cross-section will plastify
instantaneously when a combination of the stress resultants at the point of interest reaches a critical value. It is
also assumed that the material behaviour is elastic-perfectly plastic and that all plastic deformation of an element
is concentrated at the nodes, while the inside of the element remains elastic. When plasticity develops, a plastic
interaction relationship between various stress resultant components is strictly satisfied and the plastic
displacement associated with each stress resultant component is defined according to the flow rule. Further
details about the so-called “plastic node method” can be found in Ref B.6.
Three types of yield surfaces are available in ASAS-NL and these are defined as follows:
(i)
BEM2
2
 P   Mz 
 =1
  + 

 Po   M pz 
2
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-8
Appendix B
ASAS (Non-Linear) User Manual
(ii)
BEM3
2
2
 P   Mz   M y 
 +
 =1
  + 
 

 Po   M pz   M py 
2
(iii)
BEAM
C2
 Mz 


P
 + C5  M y  = 1
C1   + C3 

M 
 Po 
 M pz 
 py 
C4
where P0
=
yield force
C6
Mpz
=
yield moment about beam local z-axis
Mpy
=
yield moment about beam local y-axis
C1 to C6
=
yield function constants
B.3.1.7 Coulomb Friction
The Coulomb friction model is available for use with rigid surface elements (and implicitly with gap elements).
Slip occurs when
f = || σ t || - σ l = 0
and
σ l = min ( µ σ n , τ o )
where σt
=
tangential stress
σn
=
normal stress
µ
=
coefficient of friction
τo
=
shear stress limit
B.3.1.8 Tension Cut-off
The tension cutmodel assumes that failure occurs when the principal stress reaches a critical value, i.e.
si=σy (i=1,3)
where
σy is the uniaxial tensile strength
This material is suitable for modelling cracking in plain or reinforced concrete.
B.3.1.9 Inelastic Spring
The figure below shows a typical skeleton curve that is used to represent the inelastic spring model. The spring
initially deforms in a linear elastic manner until the initial yield force fy1 is reached. Plastic yielding will start to
develop when further loading is applied. If the loading is reduced or its direction reversed, the spring will
unload elastically.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-9
ASAS (Non-Linear) User Manual
Appendix B
The unloading/reloading stiffness after yielding occurred may be different from the initial elastic stiffness. This
is controlled by the material parameter α1. By default, the unloading stiffness is assumed to be the same as the
initial stiffness (i.e. α1 is set to 1.0 if it is specified.
The hysteretic behaviour is modelled through shifting of the spring curve origin. Origin shift takes place when
unloading continues beyond a limit point (point P above). When this happens, P will become the new origin of
the spring curve. The materials parameter α2 defines the location of point P and it allows for the modelling of
different kinematic hardening behaviour. By default, α2 = 0.0 and thus the shifted origin is always along the
displacement axis.
The setting α2 = 1.0 is almost equivalent to the pure kinematic hardening model in
continuum elements. Normally, α2 should be set between 0.0 and 1.0.
B.3.2 Hardening Rules
Hardening Rules define how the yield criterion is modified by plastic deformation. Various hardening rules are
available by giving suitable directives with the material property commands in the structural description data.
The rules are given below.
B.3.2.1 Isotropic
The yield surface expands uniformly about the origin and a uniaxial model would yield at the same value in both
tension and compression. No Bauschinger effect is reproduced.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-10
ASAS (Non-Linear) User Manual
Appendix B
B.3.2.2 Kinematic
The yield locus translates as a rigid body when plastic deformation occurs. The Bauschinger effect is modelled.
Two types of kinematic hardening are available. Prager hardening assumes that the yield locus translates as a
rigid body in the direction of the normal to its surface at the point concerned, ie
dα = c dεp
where c
=
dα =
dεp =
a constant
the instantaneous change in the position of the locus
the instantaneous plastic strain
Ziegler hardening assumes that the yield locus translates in the direction of the load vector, ie
dα = e(σ-α)
where e
=
a constant
σ
=
the current stress state
α
=
the current centre of yield (ie back stress)
Prager hardening cannot be used in reduced stress spaces, ie for plane stress, plates, shells and beams. For these
elements Ziegler hardening must be used.
B.3.2.3 Combined
Both types of kinematic hardening may be combined with isotropic hardening. The ratio of kinematic to
isotropic hardening is chosen by specifying a parameter h to have a value between zero and one (h=0 gives
kinematic and h=1 gives isotropic hardening). h is given with the material property data.
The various hardening rules are displayed in Figure B.3.1.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-11
Appendix B
ASAS (Non-Linear) User Manual
Figure B.3.1 Hardening Rules
B.3.3 Equivalent Strain
The equivalent (or effective) strain reported by the program is defined as:
ε=
4
I2
3
where I2, the second invariant of the strains vector is defined as
1 2
1 2 1 2 1 2
2
2
I2 =  ε ′xx + ε ′yy + ε ′zz + ε xy + ε yz + ε zx 
2
2
2
2 
=
B.4
1
3
3
3 
(ε xx - ε yy )2 + (ε yy - ε zz )2 + (ε zz - ε xx )2 + ε 2xy + ε 2yz + ε 2zx 

6
2
2
2 
CREEP
All time dependent material behaviour is represented in the program by the description ‘Creep’ and the analysis
of this is explained fully in Appendix -J.
Currently the creep model is limited to the von Mises potential function and associative flow rule when
extending the uniaxial creep description to multiple axes. No yield limit is used in the uniaxial creep description
(ie the yield stress is effectively zero) and so the combination of creep and conventional time independent
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-12
Appendix B
ASAS (Non-Linear) User Manual
plasticity is not possible in any one load step. There are a number of creep laws in-built to the program.
Alternatively, a creep law can be defined directly in a user supplied subroutine. Any uniaxial description which
is a function of stress, equivalent strain, time, temperature and any user-supplied constants may be defined using
the user creep subroutine.
B.4.1 In-Built Creep Laws
(i)
NORT
εc = c1σ C t C
2
3
This is a Norton law in which
σ
=
equivalent stress
t
=
time
εc
=
equivalent creep strain rate
supplied by program
and constants C1, C2, C3 are supplied by the user with the creep material properties data. Additional
versatility is possible by allowing C1-C3 to be temperature-dependent. In this case the constants for each
specified temperature are listed.
(ii)
LAW2
(-C /T)
+ C5 σ C t C exp(-C /T)
εc = C1σ C t C exp
2
3
4
6
8
7
This law thus has both primary and secondary creep components with time hardening.
Note that the temperature T is absolute Kelvin, ie that defined by any current temperature loading plus
273°. Therefore if this temperature dependence is used (ie non-zero C4 or C8) the temperature loading
should be defined in °C.
(iii)
LAW3
(-C /T)
+ C5 σ C exp(-C /T)
εc = C1σ C ε Cc exp
2
3
4
6
7
This is a strain hardening formulation with the accumulated equivalent creep strain εc participating in the
definition of the primary creep rate.
Note that the temperature T is as defined for LAW2.
(iv)
LAW4
This is a Blackburn law, implementing the creep data for 316 stainless steel for temperature ranges
between 450°C and 700°C according to the reference “Isochronous stress-strain curves for austenitic
stainless steel” Blackburn Trans ASME (1972).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-13
Appendix B
ASAS (Non-Linear) User Manual
Note that the units for LAW4 are N, mm, °C and secs.
B.4.2 User Supplied Creep Laws
A user defined creep law is associated with a particular material type via the appropriate 4 character directive
USE1, USE2, USE3, USE4 and USE5. Up to five user define laws can be added to the program. Users should
specify their creep law in the form of a FORTRAN subroutine which can then be compiled and linked into the
program. This subroutine must be named as indicated below and should be written in double precision.
4 character directive with
CREEP properties data
Subroutine name
USE1
CRPUS1
USE2
CRPUS2
USE3
CRPUS3
USE4
CRPUS4
USE5
CRPUS5
The subroutine should define the uniaxial (equivalent) creep strain rate with an argument list and format as
follows.
SUBROUTINE CRPUS1 (STRESS, SIGEQ, TEMP, DTIME, TOTIME, CRPTOT,
1
CRATE, PRICRP, MOUT, IELMAT, EQSTRN, NST,
2
DCRATE, CR)
LOGICAL PRICRP
DOUBLE PRECISION
STRESS(NST), CRPTOT(NST), TEMP, DTIME,
TOTIME, CRATE, EQSTRN, SIGEQ, DCRATE, CR (9)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-14
ASAS (Non-Linear) User Manual
Appendix B
User supplied code defining an expression for uniaxial (equivalent) creep strain rate
CRATE and, if OPTIon VISC is to be used, an expression for DCRATE (see
definition below)
IF(.NOT.PRICRP) GO TO 9999
CALL PRINT (1)
WRITE (MOUT, 2000)
2000
9999
FORMAT (19H ** CREEP USER LAW 1)
CONTINUE
RETURN
END
The variables in the argument list are defined as follows
Input:
STRESS
-
Stress Vector
SIGEQ
-
Equivalent Stress (von Mises)
TEMP
-
Temperature
DTIME
-
Time increment
TOTIME
-
Total creep time
CRPTOT
-
Total creep strain vector
PRICRP
-
A flag having a value TRUE on the first pass through the user subroutine and a value
FALSE on all subsequent passes
MOUT
-
Variable defining the output device number. All WRITE statements in the user supplied
code should take the form WRITE(MOUT, format label)
IELMAT
-
Material Property Integer
EQSTRN
-
Equivalent creep strain (total)
NST
-
Dimension of stress and creep strain vectors STRES and CRPTOT
CR
-
Vector of creep law constants C1 to C9, if supplied.
CRATE
-
Uniaxial (equivalent) creep strain rate
DCRATE
-
Derivative of CRATE with respect to SIGEQ. Only required if OPTIon VISC is to be used.
Output:
The value of NST and the nature of the stresses and strains contained in vectors STRESS and CRPTOT depend
on the type of element according to the following table:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-15
Appendix B
ASAS (Non-Linear) User Manual
Locations in Vector
Element Type
NST
1
2
3
4
5
6
Uniaxial
1
XX
-
-
-
-
-
Plane Stress / Plane Strain
4
XX
YY
XY
ZZ
-
-
Axisymmetric
4
RR
ZZ
HH
RZ
-
-
3D Solids
6
XX
YY
ZZ
XY
YZ
ZX
Thick Beams (STF4)
3
XX
XY(XT)*
XZ(-)*
Shells
5
XX
YY
XY
XZ
YZ
* For tube or box section beams
B.5
Composite Failure
Failure of a composite laminate can be analysed by specifying failure criteria in the failure material properties
data. Depending on the nature of an analysis, the data supplied may have the following different definitions:
(i)
When FAIL data are specified for a constitutive layer within a laminate and the element is elastic, these
will define the lamina strength and strain limits.
(ii)
When FAIL data are specified after the LAMInated material properties data, they will define the failure
limits of the whole laminate.
(iii)
When FAIL data are specified for a constitutive layer within a laminate and the element is plastic, these
will define the failure limits of the lamina and any failure law constants required to model the post-failure
behaviour.
B.5.1 Lamina Failure Criteria
Lamina failure criteria are applied to individual layers within a laminate. A number of lamina failure criteria for
elastic laminated composite elements are evaluated in POSTNL when options FEMV→LAMI are selected.
These are reported in the form of failure indices, F. The surface F=1 defines the failure envelope and encloses
the stress states that the material can sustain without failure. In other words,
F≥ 1
failed
F<1
safe
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-16
ASAS (Non-Linear) User Manual
Appendix B
The lamina failure indices are computed from the stresses or strains in each layer together with the specified
unidirectional strength properties. For laminated brick elements, the layer stresses and strains are directly
computed in ASASNL. For shell elements, however, these are obtained through a stress recovery process in
POSTNL. Also, in this case, a plane stress condition has been assumed in the failure criteria, and therefore only
3 in-plane stress components (σ1, σ2 and σ12) are relevant. Note that the stresses are given in the principal
directions 1, 2 and 3, ie in the fibre direction and directions perpendicular to fibre.
Let
and
and
Xt, ε1t
be the tensile stress and strain limits, respectively, in the 1-direction
Xc, ε1c
be the compressive stress and strain limits, respectively, in the 1-direction
Yt, ε2t
be the tensile stress and strain limits, respectively, in the 2-direction
Yc, ε2c
be the compressive stress and strain limits, respectively, in the 2-direction
Zt, ε3t
be the tensile stress and strain limits, respectively, in the 3-direction
Zc, ε3c
be the compressive stress and strain limits, respectively, in the 3-direction
S12, γ12
be the shear stress and strain limits, respectively, in the 12-plane
S23, γ23
be the shear stress and strain limits, respectively, in the 23-plane
S31, γ31
be the shear stress and strain limits, respectively, in the 31-plane
Zl
be the interlaminar tensile stress limit
Sl
be the interlaminar shear stress limit
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-17
Appendix B
ASAS (Non-Linear) User Manual
The various lamina failure criteria evaluated in POSTNL are defined as follows:
(i)
Azzi-Tsai
2
2
2
1 1
1 1 
 1
σ  σ  σ   1
F =  1  +  2  +  3  -  2 + 2 - 2  σ 1σ 2 -  2 + 2 - 2  σ 2 σ 3
 X   Y   Z  X Y Z 
Y Z X 
2
2
1 1 
σ  σ  σ 
 1
-  2 + 2 - 2  σ 1σ 3 +  12  +  23  +  31 
Z X Y 
 S12   S23   S31 
where
(ii)
2
X=Xt
,
σ1≥0
Y=Yt
,
σ2≥0
Z=Zt
,
σ3≥0
X=Xc
,
σ1<0
Y=Yc
,
σ2<0
Z=Zc
,
σ3<0
Norris
 σ 1   σ 2  σ 1σ 2  σ 12 
+

F1 =   +   +
XY  S12 
X Y
2
2
2
 σ 2   σ 3  σ 2 σ 3  σ 23 
+

F2 =   +   +
YZ  S23 
Y Z
2
2
 σ 1   σ 3  σ 1σ 3  σ 31 
+

F3 =   +   +
XZ  S31 
X  Z
2
2
2
2
F = MAX {F1, F2, F3}
where
(iii)
X=Xt
,
σ1≥0
Y=Yt
,
σ2≥0
Z=Zt
,
σ3≥0
X=Xc
,
σ1<0
Y=Yc
,
σ2<0
Z=Zc
,
σ3<0
Hoffman
F=
1 1
1
1 
1 1
1
1 
2
2
+
+
(σ 2 - σ 3 )
 (σ 1 - σ 2 ) + 

2  X t Xc Y t Yc Zt Zc 
2  Y t Yc Zt Zc X t Xc 
1 1
1
1 
1 
1 1
 1 1 
2  1
+ 
+
 (σ 3 - σ 1) +  -  σ 1 +  -  σ 2 +  -  σ 3
2  Zt Zc X t Xc Y t Yc 
 Zt Zc 
 Y t Yc 
 X t Xc 
2
2
σ  σ  σ 
+  12  +  23  +  31 
 S12   S23   S31 
(iv)
2
Tsai-Wu
F=
σ 12 + σ 22 + σ 32 +  1 - 1  +  1 - 1  +  1 - 1 
σ 3
σ 2 
σ 1 

X t Xc
Y t Yc
Zt Zc  X t Xc 
 Y t Yc 
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
 Zt Zc 
Page B-18
Appendix B
ASAS (Non-Linear) User Manual
2
2
2
σ  σ  σ 
+  12  +  23  +  31  + 2 F12 σ 1σ 2 + 2 F23 σ 2 σ 3 + 2 F13 σ 1σ 3
 S12   S23   S31 
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-19
Appendix B
ASAS (Non-Linear) User Manual
F12, F23, and F13 are experimentally determined coefficients and it is necessary that they satisfy the
stability condition
 1  1  2
 1  1  2
 1  1  2
 - F13 > 0

 - F23 > 0, 

 - F12 > 0, 


 X t Xc  Zt Zc 
 Y t Yc  Zt Zc 
 X t Xc  Y t Yc 
At present, F12, F23, and F13 are always set to zero and this has been shown to give good results.
(v)
Von-Mises
1
F=
X t Xc
(σ
2
1
2
2
)
+ σ 22 + σ 32 - σ 1σ 2 - σ 2 σ 3 - σ 1σ 3 + 3σ 12
+ 3σ 223 + σ 31
This criterion has assumed that Xt=Xc=X, where X is the uniaxial failure stress of an isotropic material.
All other strength properties are related to X and therefore the input values will be ignored. Because of
the special assumptions, this criterion is only applicable in certain situations.
(vi)
Maximum Stress
 σ 1 2  σ 2 2  σ 3 2  σ 12 2  σ 23 2  σ 31 2 
 , 
 
F = MAX   ,   ,   , 
 , 
 X   Y   Z   S12   S23   S31  
where
(vii)
X=Xt
,
σ1≥0
Y=Yt
,
σ2≥0
Z=Zt
,
σ3≥0
X=Xc
,
σ1<0
Y=Yc
,
σ2<0
Z=Zc
,
σ3<0
Delamination
2
σ3 
F1 =   for σ 3 > 0
 Zl 
= 0 for σ 3 <= 0
F2 =
(σ
2
23
2
)
+ σ 31
2
Sl
F = MAX {F1, F2}
Delamination is only checked at the interface between adjacent layers.
B.5.2 Laminate Failure Criteria
Unlike lamina failure criteria, the laminate failure criteria are applied directly to the entire laminate, which is
considered homogeneous but anisotropic. Thus, the global stresses and strains (or resultants) for the laminate
and their strength characterisation are required to evaluate the failure indices. A total of five failure indices are
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-20
Appendix B
ASAS (Non-Linear) User Manual
reported when POSTNL options FEMV→GFAI are selected labelled GFAIL01 to GLFAIL05. Of these five
indices, only the first is in-built and the remaining four are user defined.
Let
and
εˆ xx
εˆ yy
εˆ xy
ψˆ xx
ψˆ yy
ψˆ xy
εˆ xz
εˆ yz
be the direct strain limit in the laminate x direction (i.e. in the 0° direction)
be the direct strain limit in the laminate y direction (i.e. in the 90° direction)
be the shear strain limit in the laminate xy plane
be the bending curvature limit in the laminate x direction
be the bending curvature limit in the laminate y direction
be the torsional curvature limit in the laminate xy plane
be the shear strain limit in the laminate xz plane
be the shear strain limit in the laminate yz plane
The global laminate failure criterion evaluated in POSTNL is defined as follows:
4.
Maximum strain resultant criterion
F1 =
| ε yy |
| ε xy |
| ε xx |
; F2 =
; F3 =
| εˆ xx |
| εˆ yy |
| εˆ xy |
F4 =
| ψ yy |
| ψ xy |
| ψ xx |
; F5 =
; F6 =
| ψˆ xx |
| ψˆ yy |
| ψˆ xy |
F7 =
| ε yz |
| ε xz |
; F8 =
| εˆ xz |
| εˆ yz |
F = MAX{Fi} i = 1,8
In addition, users may specify their laminate failure criterion in the form of a FORTRAN function which can
then be compiled and linked into the program POSTNL. This function must be named as indicated below.
Laminate Failure Type
Laminate failure criterion 1 (in-built)
Name
-
Laminate failure criterion 2 (User)
GLFC02
Laminate failure criterion 3 (User)
GLFC03
Laminate failure criterion 4 (User)
GLFC04
Laminate failure criterion 5 (User)
GLFC05
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-21
ASAS (Non-Linear) User Manual
Appendix B
The function should evaluate the failure index with an argument list and format as follows:
DOUBLE PRECISION FUNCTION GLFC02 (SRES,ERES,NSRES,FAIL,NFAIL)
DOUBLE PRECISION STRES(NSRES), ERES(NSRES),FAIL(NFAIL)
C****
C**** USER CODE
C****
.
.
.
GLFC02=...
RETURN
END
The variables in the argument list are defined as follows:
Input:
SRES
-
Stress resultants in laminate reference axis system
ERES
-
Strain resultants in laminate reference axis system
NSRES
-
Number of stress/strain resultants
FAIL
-
Failure properties
NFAIL
-
Number of failure properties (=14)
-
Failure index for laminate failure criterion 2
Output:
GLFC02
B.5.3 Failure Laws
Failure laws are used to study the behaviour of composite laminate beyond the point of first ply failure. It is
assumed that the material behaves linearly up to failure. The failure surface and the post-failure degradation in
material properties are then defined by the failure law. It should be noted that the failure model currently
assumes a plane stress hypothesis, ie the transverse shear components must always remain elastic with no
degradation in material stiffness. A total of five failure laws (FLW1, FLW2, FLW3, FLW4 and FLW5) are
available in the program, of which laws FLW1 and FLW2 are pre-defined and the other three are user defined.
B.5.3.1 In-Built Failure Law
FLW1
This law checks material failure via a combination of maximum stress criterion in the fibre direction and a
choice of criteria from Tsai-Wu, Azzi-Tsai, Hoffman, Norris, von-Mises or maximum stress.
From the
governing failure criterion, the mode of failure, ie fibre or matrix failure, can be determined. The maximum
stress criterion in fibre direction can clearly be identified as an indicator of fibre cracking whereas the other
criterion selected predicts the layer strength for stress states with relatively large transverse stress components
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-22
Appendix B
ASAS (Non-Linear) User Manual
and therefore can be treated as matrix failure. The post-failure material stiffness will depend on the mode of
failure and its form for fibre and matrix failure are given as follows:
In the above, subscripts 1 and 2 denote fibre and transverse direction, respectively.
β 2 is a material parameter
defining the reduction in fibre stiffness after fibre failure. If not specified, 1- β 2 =E22/E11 which means that only
matrix stiffness remains after fibre failure. Delamination is checked using the formula stated in Appendix B.5.1.
When this failure is detected, it is assumed that the lamina will lose all its stiffness.
β is a material parameter
defining the reduction in fibre stiffness after matrix failure. Full details of the theory are given in Ref B.7.
FLW2
For this law, failure is deemed to occur when the selected failure function is exceeded. The six available failure
criteria are Tsai-Wu, Azzi-Tsai, Hoffman, Norris, von-Mises and maximum stress. This failure law has distinct
failure modes that correspond to failures in each of the principal material direction (i.e. 11,22,33,12,23,31 for 3D). When failure occurs, the dominant failure mode is determined from the stress component that has the largest
contribution towards failure.
The post-failure stiffness degradation factors for all six possible failure modes are tabulated below. These
factors have been made very general so that the law may be applied to laminae with different material
definitions.
Mode
Reduction Factors for Diagonal Terms on Material Stiffness
11
22
33
12
23
31
11
β1
β2
β2
β3
1.0
β3
22
β4
β1
β8
β5
β5
1.0
33
β4
β8
β1
1.0
β5
β5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-23
Appendix B
ASAS (Non-Linear) User Manual
12
β6
β7
1.0
β1
1.0
1.0
23
1.0
β7
β7
1.0
β1
1.0
31
β6
1.0
β7
1.0
1.0
β1
The defaults for all the βs are zero and, if specified, they must lie within the range 0.0≤ β ≤ 1.0. When more
than one failure modes is active, the reduction factor taken for a term will be the smallest among all the active
failure modes. Off-diagonal terms in the stiffness are assumed to have reduction factors of min {β i, βj}, where βi
and βj are the reduction factors for the associated diagonal terms.
Delamination is checked using the formula stated in Appendix B.5.1. When this failure is detected, it is assumed
that all the failure modes in the above table will be active.
B.5.3.2 User-Defined Failure Laws
For user-defined failure laws FLW3, FLW4, and FLW5, users should specify a set of two FORTRAN
subroutines for each of their own failure laws. One of these routines is for the formation of the material stiffness
matrix, both tangent and secant, while the other is for the evaluation of the failure index. The user routines must
be named as indicated below:
(i)
Failure law type
Material stiffness routine name
Failure index routine name
FLW3
DFAIL3
SFAIL3
FLW4
DFAIL4
SFAIL4
FLW5
DFAIL5
SFAIL5
Material Stiffness Routine
This routine should form the material stiffness matrix as a function of stress and/or strain states. Both secant and
tangent stiffnesses are required and the appropriate matrix should be set according the the value of input
argument IOPT. The following argument list and format should be adhered to.
SUBROUTINE DFAIL5 (DEP
1
ISF
DIMENSION
,DE
,STRS
,NDIM ,NSTV
,STRN
,FAIL
,NFAIL
,IOPT)
,
ISF(6)
DOUBLE PRECISION STRS(NSTV),DE(NDIM,NDIM),DEP(NDIM,NDIM),
1
STRN(NSTV),FAIL(NFAIL)
CALL SENTRY (4HDFAI,2HL5)
C
C****
C
USER CODE
.
.
.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-24
ASAS (Non-Linear) User Manual
Appendix B
CALL SEXIT
RETURN
END
The variables in the argument list are defined as follows:
Input:
DE
-
Elastic material matrix in fibre axis system (ie along fibre and normal to fibre)
STRS
-
Stress vector in fibre axis system
STRN
-
Strain vector in fibre axis system
FAIL
-
Failure properties
ISF
-
Failure indicator for each stress component (0 - not failed, 1 - failed)
ISF(1)
-
Component 11
ISF(2)
-
Component 22
ISF(3)
-
Component 33
ISF(4)
-
Component 12
ISF(5)
-
Component 23
ISF(6)
-
Component 31
NDIM
-
Dimension of material matrix (=5 for shells)
NSTV
-
Size of stress vector (=6 for shells, the last position being the ‘equivalent’ quantity)
NFAIL
-
Number of failure properties (=14)
IOPT
-
Option code for material matrix type (1 - tangent, 2 - secant)
-
Failed material matrix in fibre axis system, tangent or secant according to IOPT
Output:
DEP
(ii)
Failure Index Routine
This routine should evaluate the failure index and also report the cause of failure. The user routine should have
the following argument list:
SUBROUTINE SFAIL5 (F,IFAIL,ISFLG,STRS,STRN,FAIL,NSTV,NFAIL)
DIMENSION ISFLG(6)
DOUBLE PRECISION STRS(NSTV),STRN(NSTV),FAIL(NFAIL),F
CALL SENTRY(4HSFAI,2HL5)
C
C****
USER CODE
C
.
.
.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-25
ASAS (Non-Linear) User Manual
Appendix B
CALL SEXIT
RETURN
END
The variables in the argument list are defined as follows:
Input:
IFAIL
-
Failure status at end of last iteration (0 - elastic, 4 - fibre failure, 5 - matrix failure, 6 lamina failure, 7 - transverse shear/normal stress failure, 8 - modes 5 and 7)
STRS
-
Stress vector
STRN
-
Strain vector
FAIL
-
Failure properties
NSTV
-
Size of stress vector
NFAIL
-
Number of failure properties
F
-
Value of failure index (F=1 defines the failure surface)
ISFLG
-
Failure indicator for each stress component (0 - not failed, 1 - failed)
Output:
B.6
ISFLG(1) -
Component 11
ISFLG(2) -
Component 22
ISFLG(3) -
Component 33
ISFLG(4) -
Component 12
ISFLG(5) -
Component 23
ISFLG(6) -
Component 31
User Material
The user material interface enables users to define their own constitutive behaviour for a material. A set of two
FORTRAN subroutines are required, of which one is for the formation of material stiffness matrix and the other
is for the computation of stresses. The user is cautioned that this is an advanced capability and it generally
requires considerable expertise to develop a realistic material model. The user must also ensure that the
numerical scheme implemented is stable so as to avoid numerical instability.
(i)
User Material Stiffness Routine
This user routine should have the following argument list and format:
1
2
3
SUBROUTINE USERDM (DMAT ,ELSTR ,ESTRN ,PSTRN ,STRSB ,
STATEV,EDAT
,TEMP
,DTEMP ,TIME ,
DTIME ,ISP
,NSTAT ,NED
,NSTV ,
NST
,IELTNO ,IMATNO ,LNCNO ,ITER )
INTEGER ISP,NSTAT ,NED , NSTV ,NST ,IELTNO ,IMATNO ,LNCNO ,ITER
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-26
ASAS (Non-Linear) User Manual
Appendix B
DOUBLE PRECISION
1
2
DMAT(NST,NST),ELSTR(NSTV),ESTRN(NSTV),
PSTRN(NSTV),STRSB(NSTV),STATEV(NSTAT),
EDAT(NED),TEMP,DTEMP,TIME,DTIME
CALL SENTRY(4HUSER,2HDM)
C
C****
C
USER CODE
.
.
.
CALL SEXIT
RETURN
END
Input variables:
ELSTR
-
Stress vector
ESTRN
-
Elastic strain vector
PSTRN
-
Plastic strain vector
STRSB
-
Back stress vector
STATEV
-
State variables
EDAT
-
Elastic material properties
TEMP
-
Current temperature
DTEMP
-
Temperature increment
TIME
-
Current time
DTIME
-
Time increment
ISP
-
Stress point indicator
(0 - elastic, 1 - elastic unloading, 2 - plastic)
NSTAT
-
Number of state variables (=3)
NED
-
Number of elastic material properties (=24)
NSTV
-
Dimension of stress vector
NST
-
Number of stress components for element (=NSTV-1)
IELTNO
-
User element number
IMATNO
-
User material property integer
LNCNO
-
Load increment number
ITER
-
Iteration number
Output variables:
DMAT
(ii)
-
Material stiffness matrix
User Stress Computation Routine
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-27
Appendix B
ASAS (Non-Linear) User Manual
This user routine should have the following argument list and format:
SUBROUTINE USERST (ELSTR
,STSDEL ,ELSTN
,ESTRN
1
STRNI
,STNDEL ,STRSB
,STATEV ,EDAT
,
2
3
WORK
ISP
,TEMP
,NSTAT
,TIME
,NSTV
,
)
4
,DTEMP
,NED
,PSTRN
,DTIME
,NST
IELTNO ,IMATNO ,LNCNO ,ITER
)
INTEGER ISP,NSTAT,NED ,NSTV ,NST ,IELTNO ,IMATNO ,LNCNO,ITER
DOUBLE PRECISION
1
ELSTR(NSTV),ELSTN(NSTV),STSDEL(NSTV),
STNDEL(NSTV),STRNI(NSTV),ESTRN(NSTV),
2
PSTRN(NSTV),STRSB(NSTV),STATEV(NSTAT),
3
,
EDAT(NED),TEMP,DTEMP,TIME,DTIME,WORK
CALL SENTRY(4HUSER,2HST)
C
C****
USER CODE
C
.
.
.
CALL SEXIT
RETURN
END
Input variables:
STRNI
-
Total strain increment vector
STNDEL
-
Mechanical strain increment vector
EDAT
-
Elastic material properties
TEMP
-
Current temperature
DTEMP
-
Temperature increment
TIME
-
Current time
DTIME
-
Time increment
NSTAT
-
Number of state variables
NED
-
Number of elastic material properties
NSTV
-
Dimension of stress vector
NST
-
Number of stress components for element (=NSTV-1)
IELTNO
-
User element number
IMATNO
-
User material property integer
LNCNO
-
Load increment number
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-28
ASAS (Non-Linear) User Manual
ITER
-
Appendix B
Iteration number
Output variables:
STSDEL
-
Stress increment vector
Updated variables:
ELSTR
-
Current stress vector
ELSTN
-
Current strain vector
ESTRN
-
Elastic strain vector
PSTRN
-
Plastic strain vector
STRSB
-
Current back stress vector
STATEV
-
State variables
WORK
-
Incremental work
ISP
-
Stress point indicator
(0 - elastic, 1 - elastic unloading, 2 - plastic)
Notes
1.
User material interface cannot be used for creep or field analysis.
2.
User material interface cannot be applied to laminated shells.
3.
All variables are defined in the stress output axis system as specified in Appendix -A for individual
element types.
4.
For shell analysis, the first two user material properties specified must correspond to the Young’s
modulus and Poisson’s ratio of the material.
5.
In transient analysis, the stiffness damping factor for a user material must be set to zero.
6.
The updated variables in S/R USERST will be passed in as the values at the beginning of the current
increment and all incremental variables will be the incremental changes during the increment.
7.
Only the following element types are allowed to have user material. The number of stress components
(NST) and their orders are given in the following table:
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-29
Appendix B
ASAS (Non-Linear) User Manual
Element type
NST
Location in vector
1
2
3
4
5
6
Uniaxial
1
XX
-
-
-
-
-
Plane Stress
3
XX
YY
XY
-
-
-
Plane Strain
4
XX
YY
XY
ZZ
-
-
Axisymmetric
4
RR
ZZ
HH
RZ
-
-
3-D solids
6
XX
YY
ZZ
XY
YZ
ZX
Thick beams, STF4
3
XX
XY(XT)*
XZ(-)*
-
-
-
Shells
5
XX
YY
XY
XZ
YZ
Springs
1
XX
* for tube or box sections, XT is the tangential shear stress component
8.
The last location (ie NSTVth position) in the stress and strain vectors should only be used to store the
equivalent values. For spring elements, NST=NSTV=1 and thus the location for equivalent values in not
available.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-30
ASAS (Non-Linear) User Manual
Appendix B
B.7
References
B.1
Zienkiewicz, O.C. and Taylor, R.L., ‘The Finite Element Method, Vol. 1’, McGraw Hill, 1989 (4th
Edition).
B.2
Jones, R.M., ‘Mechanics of Composite Materials’, McGraw-Hill, 1975.
B.3
Whitney, J.M., ‘Shear Correction Factors for Orthotropic Laminate Under Static Load’, Tran. ASME,
J. Appl. Mech., 1973, pp303-304.
B.4
Hinton, E. and Owen, D.R.J., ‘Finite Elements in Plasticity’, Pineridge Press, 1981.
B.5
Crisfield, M.A., ‘Ivanov’s Yield Criterion for Thin Plates and Shells Using the Finite Element
Method’. TRRL Rep. 919, D.O.E., 1979.
B.6
Ueda, Y., and Yao, T., ‘The Plastic Node Method: A New Method of Plastic Analysis’, Comp. Meth.
Appl. Mech. Eng., Vol. 34, 1982, pp1089-1104.
B.7
Dorninger, K. and Rammerstorfer, F.G., ‘A Layered Composite Shell Element for Elastic and
Thermoelastic Stress and Stability Analysis at Large Deformations’, International Journal for
Numerical Methods in Engineering, Vol. 30, 1990, pp833-858.
B.8
Chou, T.W. and Ishikawa, T., ‘Analysis and Modelling of Two-Dimensional Fabric Composites’,
Ch.7 of Textile Structural Composites, Composite Materials Series, Vol, 3, Eds. Chou and Ko,
Elsevier, 1989, pp209-277.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page B-31
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix B
Page B-32
ASAS (Non-Linear) User Manual
Appendix - C
C.1
Appendix C
Solution Strategies in ASAS-NL
Introduction
The fundamental problem of structural analysis is to solve the equilibrium equations. In the finite element
idealization these equations are presented in the matrix form.
K* Q = P
(C.1.1)
and relate the vector of external loads P to the displacement vector Q utilising the structural stiffness matrix K.
For non-linear problems the equation (C.1.1) no longer holds, since K is a function of stress and deformation
states. However if a piecewise linearisation of the equilibrium equation (C.1.1) is applied as follows
K* dQ = dP
(C.1.2)
where dQ and dP are increments in the displacement and force vectors, the solution of the problem may be
obtained in a sequence of steps.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-1
Appendix C
ASAS (Non-Linear) User Manual
data preparation
load generation
stiffness generation
solution of incremental
equilibrium equations
calculation of displacements
calculation of updated geometry
strains and stress computation
unbalanced load calculation
Figure C.1.1 Main Program Flow Chart
The explicit form of the equation (C.1.2) depends on the type of non-linearity and formulation adopted. In
ASAS-NL this applies to non-linear material relations and large displacements. The latter are treated using the
Updated Lagrangian formulation, which implies that all state variables are referred to the current configuration
of the deformed structure. A flow chart illustrating corresponding algorithm of calculations is shown in Figure
C.1.1.
From the methodological point of view the strategy employed in ASAS-NL to calculate the solution of (C.1.2) is
a combined incremental - iterative approach.
This part of solution process may be considered as global
calculation and numerous versions of the solution strategy will be discussed in Section C.2.
During the global calculations there is another set of non-linear equations which is to be solved locally, that is in
a number of specified points within an element. This local set of equations relates stresses and strains as follows
dS = D* dE
(C.1.3)
where dS represents stress vector increment, dE is strain vector increment and D is the material stiffness matrix
(modulus matrix). The solution of (C.1.3), which is often referred to as “stress recovery” has twofold objective.
The first is to provide a state of stress corresponding to certain load level and the second to contribute to
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-2
ASAS (Non-Linear) User Manual
Appendix C
calculation of unbalanced load which is represented by dP vector during the iteration process. The solution
methods specific to the stress recovery will be discussed in Section C.3.
C.2
Incremental - Iterative Procedures
C.2.1 Introduction
The solution to the non-linear problem provided by ASASNL is obtained using incremental solution procedures
with a possibility of iterative correction within each increment. Two main types of procedures are incorporated
into the program. The first ones (code named SOLV) are the classical Newton-Raphson incremental - iterative
procedures, which provide the solution (displacements) corresponding exactly to the originally specified load.
Using the second type of procedures (code named SOLU) load level as well as displacements are adjusted
according to the response of the structure. Those procedures are often referred to as ‘structural response’ or
‘variable load’ methods. However despite the differences both types of procedures can be described using the
same general formulation, and in order to avoid unnecessary repetitions this method of presentation is adopted
here.
Numerical execution of the solution process within each increment is performed in two stages. During the first
stage a type of increment and its size is selected and incremental prediction
dQi,1 (subscript ‘i’ denotes
increment number) is obtained from the equations
K* d Qi,1 = d Pi,1
(C.2.1)
dQi,1 = a i * d Qi,1
dPi,1 = a i * d Pi,1
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-3
Appendix C
ASAS (Non-Linear) User Manual
constraint surface
dP
load - deflection curve
(true equilibrium path)
dPi,1
dP i,2
dP 2
solution points
dQi,1 dQi,2
dQ
Figure C.2.1 Constraint Surface of Solution Process
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-4
Appendix C
ASAS (Non-Linear) User Manual
where K is the stiffness matrix,
d Pi,1 is an increment of the load vector of arbitrary size and a i is a scalar
multiplier used to obtain requested increment size. During the second stage an iteration procedure is applied,
which is aimed at the improvement of initial incremental prediction. To describe in a general but precise manner
the procedures employed by ASAS-NL a concept of constraint surface is introduced. The characteristic feature
of this surface is that it contains points representing a sequence of solutions obtained during subsequent
iterations, Figure C.2.1. Exact definition of this surface will be given later. The operations performed at this
stage include choice of the type of constraint surface, application of an iteration technique of specified type and
then calculation of an iterative correction
dQ j (subscript ‘j’ denotes iteration number) from the equation.
K* d Q j = dP j
where
dP j is the residual force vector.
(C.2.2)
Next the current incremental values
dQi, j and dPi, j of the
displacement and load vectors respectively are calculated using the following formulae
dQi, j = dQi, j - 1 + b j * dQi,1 + dQ j
(C.2.3)
dPi, j = dPi, j - 1 + b j * dPi,1
where bj is a multiplier determined according to the adopted constraint as discussed later. A flow chart showing
the idea of the described above incremental - iterative method is shown in Figure C.2.2.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-5
Appendix C
ASAS (Non-Linear) User Manual
START
First stage
unscaled incremental prediction
(type of increment)
d Qi ,1
scaling multiplier
(size of increment)
ai
d Pi,1
d Qi,1
scaled incremental vectors
Second Stage
dP j
unbalanced load
(path dependent or path
independent approach)
dQ j
iterative correction
(type of iteration method)
bi
constraint multiplier
(type of constraint surface)
d Pi, j
d Qi, j
N
conv?
corrected incremental vectors
convergence check
Y
FINISH
Figure C.2.2 Flow Chart of Incremental/Iterative Solution Process
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-6
Appendix C
ASAS (Non-Linear) User Manual
C.2.2 Basic Definitions
The selection of increment type and the definition of constraint surface is based on the scalar function fi,j which
is defined in two alternative forms:
as a linear function
f i, j = G i * dQi, j + Hi * dPi, j
(C.2.4)
or as a quadratic function
f i, j =
((dQi, j )T * G i * dQi, j + (dPi, j )T * Hi * dPi, j + (dQi, j )T * Li * dPi, j)
(C.2.5)
where Gi, Hi, Li are diagonal matrices which in general may vary between increments. Prescribing the value of
the scalar fi,j at the beginning of the increment and then keeping its value constant during the iteration process
provides two additional equations, which are used to calculate the multipliers a i and
bj .
The constraint surface can now be defined as a subspace in the load/displacement space which is characterized
by a constant value of fij within the i-th increment. The position of this surface is determined by the size of the ith increment. In mathematical terms these two conditions are expressed as follows
f i,1 = dli
where
(C.2.6)
dli is the required length of incremental vector, and
f i, j - f i, j−1 = 0
(C.2.7)
Taking into account (C.2.3) and (C.2.4) or (C.2.5) the above constraint becomes
G i*(dQi, j-1+ b j*dQi,1+dQ j)+ Hi*(dPi, j-1+ b j*dPi,1)
- G i * dQi, j−1 - Hi * dPi, j−1 = 0
(C.2.8)
or
(dQi, j−1 + b j * dQi,1 + dQ j )T * G i * (dQi, j−1 + bi * dQi,1 + dQ j)
+ (dPi, j−1 + bh * dPi,1 )T * Hi * (dPi, j−1 + b j * dPi,1)
+ (dQi, j−1 + b j * dQi,1 + dQ j )T * Li * (dPi, j−1 + b j * dPi,1)
- (dQi, j−1 )T * G i * dQi, j−1 - (dPi, j−1 )T * Hi * dPi, j−1
- (dQi, j−1 )T * Li * dPi, j−1 = 0
(C.2.9)
respectively for linear or quadratic formulation.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-7
ASAS (Non-Linear) User Manual
Appendix C
The following values of matrices Gi, Hi and Li are available in ASASNL
(a)
G = [0], H = [I], L = [0]
(C.2.10)
where [I] is the identity matrix
(b)
G = [I], H = [0], L = [0]
(c)
G(n,n) = 0 for n = m, G(m,m) = 1
(C.2.11)
where ‘n’ is from 1,N. ‘N’ is the total number of displacements and ‘m’ is the number of a
specified displacement
H = [0], L = [0]
(d)
(C.2.12)
G(n,n) = K(n,n), H(n,n) = 1/K(n,n) for ‘n’ from 1,N
L = [0]
(e)
(C.2.13)
G = [0], H = [0], L = [I]
(C.2.14)
In the following sections it will be shown how the choice of matrices Gi, Hi and Li determines the character of
numerical procedure.
C.2.3 Incrementation procedures
As mentioned before, during the first stage a prescribed value of dli is adopted which together with one of the
above options gives the required type and size of the increment. This is realised as follows in ASAS-NL.
(a)
Load vector increment (proportional), obtained using (C.2.4), (C.2.6), and (C.2.10), which gives
a i = dli /(I* d Pi ,1 )
Requested by
(C.2.15)
SOLV or SOLU LOAD
with the values of dli (for i = 1,2...) are either specified using a list of pseudo-times or automatically
generated.
For the automatic procedure, the pseudo-time step size is given by
∆ t i = f ∆ t i-1
where f = FINCMX if the solution has converged in less than ITERD iterations in KSIGNL consecutive
steps and f = 1.0 otherwise. The default value of FINCMX is 1.5.
(b)
Specified displacement increment, obtained using (C.2.4), (C.2.6), and (C.2.12), which gives
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-8
Appendix C
ASAS (Non-Linear) User Manual
a i = dli /d Q(m )i,1
Requested by
(C.2.16)
SOLU CONSIT
with the initial value of dli (for i = 1) specified using INCDIS and then (for i 1) controlled by ITERD
via
1/ 2
 ITERD 

dli = dli-1 
 ITER 
and ITER is the number of iterations for convergence in the (i-1)th step.
(c)
Displacement vector increment, obtained using (C.2.5), (C.2.6), and (C.2.11), which gives
a i = dli /
Requested by
((d Qi ,1 )T * d Qi ,1 )
(C.2.17)
SOLU ARCL
with the initial value of dli (for i = 1) specified using INITPR or INCDIS and then (for i 1) controlled
by ITERD as in (b).
C.2.4 Iteration procedures
C.2.4.1 Type of constraint surface
The general definition of the constraint surface has the form of either equation (C.2.8) or (C.2.9). This combined
with one of the options for the matrices Gi, Hi and Li provides a wide selection of the constraint surfaces.
Substituting the current displacement and load vectors into the surface equation during the second stage gives the
formula which is a basis for the determination of the multiplier
b j used in (C.2.3). This in detail is presented
below together with ASAS-NL realization.
(a)
Plane of constant load, defined by the equation
bj = 0
(C.2.18)
obtained from (C.2.8) and (C.2.10).
Requested by
(b)
SOLV or
SOLU LOAD
Plane of constant displacement, defined by the equation
dQ(m ) j + b j * dQ(m )i ,1 = 0
(C.2.19)
obtained from (C.2.8) and (C.2.12).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-9
ASAS (Non-Linear) User Manual
Requested by
or by
Appendix C
SOLU CONSIT
SOLU CONSIT AUTO
In the later case displacement number ‘m’ is automatically selected from the condition
dQ(m )i ,1 = max (d Q(n )i ,1 )
(c)
(C.2.20)
Cylindrical surface of constant length of incremental displacement vector, defined by the equation
a 1* b2j + a 2 * b j + a 3 = 0
(C.2.21)
a 1 = (dQi ,1 )T * dQi ,1
(C.2.22)
where
a 2 = 2 * (dQi ,1 )T * (dQi , j-1 + dQ j)
a 3 = (dQ j )T * (2 * dQi , j-1 + dQ j)
obtained from (C.2.8) and (C.2.11).
Requested by SOLU ARCL
(d)
Piecewise plane envelope of the above, defined by the equation
(dQ j )T * dQi , j-1 + b j * (dQi ,1 )T * dQi , j-1 = 0
(C.2.23)
Obtained from truncated combination of (C.2.8) and (C.2.11). Serving as back-up for the previous case.
Requested by SOLU TARCL
(e)
Piecewise plane envelope of ellipsoidal surface of constant length of combined weighted incremental/load
vector, defined by the equation
(dQ j )T * G i * dQi , j-1 + b j * (dQi ,1 )T * G i * dQi , j-1 = 0
(C.2.24)
obtained from truncated combination of (C.2.9) and (C.2.13).
Serving as back-up for the case (c) when scaled convergence is used (see Section C.4).
(f)
Surface of constant work, defined by the equation
a 1* b2j + a 2 * b j + a 3 = 0
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
(C.2.25)
Page C-10
ASAS (Non-Linear) User Manual
Appendix C
where
a 1 = (dQi ,1 )T * dPi ,1
(C.2.26)
a 2 = (dQi , j-1 dQ j )T * dPi ,1 + (dQi ,1 )T * dPi , j-1
a 3 = dQT j * dPi , j-1
obtained from (C.2.8) and (C.2.14).
Requested by
(g)
SOLU ARCL WORKC
Piecewise plane envelope of the above, defined by the equation
(dQ j )T * dPi ,1 + b j * (dQi ,1 )T * dPi ,1 = 0
(C.2.27)
obtained from linearised combination of (C.2.9) and (C.2.14).
Requested by
SOLU CONSIT WORKC
C.2.4.2 Iteration techniques
The following iteration techniques are available in ASASNL
(a)
Standard Newton-Raphson, Figure C.2.3
This involves formation and reduction of the stiffness matrix K and solution of the equilibrium equation
on each iteration. In this case equations (C.2.1)1 and (C.2.2) are as follows
K i ,1 * d Qi ,1 = d Pi ,1
(C.2.28)
Ki, j * d Q j = d P j
It is requested by
UPDA STIF ITER ALL
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-11
Appendix C
ASAS (Non-Linear) User Manual
constraint surface
dP
load - deflection curve
dPi,1
dP i,2
dQi,1
dQi,2
dQ
Figure C.2.3 Standard Newton-Raphson
(b)
Modified Newton-Raphson, Figure C.2.4
It involves updating and reduction of the stiffness matrix K only once during an increment. The solution
of the equilibrium equation, calculated at each iteration is obtained using the most recently formulated
stiffness matrix.
The equations (C.2.1)1 and (C.2.2) are now
K i ,1 * d Qi ,1 = d Pi ,1
(4.12)
K i ,1 * d Q j = d P j
It is requested by
or
UPDA STIF INCR ALL
UPDA STIF KT1 ALL
which results in updating of K at the beginning of an increment (i = 1),
or by
UPDA STIF KT2 ALL
which results in K being updated at the 2nd iteration.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-12
Appendix C
ASAS (Non-Linear) User Manual
constraint surface
dP
load - deflection curve
dPi,1
dP i,2
dQi,1
dQi,2
dQ
Figure C.2.4 Modified Newton-Raphson
(c)
Initial stiffness, Figure C.2.5
The original structural stiffness matrix Ko is used at all iterations which results in the following form of
the equations (C.2.1)1 and (C.2.2)
K o * dQi ,1 = dPi ,1
(4.13)
K o * dQ j = dP j
This method is not suitable if the structure exhibits a high degree of non-linearity. This is the default
method.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-13
Appendix C
ASAS (Non-Linear) User Manual
dP
constraint surface
load - deflection curve
dQ i,1 dQi,2
dQ
Figure C.2.5 Initial Stiffness
(d)
Accelerations
The modified Newton-Raphson and initial stiffness techniques may be ‘accelerated’ by obtaining a new
correction of the displacement increment using a combination of current and previous displacements
rather than repeating the solution of the equilibrium equation. Two acceleration techniques are available
in ASAS-NL, namely
the Secant-Newton, requested by
OPTI SECN
and line search approach requested by
OPTI LINS
C.2.5 Solution methods
A number of solution methods are available in ASAS-NL by which the non-linear problem is solved in step by
step manner.
They can be obtained using various combinations of incremental and iteration techniques
described in the previous sections.
C.2.5.1 Euler-Cauchy method
The simplest method is the Euler-Cauchy integration scheme during which no iterative corrections are calculated
and unbalanced load from previous step is neglected. This method is also called the ‘tangent’ stiffness method,
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-14
ASAS (Non-Linear) User Manual
Appendix C
since the evaluation of the tangent stiffness matrix K, based on the state at the beginning of the step is required.
It is realised using the following commands.
JOB STAT
PROB/TITL NRES LARG . . . .
SOLV or SOLU . . . .
UPDA STIF INCR ALL
UPDA GEOM
ITER 1 TO END
OPTI OVIT
C.2.5.2 Self-correcting Euler-Cauchy
The Euler-Cauchy method can be considerably improved by taking into account the unbalanced (residual) load
due to non-linear effect. In structural analysis this method is also called “the initial load” method. It is realised
by
JOB STAT
PROB/TITL LARG . . . .
SOLV or SOLU . . . .
UPDA STIF INCR ALL
UPDA GEOM
ITER 1 TO END
OPTI OVIT
C.2.5.3 Full incremental - iterative method
This method is a combination of incremental process with an iterative technique. In ASAS-NL this combination
is defined by the user and no restrictions are imposed. Also the iteration techniques chosen can be combined
with any of the constraint surfaces available. It is realised by
JOB STAT
PROB/TITL LARG . . . .
SOLV or SOLU . . . .
UPDA STIF . . . .
UPDA GEOM . . . .
However the type of increment and the type of constraint surface must be of the same nature since they are
defined using the same command for both. For example
SOLU ARCL
results in incrementation of the displacement vector and use of cylindrical surface. Graphical representation of
this method is shown in Figure C.2.6.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-15
Appendix C
ASAS (Non-Linear) User Manual
Load
Displacem ent
Figure C.2.6 Arclength Solution Procedure with Cylindrical Constraint Surface
C.2.6 Conclusions
Two purely incremental methods described above constitute cheap but inaccurate way of tracing a non-linear
equilibrium path. In practice the solution should be rather calculated using full incremental-iterative approach,
exploiting to the best advantage a variety of options available within that method.
First a choice between SOLV or SOLU method has to be made. Having in mind full large displacement elastoplastic analysis, including possible bifurcation or snap through phenomena the arclength type method is
recommended as well suited to trace load-displacement path which contains limit points of both load and
displacement character. SOLV method should be used when solution to precisely specified load is necessary.
Therefore making first approach to obtain a solution of general non-linear problem involving both material and
geometrical non-linearities, the following procedure is recommended
1.
For non-proportional loading
JOB STAT
PROB/TITL LARG PLAS . . . .
SOLU LOAD . . . .
UPDA STIF ITER ALL
UPDA GEOM
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-16
ASAS (Non-Linear) User Manual
2.
Appendix C
If limit point is expected and proportional loading
JOB STAT
PROB/TITL LARG PLAS . . . .
SOLU ARCL nn . . . .
(or SOLU CONSIT nn AUTO . . . .)
UPDA STIF ITER ALL
UPDA GEOM
This procedure may then be changed during the course of analysis allowing to ‘tailor’ the type of non-linear
strategy to the problem being solved, thus increasing computational efficiency. This can be done using Restarts
and redefining controlling commands.
The termination of iteration within each increment is based upon satisfaction of certain criteria. This as well as
possibility of automatic restart in the case of converging solution is discussed in the later section.
C.3
Computation of Stresses
In the previous section global strategies for solution of non-linear equilibrium equations and calculation of
displacements were discussed. Separate problem which has to be dealt within each solution cycle is the
calculation of strain and stress states. As already mentioned those calculations are performed at a number of
integration points within each element according to the following algorithm.
First using geometrical relations vector of total strains E is obtained from current displacements. Then vector of
strain increments dE is calculated and applying constitutive relations vector of stress increments dS is evaluated.
In the elastic case this relation has the linear form
dS = D* dE
(C.3.1)
In the case of plasticity the constitutive relation is in general of non-linear character
dS = D* (dE- dE p)
(C.3.2)
where dEp is the vector of plastic strain increments and is a function of the stress state.
In ASAS-NL, there are two different approaches to integrate the incremental elastic-plastic constitutive
relationship and these are called the Forward Euler and Backward Euler schemes, respectively. Forward Euler
scheme is the default in the program and Backward Euler scheme is activated by OPTION BAKE.
C.3.1 Forward Euler Integration Scheme
The single step Forward Euler scheme is an explicit method that uses the plastic flow direction and yield
condition at the beginning of a step as the reference. Due to its explicit nature, the scheme is only conditionally
stable and will fail if very large increments of plastic strain occur within a step. To make the solution process
more stable and to improve accuracy, a technique known as sub-incrementation can be adopted where the strain
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-17
Appendix C
ASAS (Non-Linear) User Manual
increment is divided into a number of sub-increments and the stresses accumulated accordingly. Illustrations of
the Forward Euler scheme with and without sub-incrementation are given in Figure C.3.1.
The number of sub-increments NSUB for each strain increment can be determined either by setting it explicitly
using
PARA SUBINC NSUB (default to 1)
or by setting the required size of strain sub-increment using
PARA SUBTOL tolerance value
S
no sub-increment
NSUB sub-increments
stress-strain relation curve
dS
E
NSUB
dE
Figure C.3.1 Forward Euler Integration Scheme
The number of sub-increments is then determined by
NSUB =| dET * dE | /SUBTOL
(C.3.3)
The appropriate value of SUBTOL may be difficult to predict, thus giving it the value 0.0 results in
NSUB = ((| dET (i) * dE(i) |) /(| dET (1) * dE(1) |)) *10
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
(C.3.4)
Page C-18
Appendix C
ASAS (Non-Linear) User Manual
During the iteration process the element strains and stresses are calculated after each iteration. In ASAS-NL this
calculation is approached by the “path independent” scheme. The flow chart for the stress computation is shown
in Figure C.3.2.
Qi , j
current total displacements
Ei , j
current total strains
d Ei , j = Ei , j - Ei-1
dSi , j = f(dEi , j )
Si , j = Si-1 + dSi , j
incremental strains
constitutive law
current total stresses
Figure C.3.2 Flow Chart of Path Independent Stress Calculation
In the path independent scheme strain increment is calculated as the difference between the current strains and
those obtained from the previous step (increment), related therefore to converged solution. Corresponding stress
increment as well as total stress are then calculated. But until a convergence is satisfied the total stress
contribute only to recalculation of unbalanced load (residuals) used in the next displacement iteration. The final
state, being a sum of the previous converged solution and the current increment does not depend directly on the
solution path.
The main advantage of the path independent scheme is that it reduces the risk of incorrectly predict unloading
during plasticity analysis. It is particularly suitable to be used in combination with variable load methods. In
situations where the strain increment may have relatively large values, it is more effective to use the path
independent scheme in combination with sub-incrementation or with the Backward Euler Integration Scheme in
the next section.
C.3.2 Backward Euler Integration Scheme
The Backward Euler scheme is a fully implicit method where the plastic conditions are enforced at the end of a
load step. It is unconditionally stable and is therefore capable of handling large plastic strain increments. It has
been shown that rapid convergence of the global set of non-linear equilibrium equations can be achieved if the
Backward Euler scheme adopts a path independent strategy and a “consistent” tangent modulus that takes into
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-19
ASAS (Non-Linear) User Manual
Appendix C
account the effect of finite step size is employed in the stiffness calculation. This procedure will be in force
when OPTION BAKE is specified
At present, the Backward Euler scheme is only available for von Mises yield criterion with isotropic and/or
kinematic hardening. For plane stress, beam and shell elements, there is an additional requirement that any nonlinear hardening must be isotropic. Other types of yield surfaces must use the Forward Euler scheme.
C.4
Convergence and Auto-Recovery
C.4.1 Convergence Check
The convergence criteria specify what level of accuracy of the iterative solution is acceptable. Convergence
check is performed after each iteration using the following inequality
NORM (dq j) /NORM (qi , j ) <= tolerance
where dqj is j-th iterative correction of selected quantity, calculated during i-th increment, and qi,j is the total
incremental value of this quantity obtained after j-th iteration of i-th increment. Several state variables can be
used in the convergence criteria, such as; displacements, residual forces, strains and stresses. NORM used in the
left hand side of the above inequality may be selected as one of the following; Absolute, Euclidean, or Maximum
value. In addition if displacements or residual forces are used in the convergence criteria, its components can be
scaled according to the formula
(dQT * D* dQ)
or
(dPT * D-1 * dP)
for displacements or residual forces respectively, where D is the matrix of diagonal stiffness terms.
After the convergence requirement is satisfied the run is terminated or the next increment can be started.
Otherwise the iterative process is repeated and new values of state variables are calculated. However the number
of iterations within one increment is limited (to default number of 10, or to the user specified number). If
convergence test is not satisfied within that limit the run is terminated.
C.4.2 Auto-Recovery
In some cases the iteration process may not be converging fast enough or even diverging. A facility is available
in the SOLU procedures to break out of diverging (or slowly converging) iteration process and restart a new one
from last converged solution. For restarted increment standard Newton-Raphson iteration procedure will be
automatically invoked and step size will be reduced
new step = STEPRF * old step
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-20
Appendix C
ASAS (Non-Linear) User Manual
The multiplier STEPRF has the default value 0.5, but if required can be redefined using the PARAMETER
command. The number of auto-recoveries is 3 by default, but it again can be adjusted using the PARAMETER
command and specifying required number after parameter MXAUTO.
C.5
Eigenvalue Analysis
In ASAS-NL three separate applications of eigenvalue analysis are available. First is to a stability analysis
which provides the information about a buckling load. The buckling (or bifurcation) point is defined as the
intersection between two distinct equilibrium paths; primary and secondary.
Two situations may be
distinguished
(a)
Linear prebuckling behaviour, where the primary path is linear (e.g. Euler column).
(b)
Non-linear prebuckling behaviour characterized by non-linear primary path (e.g. shallow circular arch
under central point load).
The second application is to spectral analysis of the small displacement stiffness matrix.
The third application is for natural frequency analysis to evaluate the vibration characteristics of a loaded or
unloaded structure.
C.5.1 Linear Pre-buckling Case
To obtain the bifurcation point for the situations where the pre-buckling (or primary path) is linear, the following
eigenvalue problem is solved
(K o + λ * K G ) *φ = 0
(C.5.1)
where Ko is the current small deflection stiffness, KG(σ) the geometric stiffness, λ is the eigenvalue and
φ
is
eigenmode.
The buckling (critical) load Pc, is given by
Pc = λ * P
(C.5.2)
where P is the applied load.
C.5.2 Non-linear Pre-buckling Case
In this case the buckling problem may be derived from an incremental displacement relation
K* dQi = dPi
(C.5.3)
or in expanded form
(K o + K G ) * dQi = d Pi
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
(C.5.4)
Page C-21
ASAS (Non-Linear) User Manual
Appendix C
Assuming locally linear behaviour, buckling occurs if it is possible to find a displaced state
dQ+ φ without
change in load dP. In other words there exist a neighbouring configuration
dQ+ φ that is also in equilibrium
with load dP. The incremental load deflection relationship is thus
(K o + λ i * K G ) *φ = 0
(C.5.5)
in which we seek values of the multiplier λi which yields a non-zero solution for
φ.
It is possible to carry out
an eigenvalue analysis at any point in the load history once a converged state has been reached i.e. at the end of
an increment.
The buckling (critical) load is again calculated from the formula
Pic = λ * P
(C.5.6)
P
critical load curve
λ>1
bifurcation point
λ=1
λ<1
secondary path
primary
path
Q
Figure C.5.1 Critical Load Evaluation using Eigenvalue Analysis
Figure C.5.1 illustrates the procedure, where the solid curve is the load-deflection curve (the so called primary
path). The dashed curve is the locus of critical loads Pic. The point of intersection between these two curves
occurs at λ = 1 and coincides with the bifurcation point. However because in many practical cases the critical
load curve is almost straight, it is not necessary to carry out costly eigenvalue analysis at every increment. Often
two or three points on that curve are sufficient to determine the bifurcation point (Ref.C.1).
C.5.3 Spectral Analysis
This is a standard eigenproblem written in the form
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-22
ASAS (Non-Linear) User Manual
(K o + λ I)φ = 0
Appendix C
(C.5.7)
where I is the unit matrix. The solution of (C.5.7) is used in the evaluation of an element stiffness matrix or in
the calculation of the condition number of a structure stiffness matrix.
C.5.4 Natural Frequency Analysis
In this case the eigenproblem can in general be written as
(K o + K G + K C) φ i = w i2 M φ i = λ i M φ i
where
Ko and KG
Kc
M
λi
φi
(C.5.8)
are as defined before
is the centrifugal stiffness and is a function of the angular velocity
is the mass matrix
is the ith eigenvalue and is equal to the square of angular velocity, wi
is the corresponding mode shape
Once the eigenproblem is solved, the natural frequency of vibration, fi, can be obtained from
fi =
wi
2π
Note that if the structure is not spinning or loaded in any way, both KG and Kc will be zero and equation (C.5.8)
becomes
Ko φ i = wi M φ i
2
which is the standard generalised eigenvalue problem for unloaded structures.
C.6
Contact Analysis
Two types of solution procedures for contact analysis are available in ASAS-NL; namely the penalty method and
the augmented Lagrangian method. The penalty method is used for both gap elements and rigid surface
elements while the augmented Lagrangian method is only available to rigid surface elements on request (by
specifying a positive integer for PARAmeter MXAUGM).
C.6.1 Penalty Method
In this method, penalty springs of very high stiffness are introduced at regions where contact occurs to enforce
the necessary impenetrability and stick (if any) conditions. The contact constraints can be more strongly
satisfied by increasing the penalty stiffness but this may also create matrix conditioning problems. On the other
hand, the contact conditions may not be properly enforced if the penalty is too small. Thus, the choice of
suitable penalty parameters for the solution is very important.
In ASAS-NL, the penalty stiffness for the gap elements is specified through the effective stiffness from the
material property data and the parameter GAPSTF. These two parameters can be adjusted to give the desired
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-23
ASAS (Non-Linear) User Manual
Appendix C
penalty effect. Magnitudes of the penalty stiffness for the rigid surface elements in both the normal and
tangential directions are supplied as elastic and Coulomb friction material data.
C.6.2 Augmented Lagrangian Method
The augmented Lagrangian method (Ref C.2) can be viewed as a combined Lagrange multiplier and penalty
method. It has been shown that this method can provide added robustness to the penalty approach because of its
ability to correct under-penalised solutions while maintain good numerical conditioning.
In essence, the
augmented Lagrangian method assumes that the contact forces are decomposed into the penalty and Lagrange
multiplier parts. Instead of treating the Lagrange multipliers as additional global variables, they are fixed during
the global solution stage and thus the entire solution process works in the same way as the penalty method, with
the appropriate consideration of the multiplier contributions. Augmentation of the multipliers is performed only
after a new global solution is obtained and when the following conditions are met:
1.
The maximum number of augmentations, MXAUGM, has not been reached, and
2.
Contact conditions have not been completely satisfied, i.e. penetration > GAPCVG at any of the contact
positions, or relative tangential displacement > TANCVG at any of the stick positions.
MXAUGM, GAPCVF and TANCVG are parameters which may be reset using the PARA command.
C.7
C.1
References
Chang, S.C. and Chen, J.J., ‘Effectiveness of Linear Bifurcation Analysis for Predicting the Non-linear
Stability Limits of Structures,’ Int. Jnl. Num. Methods in Eng., Vol.23, pp831-846, 1986.
C.2
Simo, J.C., and Laursen, T.A., ‘An Augmented Lagrangian Treatment of Contact Problems Involving
Friction’, Comp. Struct., Vol. 42, pp97-116, 1992.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page C-24
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix C
Page C-25
ASAS (Non-Linear) User Manual
Appendix - D
D.1
Appendix D
Restarts
Introduction
Restarts have obvious advantages in economy and convenience compared with re-running an original analysis
from the start and are normal practice for most non-linear analyses. The facilities provided in ASAS-NL allow
an analysis to be restarted from any previous valid load step with a new set of control instructions and loading if
required. For a restarted job, only the Preliminary data, suppressions data, prescribed freedoms data, loading
data and additional mass data may be changed.
Restarts may be used for a number of purposes, including:
•
running an analysis in a series of controlled stages
•
continuing an analysis terminated through lack of resources
•
re-running with new loading
•
re-running (from previous steps) with new solution strategies
•
continuing an analysis from onset of non-linear behaviour after scaling the initial linear analysis with
the SCALE command.
During the course of an analysis, information about the current state of the analysis is saved on two external
files, the data manager archive file and element stiffness matrix archive file (see Section 4.4.4), according to
instructions specified with the Preliminary data SAVE command. When a restart is attempted, the internal file
structure is re-created from these two backing files. Restarts may thus only be performed from load steps at
which the two backing files were archived in the initial analysis.
D.2
Initial Analysis
The following action is needed:
(i)
Define the names of the (new) stiffness and data manager archive files. This is done by means of FILE
commands (one for each file), together with the directive ‘NEW’ specified with the SAVE command. If
no names are defined explicitly, default names (see Section 6) will be used, but this is not recommended.
(ii)
With the SAVE command, give the increments at which data is to be archived.
In the absence of a SAVE command, both files are automatically archived for the last load increment
only.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page D-1
ASAS (Non-Linear) User Manual
Appendix D
Note that stiffness matrices are only archived if a change of state has taken place from the previous
archive. Thus, the stiffness file may not be checkpointed at certain load stages, despite the request with
the SAVE command.
D.3
Restarted Jobs
Before restarting an analysis, the user must ensure that the appropriate data manager and stiffness files for the
restart are to hand.
If the restarted analysis is to follow the original load history then only Preliminary data should be present,
together with a STOP command.
If the load history or boundary conditions are to be redefined, then all data blocks including the STOP command
are required. However, in this case the structural description data must be identical to the original model.
The following points apply to Preliminary Data:
(i)
The name and title specified with the PROJECT command must be the same as for the initial analysis.
(ii)
The name of an existing structure within the same project should be specified with the STRUCTURE
Command.
(iii)
The name of the structure to be created in this run should be specified with the NEWSTRUCTURE
command
(iv)
The name of the old data manager archive file must be specified with the JOB command together with the
checkpoint number of the restart. The checkpoint number is given preceding the displacements for the
restarted load step on the ASAS-NL output file for the initial analysis.
(v)
The name of the old stiffness matrix file may optionally be given with a FILE command.
(vi)
The SOLVE command should be replaced by a RESTART command, giving the time from which the
restart is to be made (say Tr), followed by a list of solution times. No solution is attempted at the restart
time Tr. The checkpoint number specified with the JOB command must correspond to the load step Tr.
If the SOLU command was used in the initial analysis it should be replaced by the SREST command,
giving the increment number from which the restart is to be made. No solution is attempted at this
increment.
(vii)
Number of groups and their definition must be the same for both initial and restarted runs.
(viii) Archiving during the restart should be defined as before using the SAVE command.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page D-2
ASAS (Non-Linear) User Manual
(ix)
Appendix D
If the option ‘NEW’ is specified on the SAVE command, then new backing files will be created during
the restarted analysis. The file names should be defined using FILE commands. If the option ‘OLD’ is
specified with the SAVE command, then the old backing files will be used for all archiving during the
restart. Archived information will be appended to previously archived data up to the restart time. Any
previous archives made after the restart time will be overwritten.
In general, it is recommended that ‘NEW’ be used rather than ‘OLD’.
D.4
Examples
Initial Analysis
A sample ASAS-NL data file for performing an initial analysis is given below.
SYSTEM
DATA
AREA
2000000
PROJ APRJ * RESTARTS
STRUCTURE ASTR
JOB STAT
TITL
PLAS
SOLV
FILE
0.1 0.2 0.3
ARCH ARCHA
*INITIAL
FILE
UPDA
NSTF
STIF
SAVE
NEW
STIFA
KT2 0.1
ANALYSIS
0.4
0.3
ALL
END
Structural description data
Boundary conditions data
Loading data
Additional mass data
(Initial conditions data)
STOP
Checkpoints are written to the new archive files ARCHA and STIFA for each load increment as follows:
Increment
Time
File
Checkpoint
1
0.1
STIFA
ARCHA
1
2
2
0.2
ARCHA
3
3
0.3
STIFA
ARCHA
3
4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page D-3
ASAS (Non-Linear) User Manual
Appendix D
4
0.4
ARCHA
5
The two files are checkpointed separately. Checkpoint 1 is written to ARCHA by PRENL. STIFA is not
checkpointed for load steps 0.2 and 0.4 as the stiffness matrices are not reformed in these load steps (see UPDA
command).
Restarted Analysis
The ASAS-NL data file for performing a restart from the conclusion of the second load step is as follows:
SYSTEM
DATA
AREA
20000
PROJ APRJ *RESTARTS
STRUCTURE ASTR
NEWSTRUCTURE BSTR
JOB STAT ARCHA (3)
TITL
PLAS
*EXAMPLE
REST
FILE
0.2 0.3 0.4
OSTF STIFA
FILE
FILE
NSTF
ARCH
UPDA
STIF
SAVE
END
NEW
RESTART
0.5
0.6
STIFB
ARCHB
INCR
0.4
0.2
0.5
STOP
Checkpoint 3 is used on the data manager archive file. New backing files ARCHB and STIFB are created in the
restarted analysis. The checkpoints written during the restarted analysis are:
Increment
Time
File
Checkpoint
4
0.4
ARCHB
5
5
0.5
ARCHB
6
6
0.6
ARCHB
7
No solution is attempted at the first solution time specified with REST command. The file STIFB was not
created as the element stiffness matrices are not reformed during the analysis.
Re-Restart Analysis
A further restart continuing the analysis from the end of the previous restart is obtained with the following:
SYSTEM
DATA
PROJ APRJ
AREA
2000000
*RESTARTS
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page D-4
ASAS (Non-Linear) User Manual
Appendix D
STRUCTURE BSTR
NEWSTRUCTURE CSTR
JOB STAT ARCHB (7)
TITL PLAS *EXAMPLE
REST
0.6
UPDA
END
STIF
0.7
KT2
RE-RESTART
0.8
ALL
STOP
The archived element stiffness matrices are read from STIFA and data manager file from checkpoint 7 on
ARCHB created in the previous restart analysis. The new checkpoints created are:
Increment
Time
File
Checkpoint
8
0.8
STIFA
ARCHB
8
9
As no SAVE command was given, the original backing files were overwritten (in this case the restart continued
from the end of the previous restart and thus the extra checkpointed information would be appended to the
original backing file).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page D-5
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix D
Page D-6
ASAS (Non-Linear) User Manual
Appendix - E
E.1
Appendix E
Example Data Files
Example 1: BM3D Plasticity Model (T0574)
Description
Data
SYSTEM DATA AREA 100000
PROJ *VALIDATION TEST FOR PLASTICITY MODEL FOR BM2D AND BM3D
JOB STAT
TITL PLAS * 3D FRAME COLLAPSE - SHI ET AL (EX.3)
TEXT
TEXT
ASAS-NL TEST FILE - T0574PRE.DAT
CREATED - 23/07/90
SOLV 10.0 12.0 14.0 16.0 17.0 17.5 17.75 18.0 18.25 18.5 18.75 19.0
SOLV 19.25 19.5 19.75 20.0 20.15
UPDA STIF ITER ALL
PARA SUBINC 5
OUTP 1 ALL
BLOC 1 SRES
OPTI PIND
END
COOR
1
2 0 0 2500
3 0 0 5000
4 5000 0 0
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-1
ASAS (Non-Linear) User Manual
Appendix E
5 5000 0 5000
6 0 5000 5000
7 0 10000 5000
8 0 10000 0
9 5000 10000 5000
10 5000 10000 0
END
ELEM
MATP 1
BM3D 1 2 1
BM3D 3 5 1
BM3D 5 4 1
BM3D 6 7 1
BM3D 5 9 1
BM3D 8 7 1
BM3D 7 9 1
BM3D 9 10 1
MATP 2
BM3D 2 3 1
BM3D 3 6 1
END
MATE
1 ISO 207000 0.3
1 PLAS BEAM 8.1127E6 8.4582E8 8.4582E8
: 1.0 2.0 1.0 2.0 1.0 2.0
2 ISO 207000 0.3
2 PLAS BEAM 8.1127E6 9.0E8 9.0E8
: 1.0 2.0 1.0 2.0 1.0 2.0
END
GEOM
1 BM3D 2.3628E4 3.17376E8 3.17376E8 6.34752E8 2500 5000 0
END
SUPP
ALL 1 4 8 10
END
LOAD
SET 1 VERT AND HORIZ LOAD
NODAL LOAD
X 49050. 2
X 24525 6
Z -49050. 3 5 7 9
END
STOP
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-2
ASAS (Non-Linear) User Manual
E.2
Appendix E
Example 2: TCS9 Geometric non-linearity (T0533)
Description
Data
SYSTEM DATA AREA 100000
PROJ * FOUR AND NINE NODE SHELLS
JOB STAT
TITL LARG * SHELL ROOF UNDER VERTICAL PRESSURE
TEXT
TEXT
SOLV
PRENL TEST DATA - T0533PRE.DAT
CREATED - 23/04/90
.001 .002
.003 .004
UPDA GEOM ITER ALL
UPDA STIF ITER ALL
PARA PENFUN 1.E-3
END
DRILF 1.E-6 SHEARL 0.0
COOR
CYLI AXES
RAD
DCOS 1. 0.0 0.0 0.0 0.0 -1.
ORIG
//
/
1
RP
0.0
0.0
7600.
4.71238898
9
1
RRP
END
0.0
0.0
9
9
0.0
.087266462
0.0
0.0
0.0
950.
ELEM
//
/
TCS9
1
2
3
12
21
20
19
10
11
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
1
1
Page E-3
ASAS (Non-Linear) User Manual
RP
RRP
4
4
Appendix E
2
18
END
MATE
1
ISO
2.1E4
TCS9
76.
0.0
0.0
1.3412736E-6
END
GEOM
1
END
SUPP
X
1
X
10
19
28
37
46
55
64
73
2
3
4
5
6
7
8
9
Y
Z
73
1
74
2
75
3
76
4
77
5
78
6
79
7
80
8
81
9
RX
RY
73
1
74
2
75
3
76
4
77
5
78
6
79
7
80
8
81
9
10
19
28
37
46
55
64
73
10
74
19
75
28
76
37
77
46
78
55
79
64
80
73
81
RY
RZ
RZ
1
END
LOAD
SET 1
BODY FOR
0.0
0.0
-9810.
END
STOP
E.3
Example 3: QUX4 Incompressible behaviour (T0540)
Description
Sphere under internal pressure
1. 16 QUX4 elements with constant volumetric
dilatation (i.e. PINO 1)
2. ν=0.49999
Inner radius = 0.5
Outer radius = 1.0
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-4
ASAS (Non-Linear) User Manual
Appendix E
Data
SYSTEM DATA AREA 100000
PROJ * HYPERELASTICITY AND INCOMPRESSIBILITY
JOB STAT
TITL * ISOTROPIC SPHERE UNDER INTERNAL PRESSURE (QUX4)
TEXT
TEXT
ASAS-NL TEST FILE - T0540PRE.DAT
CREATED - 15/03/90
SOLV 1.0
PINO 1 (16) (1,1)
OUTP 1 ALL
BLOC 1 DISP
OUTP 2 ALL
(5)(1,1) (5)(33,1)
BLOC 2 STRS STRN
END
1
2
3
4
COOR
CYLI
XXXX
DCOS 1.0 0.0 0.0 0.0 0.0 1.0
ORIG 0.0 0.0 0.0
//
/
1
RP
0.5
5 1
0.0
0.125 0.0
RRP 4 8
FIN
0.0
22.5
CART
/
33
0.0
0.0
0.5
RP 5 1
END
0.0
0.0
0.125
ELEM
MATP
1
/
QUX4
1
2
10
9
QUX4
2
3
11
10
QUX4
QUX4
3
4
4
5
12
13
11
12
RP
END
4
8
MATE
1
ISO
END
20000.0
0.49999
SUPP
/
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-5
ASAS (Non-Linear) User Manual
Z
R
Appendix E
1
33
RP
END
5
1
LOAD
SET 1 ’INTERNAL PRESSURE’
PRESSURE
/
U
RP
END
1.0
1
4
8
9
STOP
E.4
Example 4: QUS4 Elasto-plastic stiffened shell (T0553)
Description
R=400
L=200
t=1 (shell)
stiffener depth=10=D
thickness (stiffener)=1
E=2.1x105, ν=0.3,
σy=350
R
L=200
D
96 QUS4 elements
47 increments
181 iterations
54 stiffeners
Data
SYSTEM DATA AREA 350000
SYSPAR LPGSIZ 256
PROJ * FOUR AND NINE NODE SHELLS
JOB STAT
TITL PLAS LARG *STRINGER STIF. CYL. - IMP. COLL. PROB. F10
TEXT
TEXT
PRENL TEST FILE - T0553PRE.DAT
CREATED - 23/04/90
TEXT
TEXT
CYLINDRICAL PANEL WITH FLAT BAR STRINGER STIFFENER
TEXT
TEXT
R=400.0 L=200.0 T=1.0 STIFFENER D=10.0 T=1.0
E=2.1E5,PR=0.3 SIGY 350
TEXT
IMPERIAL COLLEGE PROBLEM - F10
TEXT
DRILF 1.E-6 PENFUN 1.E-3 FLATOL 90.0
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-6
ASAS (Non-Linear) User Manual
TEXT
TEXT
Appendix E
INTE 1 1 5
SOLU ARCL 50 INITPR 14.25 ITERD 4 MAXDIS 3 Z 0.4
UPDA STIF KT2 ALL
UPDA GEOM ITER ALL
PARA DRILF 1.E-6 PENFUN 1.E-3 FLATOL 90.0
OUTP 1 ALL
BLOC 1 DISP 3
ITER 20 TO END
INTE 1 1 5 (96)(1,1)
CONV EUCN DISP 0.001
OPTI GOON PIND AUTO OVIT
FILE POST T0553PST
POST DISP ALL
END
COOR
CART
1 395.0753
2 398.7669
-62.5738
-31.3836
0.0000
0.0000
3 400.0000
4 398.7669
0.0000
31.3836
0.0000
0.0000
5 395.0753
6 395.0020
62.5738
-62.5622
0.0000
16.6667
7 400.0000
0.0000
16.6667
8 395.1487
9 394.9299
62.5854
-62.5508
16.6667
33.3333
10 398.6631
11 400.0000
-31.3755
0.0000
33.3333
33.3333
12 398.8707
31.3918
33.3333
13 395.2208
14 394.8603
62.5968
-62.5397
33.3333
50.0000
15 400.0000
16 395.2904
0.0000
62.6079
50.0000
50.0000
17 394.7944
18 398.5664
-62.5293
-31.3679
66.6667
66.6667
19 400.0000
0.0000
66.6667
20 398.9675
21 395.3563
31.3994
62.6183
66.6667
66.6667
22 394.7332
23 400.0000
-62.5196
0.0000
83.3333
83.3333
24 395.4174
62.6280
83.3333
25 394.6779
26 398.4833
-62.5108
-31.3613
100.0000
100.0000
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-7
ASAS (Non-Linear) User Manual
Appendix E
27 400.0000
28 399.0505
0.0000
31.4060
100.0000
100.0000
29 395.4727
30 394.6295
62.6367
-62.5032
100.0000
116.6667
31 400.0000
0.0000
116.6667
32 395.5212
33 394.5887
62.6444
-62.4967
116.6667
133.3333
34 398.4196
35 400.0000
-31.3563
0.0000
133.3333
133.3333
36 399.1143
37 395.5620
31.4110
62.6509
133.3333
133.3333
38 394.5561
-62.4916
150.0000
39 400.0000
40 395.5946
0.0000
62.6560
150.0000
150.0000
41 394.5325
42 398.3795
-62.4878
-31.3531
166.6667
166.6667
43 400.0000
0.0000
166.6667
44 399.1544
45 395.6182
31.4141
62.6598
166.6667
166.6667
46 394.5182
47 400.0000
-62.4855
0.0000
183.3333
183.3333
48 395.6325
49 394.5133
62.6620
-62.4848
183.3333
200.0000
50 398.3658
-31.3521
200.0000
51 400.0000
52 399.1680
0.0000
31.4152
200.0000
200.0000
53 395.6373
54 397.5
62.6628
0.0
200.0000
0.0
55 397.5
0.0194
33.3333
56 397.5
57 397.5
0.0375
0.0531
66.6667
100.0000
58 397.5
59 397.5
0.0650
0.0725
133.3333
166.6667
60 397.5
61 395.0
0.0750
0.0
200.0000
0.0
62 395.0
0.0195
16.6667
63 395.0
64 395.0
0.0388
0.0574
33.3333
50.0000
65 395.0
66 395.0
0.0750
0.0913
66.6667
83.3333
67 395.0
0.1061
100.0000
68 395.0
69 395.0
0.1190
0.1299
116.6667
133.3333
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-8
ASAS (Non-Linear) User Manual
Appendix E
70 395.0
71 395.0
0.1386
0.1449
150.0000
166.6667
72 395.0
73 395.0
0.1487
0.1500
183.3333
200.0000
74 392.5
0.0
75 392.5
76 392.5
0.0583
0.1125
33.3333
66.6667
77 392.5
78 392.5
0.1591
0.1949
100.0000
133.3333
79 392.5
80 392.5
0.2174
0.2250
166.6667
200.0000
81 390.0
0.0
82 390.0
83 390.0
0.0390
0.0777
16.6667
33.3333
84 390.0
85 390.0
0.1148
0.1500
50.0000
66.6667
86 390.0
0.1827
83.3333
87 390.0
88 390.0
0.2122
0.2380
100.0000
116.6667
89 390.0
90 390.0
0.2598
0.2772
133.3333
150.0000
91 390.0
92 390.0
0.2898
0.2974
166.6667
183.3333
93 390.0
0.3000
200.0000
0.0
0.0
201
203
398.7147
398.8191
-31.3795
31.3877
16.6667
16.6667
209
211
398.6138
398.9200
-31.3715
31.3958
50.0000
50.0000
217
398.5234
-31.3644
83.3333
219
225
399.0104
398.4495
31.4029
-31.3585
83.3333
116.6667
227
233
399.0843
398.3973
31.4088
-31.3544
116.6667
150.0000
235
241
399.1366
398.3703
31.4129
-31.3522
150.0000
183.3333
243
399.1636
31.4150
183.3333
301
302
397.5000
397.5000
0.0097
0.0287
16.6667
50.0000
303
304
397.5000
397.5000
0.0457
0.0595
83.3333
116.6667
305
397.5000
0.0693
150.0000
306
307
397.5000
392.5000
0.0744
0.0293
183.3333
16.6667
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-9
ASAS (Non-Linear) User Manual
Appendix E
308
309
392.5000
392.5000
0.0861
0.1370
50.0000
83.3333
310
311
392.5000
392.5000
0.1785
0.2080
116.6667
150.0000
312
392.5000
0.2231
183.3333
END
ELEM
MATP 1
/
QUS4
QUS4
1 6 201
2 201 7
2 1
3 1
QUS4
3
4
QUS4
QUS4
4 203 8
6 9 10
5 1
201 1
QUS4 201 10 11
QUS4 7 11 12
7 1
203 1
7
203
QUS4 203 12 13
1
8
1
RP 6 8
/
QUS4
RP
3 7 301 54 2
6 8 8 1 1
/
QUS4
54
RP
6 1 1
/
QUS4
RP
/
7
301
62
QUS4
301 55
RP 6
/
1 1 2 2
2
2 2
11
6 8 8 1
61
55
301 2
63
62
1
2
QUS4 61 62 307 74 2
RP 6 2 2 1 1
/
QUS4 74 307 82 81 2
RP 6 1 1 2 2
/
QUS4 62 63 75
307 2
RP 6 2 2 1 1
/
QUS4 307 75 83 82
2
RP 6 1 1 2 2
END
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-10
ASAS (Non-Linear) User Manual
Appendix E
MATE
1 ISO 210000.0 0.3
1 PLAS MISE 350.0 0.0
END
GEOM
1 QUS4 1.0
2 QUS4 1.0
END
SKEW
1
2
0.9877
0.9969
-0.1564
-0.0785
0.0
0.0
0.1564
0.0785
0.9877
0.9969
0.0
0.0
3
0.9969
0.0785
0.0
-0.0785
0.9969
0.0
4
END
0.9877
0.1564
0.0
-0.1564
0.9877
0.0
SUPP
/
1 Y RX RZ 1
RP 7 8
/
1 Y RZ RX 6
RP 6 8
/
4 Y RX RZ 5
RP 7 8
/
4 Y RX RZ 8
RP 6 8
1 X Y RX RZ 1
2 X Y RX RZ 2
X Y RX RZ 3
3 X Y RX RZ 4
4 X Y RX RZ 5
1 Z RX RY 49
2 Z RX RY 50
Z RX RY 51
3 Z RX RY 52
4 Z RX RY 53
/
X Y RZ 54
RP 2 20
/
X Y RZ 61
RP 2 20
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-11
ASAS (Non-Linear) User Manual
Appendix E
/
Z RX RY 60
RP 2 20
/
Z RX RY
73
RP 2 20
END
LOAD
SET 1
NODAL LO
1 Z 1 15.705 1
2 Z 1 31.41 2
Z 1 32.66 3
3 Z 1 31.41 4
4 Z 1 15.705 5
Z 1 2.5 54
Z 1 2.5 61
Z 1 2.5 74
Z 1 1.25 81
END
LOAD-FUN
1 0.0 0.0 350000.0 350000.0
END
STOP
E.5
Example 6: QUS4 transient dynamics (T0591)
Description
Impulse loaded clamped plate (one quarter model)
Lines of Symmetry
v1
v2
0.6
5.0
t
ρ
E
ν
σy
=
=
=
=
=
0.125
2.61x10-4
10.4x106
0.3
41.4x103
Initial velocities
Features:
1.
2.
3.
4.
5 QUS4 elements
1x1x5 integration
LARG+PLAS
TALPHA = -0.05
v1 = 5000
v2 = 3904
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-12
ASAS (Non-Linear) User Manual
Appendix E
Data
SYSTEM DATA AREA 180000
PROJ *AUTOMATIC TIMESTEPPING TEST
JOB TRAN
TITL LARG PLAS * IMPULSE LOADED CLAMPED PLATE (1/4 MODEL)
TEXT
TEXT
PRENL TEST FILE - T0591PRE.DAT
CREATED - 31/05/92
SOLU DOMFRQ 26 FIRTIN 1.0E-5 MAXTIM 1.0E-3
TEMP TALPHA -0.05 KSIGNL 3 FINCMX 1.5
UPDA GEOM ITER ALL
UPDA STIF ITER ALL
INTE 1 1 5 (5)(1,1)
OPTIONS GOON PIND SAVJ BAKE
OUTP 1 ALL
BLOC 1 DISP 11
END
COOR
CART
//
/
1 0.0 0.0 0.0
RP 6 1 1.0 0.0 0.0
RRP 2 10 0.0 0.6 0.0
END
ELEM
MATP 1
/
QUS4 1 2 12 11 1
RP 5 1
END
MATE
1 ISO 10.4E06 0.3 0.1E-05 2.61E-4
1 PLAS MISE 41.4E3 0.0
END
GEOM
1 QUS4 0.125
END
SUPP
ALL
6
16
X RY RZ 1
Y RX
11
11
Y RX RZ 12
END
13
14
15
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-13
ASAS (Non-Linear) User Manual
Appendix E
LOAD
SET 1 DUMMY NODAL LOAD
NODAL LO
Z
1
1.0
11
END
LOAD-FUN
1 0.0 0.0 2.0 0.0
END
INIT
Z
Z
0.0
0.0
5000.0
3904.0
1
2
11
12
END
STOP
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page E-14
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix E
Page E-15
ASAS (Non-Linear) User Manual
Appendix - F
Appendix F
List of Freedom Names
A three-character alphanumeric name is used to indicate each of the freedoms at a node. The direction of the
freedoms is determined by the current orientation of the global axes, for the particular node (i.e. the axes
established after any skewed suppression constraint or prescribed displacement has been applied).
The following list gives the freedom names used. Names with one or two characters must always be rightjustified in a three character field for fixed format data input.
ALL
All freedoms at the node
X
Displacement along the x-axis
Y
Displacement along the y-axis
Z
Displacement along the z-axis
RX
Rotation about the x-axis
RY
Rotation about the y-axis
RZ
Rotation about the z-axis
R
Displacement radially
WRR
Curvature about local r-axis
EZZ
Strain in z direction
T
Field variable
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page F-1
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix F
Page F-2
ASAS (Non-Linear) User Manual
Appendix - G
G.1
Appendix G
Isoparametric Elements
Curvilinear Axes
Isoparametric elements employ curvilinear coordinates l, m, n (or for triangular faces L1L2L3) which result from
‘mapping’ the element from its parent regular form to the actual distorted shape, see Figure G.1. Note that the
direction of each curvilinear axis is determined by the order in which the element nodes are listed. They do not
necessarily form a right handed system.
An element’s local axes (which is often the reference frame for stress and strain calculations) are usually defined
with respect to the curvilinear axes.
G.2
Integration Rules
All continuum elements in ASAS-NL use Gaussian quadrature; structural elements (i.e. shell and beam) use
Gaussian quadrature in the plane (axis) of the shell (beam) and closed Newton-Cotes rules for through thickness
effects.
The user is free to select the order of the rule used, but cannot change the type (e.g. from Gaussian to NewtonCotes). The order of rule required is specified by giving the number of integration points in each of the
elements’ local directions with INTEgration rule commands in the Preliminary data.
(For elements with
triangular faces the number of points in the triangular plane is given.) If an INTEgration rule command is not
present for an element the default rule (given on the element description sheet) is used.
For continuum elements integration points for each element are numbered sequentially from 1 in the order given
by (((X=1,NGX), Y=1,NGY),Z=1,NGZ) where NGX, NGY and NGZ are the number of integration points in
directions l, m, and n respectively. (For elements with triangular faces NGX is conventionally 1 and NGY is the
number of points in the triangular point rule.)
For beam and shell elements, all integration points with the same planar coordinates (i.e. l for beams, l, m, for
shells) are numbered sequentially from the bottom surfaces towards the top surface. Thus, for shell elements for
example, Surface 1 is the bottom surface and surface NGZ is the top suface.
Figure G.2 illustrates the above conventions.
The coordinates of all integration points can be printed at the start of the analysis by using option GAUS with the
OPTIons command. The position of each point within an element can be obtained from Table G.1.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page G-1
ASAS (Non-Linear) User Manual
Appendix G
Figure G.1 Curvilinear Axes for Shells and Beams
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page G-2
ASAS (Non-Linear) User Manual
Appendix G
Figure G.1 Curvilinear Axes for Continuum Elements (...cont.)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page G-3
ASAS (Non-Linear) User Manual
Appendix G
Figure G.2 Sample Point Numbering for Shells and Beams
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page G-4
Appendix G
ASAS (Non-Linear) User Manual
3
3
3
(1 x 1 x 1)
2
(1 x 3 x 1)
1
1
2
1
2
1
m
m
4
4
3
3
3
4
4
6
5
l
1
l
(2 x 2 x 1)
2
1
2
1
2
1
8
m
7
3
4
5
6
4
11
12
9
10
7
8
l
(2 x 3 x 2)
m
2
1
(3 x 2 x 1)
3
2
5
6
3
4
1
2
4
l
5
5
6
6
(1 x 3 x 2)
2
1
1
3
2
3
Figure G.2 Sample Point Numbering for Continuum Elements (...cont.)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page G-5
Appendix G
ASAS (Non-Linear) User Manual
P
a
A
B
c
c
Note, P is the integration point and a its position from the mid point of the curvilinear line AB, length 2c
No. of
Integration Points
1
2
3
4
5
6
7
8
9
10
11
GAUSS
+/- a/c
0.0
0.57735
0.77459
0.0
0.86113
0.33998
0.90617
0.53846
0.0
0.93246
0.66120
0.23867
0.94910
0.74153
0.40584
0.0
0.96028
0.79666
0.52553
0.18343
0.96816
0.83603
0.61337
0.32425
0.0
0.97390
0.86506
0.67940
0.43339
0.14887
0.97822
0.88706
0.73015
0.51909
0.26954
0.0
NEWTON-COTES
+/- a/c
0.0
1.0
1.0
0.0
1.0
0.33333
1.0
0.5
0.0
1.0
0.6
0.2
1.0
0.66667
0.33333
0.0
1.0
0.71429
0.42857
0.14285
1.0
0.75
0.5
0.25
0.0
1.0
0.77778
0.55556
0.33333
0.11111
1.0
0.8
0.6
0.4
0.2
0.0
Table G.1 Integration Point Positions for Different Rules (cont...)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page G-6
Appendix G
ASAS (Non-Linear) User Manual
No. of
Integration Points
12
13
GAUSS
+/- a/c
0.98156
0.90411
0.76990
0.58731
0.36783
0.12523
0.98418
0.91759
0.80157
0.64234
0.44849
0.23045
0.0
NEWTON-COTES
+/- a/c
1.0
0.81818
0.63636
0.45455
0.27273
0.09091
1.0
0.83333
0.66667
0.5
0.33333
0.16667
0.0
Table G.1 Integration Point Positions for Different Rules (...cont)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page G-7
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix G
Page G-8
Appendix H
ASAS (Non-Linear) User Manual
Appendix - H
ASAS/ASAS-NL Compatibility
ASAS/ASAS-NL Differences
The following ASAS Data are not appropriate to ASAS-NL.
Preliminary Data
ASAS has its own commands for this data
Structural Description
Component Topology
Boundary Conditions
Link freedoms
Master freedoms
Freedom Releases (Global)
Special Freedom Directions
Gaps
Loading
Component loads
Additional Mass
Consistent mass input
Component Recovery
All
Stiffness Input
All
Combined Loadcases
All
All other ASAS data blocks are fully compatible with ASAS-NL subject to the following:
Structural Description
Element Topology
Group numbers are assigned in the Preliminary data in ASAS-NL, not in the topology data as in ASAS.
Material Properties
Elastic material behaviour is defined as in ASAS. Additional data is required to define non-linear materials.
When defining anisotropic material properties in ASAS-NL, 30 properties are always required. This is not the
case with ASAS.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page H-1
ASAS (Non-Linear) User Manual
Appendix H
Loading Data
Load cases used in ASAS are treated as Load Sets in ASAS-NL. In general, a load function number may be
specified with ASAS-NL data, which is not required by ASAS.
Temperature Loads
Temperature values are construed as absolute temperatures and thermal loads are calculated due to the difference
between these and the reference temperature, TREFLD, defined in the Preliminary data (PARAMETER
command).
Face Temperature Loads
Similar to temperature loads.
Additional Mass
Lumped Mass Input
FULL MAS option is not available in ASAS-NL.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page H-2
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix H
Page H-3
ASAS (Non-Linear) User Manual
Appendix - I
Appendix I
POSTNL General Post-Processor Interface Program
I.1 Introduction
POSTNL is an interface program required by all ancillary post-processing programs. It converts the postprocessing file (or “porthole” file) produced by ASAS-NL when the POST command is used, into a suitable
format for the post-processor. It has the following uses (or “output options”)
1.
to interface with FEMVIEW
2.
to interface with PATRAN
3.
to produce time histories of one or more quantities for plotting
4.
to print selective element stress strain and associated quantities, and nodal displacements, eigenvectors
etc.
POSTNL will also, if appropriate to the output interface and requested by the user, perform certain additional
post-processing calculations
1.
calculation of principal stresses, stress resultants, strains etc.
2.
extrapolation of element integration point quantities (eg stresses & strains) to nodes. Principal quantities,
if requested, are not extrapolated but are recomputed from nodal quantities
3.
averaging of element nodal stresses at common nodes for all elements in a group. The averaging is done
across groups if specifically requested (except for the PATRAN interface where it is done automatically).
Note that no account is taken of any difference in the local axes system; thus it is up to the analyst to
ensure that the averaging is meaningful.
4.
recalculation of equivalent quantities (e.g. equivalent stress) at nodes following nodal averaging
5.
unskewing of any displacements or reactions in a local skew axis to the common global axis system (this
option is automatically enforced for PATRAN and FEMVIEW)
6.
recovery of layer stresses and strains for laminated shells and calculation of failure indices (for
FEMVIEW only)
7.
calculation of fracture mechanics parameters (for PRINT only)
I.2 Usage
The program is an interactive one which will prompt the user for the required response. The input commands are
echoed both to the terminal and also to a file named ZZZMONIT.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-1
ASAS (Non-Linear) User Manual
Appendix I
The program requires the name of the porthole file created by the ASAS-NL run. If this was not explicitly
named on a FILE command it will default to ZZZPORTF. POSTNL also requires to know whether any shell or
beam elements are to be post-processed (this information is needed in order to allocate space efficiently).
The program then asks for the “output option” required. The following 4 character options are valid
FEMV
-
to interface with FEMVIEW (see I.3)
PATN
-
to interface with PATRAN (see I.4)
PRIN
-
to print selected quantities (see I.5)
TIME
-
to obtain time histories of selected quantities (see I.6)
INDX
-
to obtain a list of the output types on the named porthole file for each increment (see
below)
NEW
-
to post-process output on another porthole file (see below)
STOP
-
to terminate the POSTNL session
On completion of the processing in one of the above ‘output options’ POSTNL prompts the user for a further
‘output option’. To exit from the program at this stage enter STOP.
To obtain a catalogue of the quantities saved on the porthole at each increment enter INDX. Identifiers are listed
together with pseudo-times.
On completion of the current post-processing, output on a different porthole file can be processed by entering
NEW. The program then asks for the name of the new post-processing file. Note that this has to be on the same
project, as identified with the ASAS-NL JOB command.
I.3 FEMVIEW Interface
The interface between POSTNL and FEMVIEW consists of a single formatted file containing details of both the
model (ie coordinates and element topology) and all the results to be displayed. POSTNL will either append the
results to an existing model file, or create it as required. In the former case the model file will have been created
by a FEMGEN run or by specifying FEMV with the ASAS-NL OPTIONS command, or in a previous session of
POSTNL.
After entering FEMV to request the FEMVIEW interface, the program asks for the ‘model name’ and an
‘operation code’ to indicate whether the model file is to be created anew (C) and the results added, or that the
results are to be appended to an existing model file (A). In the latter case the model name should correspond to
that on the existing model file (if this was created in the ASASNL run then the name is the first 6 characters of
the title specified with the TITLE/PROBLEM command).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-2
Appendix I
ASAS (Non-Linear) User Manual
If A is input POSTNL creates a file (with no structure data) which may be used to append to an existing
FEMVIEW data base for this model name. The program then asks for the filename to which results are to be
written. This name should be unique to avoid the possibility of deleting existing output files.
If operation code C was entered the filename must be the name of the existing model file (if created in the
ASAS-NL run this will be ZZZMODEL by default or otherwise as named with a FILE command).
The program then asks for the four character label identifying the output type and increment. Valid output type
labels are given in Table I.1. The next prompt determines the format in which quantities are output to the
FEMVIEW neutral file. Note that all element based quantities do not involve any averaging process across
element boundaries. Having transferred data for the current output type, the program prompts for the next output
type and increment. To exit, enter END. This will result in a prompt for a further output file name. To exit from
this level enter FIN.
Primary Nodal Variables
DISP
Displacements
VELO
Velocities
ACCN
Accelerations
REAC
Reactions
EIGN
Eigenvector
Primary Element Based Variables
STRS
Element stresses
STRN
Element (total) strains
ELAS
Element elastic strains
INST
Element plastic strains
CRSN
Element creep strains
TEMP
Element temperatures
SRES
Element stress resultants
(beams & shells only)
RESN
Element strain resultants
(beams & shells only)
Secondary Element Based Variables
LAMI
Lamina stress/strains and failure indices
GFAI
Shell global failure indices
SFAI
Shell surface failure indices
Table I.1 Output Types for FEMGEN
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-3
ASAS (Non-Linear) User Manual
Appendix I
The various prompts encountered using the FEMV option are detailed below.
Enter FEMV at the prompt for an output option.
ENTER MODEL NAME AND OP. CODE (C,CREATE A,APPEND) (6A1,1X,A1)
Type in a 6 character name, followed by C or A.
If A is entered the name should match that given before and the file created may be used to append to an existing
FEMVIEW database.
ENTER NAME OF OUTPUT FILE OR FIN (12A1)
Enter a unique name of up to 12 characters beginning with a letter. (The filename should be unique even though
operation Code A has been entered in the previous command since any existing output file with the same name
would be overwritten).
Enter FIN to exit from the FEMV option.
ENTER CURC FOR PLOTTING RESULTS ON CURRENT CONFIGURATION ELSE BLANKS
If the create option (C) has been entered for the operation code and CURC is entered for this prompt then the
coordinates written to the FEMVIEW neutral file will be the original coordinates plus the displacements for the
increment selected. The CURC option has to be selected if it is required to rotate any shell stresses/strains and/or
stress/strain resultants into a common axis system.
ENTER OUTPUT TYPE AND INCREMENT, ELSE END (A4,FREE)
Type in 4 character keyword for one of the FEMVIEW output types (see Table I.1) and the increment number
for output. Currently the data for one increment only may be processed.
Various prompts will appear depending on the output type selected. The prompts divide into two basic sets;
those dealing with primary nodal variables, ie DISP, VELO, ACCN, REAC and EIGN and the remainder which
are all element based variables, eg STRS and STRN.
I.3.1 Primary Nodal Variables
If any of the output types DISP,VELO,ACCN or REAC are selected then the displacements, velocities,
accelerations or reactions respectively are unskewed (if necessary) and copied directly to the output file. If
output type EIGN is selected then the following prompt will appear:
ENTER REQUIRED MODE NUMBER/GENERATOR OR ALL
Enter eigenvector mode number, list of modes optionally using topological format (see Section 4.2.3) or all
modes to be transferred. Examples are:
1
mode 1 only
1 3 5 7
modes 1, 3, 5 and 7
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-4
ASAS (Non-Linear) User Manual
(4) (1,2)
ALL
Appendix I
modes 1, 3, 5 and 7
all modes
I.3.2 Primary Element Based Variables
The primary element based variables are stresses and strains, stress and strain resultants (beams and shells only)
and stress point indicators. For most element types these variables are only stored as Gauss point quantities. If
element by element nodal values are required an extrapolation process has to be carried out. Some shell and
beam element results (e.g. Stresses) contain more than one surface. The surface number corresponds to the
sequence in which the integration points are numbered through a section. For shells, these are from 1 (bottom)
to NGZ (top) (see Appendix G). Note that this definition is opposite to the convention adopted by FEMVIEW
and thus care must be taken when displaying the TOP SURFACE and BOTTOM SURFACE results in
FEMVIEW. Additionally for shell elements there are a variety of options for rotating stresses into a common
axis system, extracting individual layer data from a non-linear material analysis and the computation and output
of subsidiary data such as failure indices for laminated composite structures. The various prompts which may be
encountered are as follows:
ENTER GAUS, NODE OR ELND FOR OUTPUT POSITION (A4)
Results may be output to the FEMVIEW neutral file in ‘Element at Gauss points’ format (enter GAUS), ‘Element
at Nodes’ format (enter ELND or NODE, both have the same effect).
I.3.2.1 Rotation of Shell Element Based Variables
If shell elements are being processed it is possible to instruct POSTNL to rotate stresses/strains and stress/strain
resultants into a common local axis system. The necessary data required to carry out these rotations is prompted
for with the following instructions. Full details of the theory behind the computations carried out are given in
Section I.77 of this Appendix.
ENTER ROTA IF ‘output type’ VALUES ARE TO BE ROTATED, ELSE BLANKS
If output type STRS,STRN,SRES or RESN have been selected the option to rotate the values is given.
ENTER RADI FOR RADIAL DEFINITION OF NEW LOCAL X DIRECTION, ELSE BLANKS
The values may be rotated into a common axis system where all element local x and y directions are parallel.
Alternatively, a radial axis system may be selected, by entering RADI, where all the element local x directions
point to a common central point.
ENTER GLOBAL COORDINATES OF POINT DEFINING NEW LOCAL X DIRECTION
The common local x direction for each element is parallel to a vector starting at the global origin (X=Y=Z=0.0)
and terminating at the point whose coordinates are prompted for here.
ENTER GLOBAL COORDINATES OF CENTRE POINT FOR RADIAL AXIS SYSTEM
If RADI is selected the user is required to enter the global X,Y,Z coordinates of the common central point.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-5
ASAS (Non-Linear) User Manual
Appendix I
ENTER GLOBAL COORDINATES OF THE REFERENCE POINT FOR THE CONTROL VECTOR
To ensure the top and bottom surface for each shell is correctly aligned the user is requested to input the
coordinates of a reference point. The control vector is constructed from this reference point to any integration
(Gauss) point. This control vector enters the element through the bottom surface and exits through the top
surface.
ENTER GROUP NUMBERS FOR WHICH VALUES ARE TO BE ROTATED (FREE)
As it may only be sensible to rotate values for certain groups of elements the choice of selecting only certain
groups is available. Enter ALL if all element groups are to be rotated.
INPUT FILENAME FOR FILE TO HOLD ROTATION ANGLES (12A1)
The calculation of the necessary rotations at each integration point can be time consuming, particularly for large
structures with many elements. To avoid repetition, various data is stored on a disc file. The user is asked to
provide the name of this file as, by default, it is not deleted on completion of the POSTNL session.
I.3.3 Secondary Element Based Variables
Various facilities exist within the FEMVIEW interface to calculate subsidiary data from the primary element
based variables.
I.3.3.1 Laminated Composite Shells
Two basic types of laminated composite shell analysis are available in ASAS-NL; elastic and ‘plastic’ or failure
analysis. Both types require the user to supply material and geometric property data defining the layup sequence
and the material properties of each layer.
For an elastic analysis, it is not necessary to continually monitor and/or update the change in stress for each
lamina. Hence, recovery of lamina stresses and strains and the calculation of failure indices (according to
several different theories) is carried out, on request, in POSTNL. These calculations are currently only available
in the FEMVIEW interface and are obtained by requesting output type LAMI. The LAMI option is only valid if
stress resultants (SRES) have been saved onto the porthole file. It should also be noted that output positions
other than GAUS are also not currently available. On entering GAUS the following prompt will be obtained:
ENTER USER LAYER NUMBER (0 IF NON-LAMI DATA, -1 IF ALL LAYERS)
Enter a layer number or -1 for all layers or 0 if non-laminate data are to be processed. With LAMI requested, a
0 user layer number means that no processing will be carried out.
For a laminated composite analysis employing a non-linear material failure law, information concerning the state
of stress and strain are available using the output types STRS and STRN in the usual manner. The same user
layer number prompt will appear on entering GAUS so that the user may request output at a particular layer or all
layers within the laminate. If an analysis contains both laminated and homogeneous shell elements, entering a 0
at this prompt will cause the program to process the results of homogeneous shell only. Note also that, in this
case, it is not possible to process both the laminated and homogeneous sets of results simultaneously.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-6
ASAS (Non-Linear) User Manual
Appendix I
Similarly, when there is a mixture of elastic and plastic shell elements in the same run, the user should use LAMI
to recover the lamina stresses/strains of the elastic elements and STRS/STRN to process the plastic elements
separately.
I.3.3.2 Surface and Global Failure Indices
The surface failure index, Fs, is a single value computed at each shell surface integration point and is defined as
follows;
No. of through-thickness integration points that have failed
Fs =
Total no. of through-thickness integration points
Note that this index is available for both homogeneous and laminated shells. For homogeneous or ‘plastic’
laminate analysis only a single value will be output at each surface integration point. For elastic laminate
analysis, ten surface failure indices, corresponding to the ten lamina failure indices computed for each lamina,
will be output.
To obtain the surface failure indices, specify output type SFAI. Again, this option is currently only available
with output position GAUS.
Global failure indices are for laminated shells only and are obtained by using output type GFAI with output
position GAUS. Up to five global failure indices are computed, the first being in-built (see Appendix B.5.2 for
details) and the remaining four being user-defined.
It should be noted that the SFAI and GFAI options are only valid if stress resultants (SRES) have been saved
onto the porthole file.
I.3.3.3 Laminated Composite Bricks
The calculations available for laminated bricks are very similar to those for laminated shells. In this case,
however, the lamina stresses and strains are computed in ASASNL and therefore it is not necessary to
distinguish between elastic and failure analysis.
The lamina failure indices can be obtained by requesting output type LAMI as before. The LAMI option is only
valid if stresses (STRS) have been saved onto the porthole file.
If only the lamina stresses or strains are required, these can be obtained using the output types STRS and STRN
in the usual manner.
The surface failure indices are obtained by specifying output type SFAI. Again, stresses (STRS) should be
saved onto the porthole file. Note that surface failure indices are only available for an elastic laminated brick
analysis.
Global failure indices are not available to laminated bricks as stress resultants are not calculated.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-7
Appendix I
ASAS (Non-Linear) User Manual
I.4 PATRAN Interface
The interface between ASAS-NL and PATRAN consists of the so-called PATRAN model file containing
coordinate and element topological data, and a set of neutral results files, one for each required output type (e.g.
STRS at increment 2). The model file is created by a PATRAN pre-processing run, or by specifying PATN with
the ASAS-NL OPTIONS command. The results files are created by POSTNL. They are in binary form but their
formatted contents are put to the command file ZZZMONIT by entering ECHO after an appropriate prompt.
After entering PATN for the PATRAN interface the program asks for the name of the output file which is to be
created. This must be unique to the output type it is to contain. The program then asks for the 4 character label
identifying the output type and the increment number. Valid type labels are given in Table I.2.
Integration point quantities cannot be handled by PATRAN and all such data is therefore extrapolated to nodes
and averaged across common elements. Principal quantities, if requested, are computed from extrapolated nodal
values and then averaged; equivalent values are computed from averaged nodal data.
Shell elements require each layer to be treated separately. The layer number corresponds to the sequence in
which the integration points are numbered through the shell thickness (1 to NGZ see Appendix -G). However
the mid surface can also be identified by the label 0 and top surface by the label 999.
Having written the selected output to the neutral file, the program returns with a further prompt for the name of
the output file for the next output type. To exit enter FIN.
The various prompts encountered using the PATN option are detailed below.
STRS
Element stress vectors
STRN
Element (total) strain vectors
ELAS
Element elastic strain vectors
INST
Element plastic strain vectors
CRSN
Element creep strain vectors
SRES
Element stress resultants (beams & shells only)
RESN
Element strain resultants (beams & shells only)
ISP
Element stress point indicators
EIGN
Eigen vectors
DISP
Displacement vectors
REAC
Reactions
TEMP
Element temperatures
Table I.2 Output Types for Patran
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-8
Appendix I
ASAS (Non-Linear) User Manual
4.1
ENTER NAME OF OUTPUT FILE OR FIN (12A1)
Give a unique name for the results file of up to 12 characters, or type in FIN to exit from the PATN option.
Next prompt 4.2.
4.2
ENTER ECHO FOR PATRAN O/P ECHOING ELSE BLANKS
Type in ECHO to cause all the Patran data to be echoed to ZZZMONIT, or press return.
4.3
ENTER O/P TYPE AND INCREMENT ELSE END (A4, FREE)
STRS
3.4, 3.5, (3.6, 3.7)
STRN
3.4, 3.5, (3.6, 3.7)
ELAS
3.4, 3.5, (3.6, 3.7)
INST
3.4, 3.5, (3.6, 3.7)
CRSN
3.4, 3.5, (3.6, 3.7)
SRES
3.4, 3.5, (3.6, 3.7)
RESN
3.4, 3.5, (3.6, 3.7)
ISP
3.4, 3.5, (3.6, 3.7)
EIGN
3.8
DISP
all disp/reac unskewed then transferred
REAC
3.1
TEMP
3.4, 3.5, (3.6, 3.7)
All return to prompt 4.1.
4.4
ENTER
PRINC
TO
CALCULATE
PRINCIPAL
QUANTITIES
FOR
2D
AND
SHELL
ELEMENTS, ELSE BLANKS
Type in PRINC or press return.
4.5
ENTER
EQUIV
TO
RECALCULATE
EQUIVALENT
QUANTITIES
AT
NODES,
ELSE
BLANKS
Enter EQUI for recalculation of equivalent quantities following nodal averaging.
Next prompt 4.6
Press return for no recalculation
4.6
ENTER YIELD FUNCTION TYPE (1 VON MISES, 2 TRESCA, 4 MOHR-COULOMB, 5
DRUCKER-PRAGER)
Enter number for yield function to be used. If 4 or 5, then prompt 4.7.
4.7
ENTER ANGLE OF FRICTION
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-9
ASAS (Non-Linear) User Manual
Appendix I
Enter angle in degrees.
4.8
ENTER REQUIRED MODE NUMBER
Enter mode number for the eigenvector to be transferred.
I.5 Printer Interface
Any of the data on the porthole can be selectively printed. In addition the following quantities are also available.
•
displacements, velocities, accelerations, reactions and/or eigenvectors in the global axis system
•
displacements, velocities, and/or accelerations at any, arbitrary, user defined point
•
nodal element quantities, obtained by extrapolation of integration point values
•
element quantities at any, arbitrary, user defined point
•
principal quantities at integration points
•
principal quantities at any, arbitrary, user defined point
•
principal quantities at nodes calculated from nodal quantities rather than by extrapolation of
integration point values
•
fracture mechanics processing (J, J*, C or C*) (see also I.88)
•
create nodal load data from reaction results
•
create prescribed displacement data from displacement results
•
create temperature load data from heat analysis results
•
create eigenvector perturbated coordinate data
All output requested is automatically printed to the monitor file ZZZMONIT. POSTNL prompts for the word
VIEW if, in addition, the data is to be displayed on the screen. The program then asks for the keyword PLOT if
data concerning stress/strain resultants for beams is to be output to a file.
The user is then asked to enter the output type and increment, or type END to exit from the printer interface.
Valid output types are given in Table I.3.
The output type labels are similar to those specified with the ASAS-NL POST command. Where displacements
are stored (DISP), as shown on the index, reactions are also stored. Similarly for stress resultants and strain
resultants. Any number of output types may be printed to the monitor file.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-10
ASAS (Non-Linear) User Manual
Appendix I
Nodal quantities (displacements, reactions and eigenvectors) can be transformed from any local skew systems to
the common global system if required.
Element quantities can be the original integration (Gauss) point quantities or the same quantities extrapolated to
the nodes. In either case they relate to the axis system chosen for the ASAS-NL calculation. Nodal principal
quantities (requested by entering PRIN at the appropriate prompt) are calculated from the nodal components
after extrapolation from the integration points. Element stress point indicators are always printed with any
element quantities.
Both displacements and element quantities may be requested to be output at any arbitrary user defined point.
STRS
Element stress vectors
STRN
Element (total) strain vectors
ELAS
Element elastic strain vectors
INST
Element plastic strain vectors
CRSN
Element creep strain vectors
SRES
Element stress resultants (beams & shells only)
RESN
Element strain resultants (beams & shells only)
ISP
Element stress point indicators
EIGN
Eigen vectors
DISP
Displacement vectors
VELO
Velocity vectors
ACCN
Acceleration vectors
REAC
Reactions
WORK
Sum of element work for each group
TEMP
Element temperatures
JAY
J integral
JAYS
J* integral
CEE
C integral
CEES
C* integral
HEAT
Create temperature load data from thermal results
Table I.3 Output Types for the Printer Interface
The various prompts encountered using the PRIN option are detailed below.
5.1
ENTER VIEW FOR SCREEN COPY ELSE BLANKS
Type in VIEW for data to be echoed to the screen as well as ZZZMONIT, or press return to continue.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-11
ASAS (Non-Linear) User Manual
5.2
Appendix I
ENTER ‘PLOT’ IF PLOT FILE IS REQUIRED FOR NODAL BEAM RESULTANTS ELSE
BLANKS
Type in PLOT to open a plot file, next prompt 5.3. Each data set written to the plot file contains the user element
number, node number, followed by beam resultants as given in Table I.6.
Press return to continue to 5.4.
5.3
INPUT C(CREATE)/A(APPEND) AND FILENAME FOR PLOT FILE (A1,1X,12A1)
ELSE BLANKS
Enter C or A and a filename or press return to continue to prompt 5.4. (C to create a new plotfile and A to
append to an existing one).
5.4
ENTER ‘PERT’ IF EIGENVECTOR COORDINATE PERTURBATION IS REQUIRED,
ELSE BLANKS
Enter PERT if the global nodal coordinates are to be recovered from the porthole file and scaled eigenvectors are
to be added to the coordinates subsequently.
5.5
ENTER O/P TYPE AND INCREMENT ELSE END (A4, FREE)
Enter an output type or END.
STRS
5.6, 5.7, (5.10.1, 5.10.2, 5.10.3), 5.8
STRN
5.6, 5.7, (5.10.1, 5.10.2, 5.10.3), 5.8
ELAS
5.6, 5.7, (5.10.1, 5.10.2, 5.10.3), 5.8
INST
5.6, 5.7, (5.10.1, 5.10.2, 5.10.3), 5.8
CRSN
5.6, 5.7, (5.10.1, 5.10.2, 5.10.3), 5.8
TEMP
5.6, 5.7, (5.10.1, 5.10.2, 5.10.3), 5.8
SRES
5.6, 5.7, (5.10.1, 5.10.2, 5.10.3, (5.10.4, 5.10.5)), 5.8
RESN
5.6, 5.7, (5.10.1, 5.10.2, 5.10.3), 5.8
DISP
5.9, 5.10, (5.10.1, 5.10.2, 5.10.3), 5.12, 5.14, (5.18)
VELO
5.9, 5.10, (5.10.1, 5.10.2, 5.10.3), 5.12
ACCN
5.9, 5.10, (5.10.1, 5.10.2, 5.10.3), 5.12
REAC
5.9, 5.10, 5.12, 5.15, (5.18)
EIGN
5.9, 5.10, (5.10.1, 5.10.2, 5.10.3), 5.11, 5.12, (5.17, 5.18,
5.19)
JAY
5.13
JAYS
5.13
CEE
5.13
CEES
5.13
HEAT
5.16, 5.18
WORK
END
All options return to 5.5 after printing.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-12
Appendix I
ASAS (Non-Linear) User Manual
5.6
ENTER PRINC TO CALCULATE PRINCIPAL QUANTITIES FOR 2D AND SHELL ELEMENTS,
ELSE BLANKS
Enter PRINC or press return if inapplicable.
5.7
ENTER GAUS OR NODE OR POIN FOR OUTPUT POSITION (A4)
Type in GAUS to output data at the integration points
Type in NODE to output data extrapolated to the nodes
Type in POIN if element values at a user defined point are required. For GAUS and NODE, the next prompt is
5.8. For POIN, the next prompt is 5.10.1
5.8
ENTER USER ELEMENT NUMBER(S)/GENERATOR (O TO FINISH) OR ALL
Type in either a list of 1 or more element numbers, use the free format generator (see Section 4.2.3) or ALL to
output data for all elements. The free format generator may only be used to generate up to 80 elements. Next
prompt is 5.5 after data has been transferred.
5.9
ENTER ‘GLOBAL’ IF VECTORS ARE TO BE SKEWED TO COMMON GLOBAL AXES
ELSE BLANKS FOR OUTPUT IN SKEW SYSTEMS
Enter GLOBAL or press return.
5.10
ENTER ‘POINT IF DISPLACEMENTS AT USER DEFINED POINT ARE REQUIRED,
ELSE BLANKS
Press return to continue to 5.12 (5.11 for output type EIGN). If POINT is entered, the following prompts are
made:
5.10.1
ENTER ELEMENT NUMBER WITHIN WHICH THE POINT LIES
Enter user element number (or system element number if no user element numbers specified).
5.10.2
ENTER ‘GLOB’ OR ‘CURV’ FOR INPUT OF GLOBAL OR CURVILINEAR
COORDINATES OF POINT
The position of the point within the element may be specified using global cartesian coordinates or in terms of
the element curvilinear coordinate system.
See Appendix -G for definitions of the element curvilinear
coordinate systems.
5.10.3
ENTER GLOBAL (CURVILINEAR) COORDINATES OF POINT
Sufficient coordinate values must be given to specify the point. One, two or three values will be required
depending on the element and the coordinate system specified. Next prompt is 5.5 for all output types except
EIGN and SRES. For output type EIGN, the next prompt is 5.11, after which the program returns to prompt 5.5.
If output type SRES has been specified and the current element is a shell element, the following prompt is made.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-13
ASAS (Non-Linear) User Manual
5.10.4
Appendix I
ENTER ‘TTVL’ IF THROUGH THICKNESS STRESSES ARE REQUIRED, ELSE BLANKS
Press return to continue to prompt 5.5. If TTVL is entered, the following prompt is made.
5.10.5
ENTER THROUGH THICKNESS COORDINATE (ZITA) AT POINT
The value entered for zita should be between +/- 1.0. Next prompt is 5.5.
5.11
ENTER REQUIRED MODE NUMBER
Enter a list of 1 or more mode numbers for this increment for which the eigenvector is to be printed.
5.12
ENTER NODE NO / GENERATOR OR ALL
Type in either a list of 1 or more node numbers, use the free format generator (see Section 4.2.3) or ALL to
output data for all nodes.
5.13
ENTER NAME OF CONTOUR DEFINITION FILE (12A1)
Enter the name of the contour definition file, up to 12 characters beginning with a letter. See Appendix I.88 for
format of this file.
5.14
ENTER PRES TO CONVERT DISPS TO LOADS, ELSE BLANKS
Enter PRES to create prescribed displacement data from the displacement results obtained or press return.
If PRES is entered, a DISP data block is created for all freedoms at all nodes selected except those which have a
displacement ‘exactly’ equal to zero. These freedoms are assumed to be suppressed. Also, PRESCRIB load
data is created with the non-zero displacements as prescribed values. All output is to a user defined text file.
Enter return to obtain normal printed output.
5.15
ENTER NODA TO CONVERT REACS TO LOADS, ELSE BLANKS
Enter NODA to create nodal load data from the reaction results obtained or press return.
If NODA is entered, all reactions at all nodes selected are converted into NODAL LO data except those
freedoms where the reactions are ’exactly‘ equal to zero which are ignored. All output is to a user defined text
file. Enter return to obtain normal printed output.
5.16
ENTER GROUP NO/GENERATOR OR ALL
Type in a list of group numbers, use the free format generator (see Section 4.2.3) or ALL to output data for all
groups.
5.17
ENTER ‘EIGV’ IF EIGENVECTOR IS TO BE ADDED TO COORDINATES
If PERT has been entered in response to prompt 5.4, the above prompt will be displayed. Press return if the
current requested eigenvector is to be ignored, in which case the next prompt is 5.5. Entering EIGV causes the
prompts for a coordinate data filename and scaling factor for the perturbation to be displayed.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-14
ASAS (Non-Linear) User Manual
5.18
Appendix I
ENTER 4 CHARACTER IDENTIFIER FOR .AAA FILE
Type in a 4 character identifier for the load data file to be created. In the above prompt, AAA will appear as
LOD for nodal load data, as DIS for prescribed displacement data, as TEM for temperature load data, and as
COR for perturbated coordinate data. The name of each output file produced is XXXXnnnn.AAA, where
XXXX is the file identifier, nnnn is the increment number. It should be noted that two files are created for
prescribed displacement data. The .DIS file contains the DISP data while the .PRD file contains the PRESCRIB
data.
5.19
ENTER NODE, DOF (1, 2 OR 3) AND ABSOLUTE VALUE
Before adding the eigenvector to the current global nodal coordinates, the eigenvector is scaled such that the
specified degree of freedom (translational only) at the specified node will have a magnitude equal to the absolute
value specified. This prompt is repeated for each requested mode and then each requested increment.
I.6 Time Histories
Tabulated time histories of up to 10 selected quantities can be extracted and listed. They are formatted in a form
suitable for importing into a spreadsheet program for plotting.
Quantities are identified by 4 character labels. Valid identifiers are listed in Table I.4.
After entering TIME to obtain the Time history interface the user is prompted for VIEW if screen copy is
required and a filename if the output is to be plotted. The program next asks for a list of increments (or ALL for
all increments on the porthole file) for which quantities are to be obtained, followed by the number of time
histories (or identifiers). Each identifier is then requested in turn.
Nodal quantities (displacements, velocities, accelerations, reactions and eigenvectors) require the freedom to be
identified by an integer label 1-10. This requires users to know the number of degrees of freedom at the node.
The sequence follows that given in the ASAS-NL output and is given in Table I..
Element quantities (e.g. stresses, strains) are normally integration point quantities as calculated in ASAS-NL (i.e.
no principal and/or nodal values can be selected). They are identified by their element number, integration point
number (see Appendix -G) and the component number. The latter corresponds to the column number of the
printed output and varies from element to element. Details are given in Table I..
Output types DISP, VELO, ACCN, REAC, DMAX, RSUM, PSUM have an option to input rotation and
translation factors A and B such that the value output is A*value + B.
Both displacements and element quantities may be requested to be output at any arbitrary user defined point.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-15
Appendix I
ASAS (Non-Linear) User Manual
DISP+
Nodal displacements
VELO+
Nodal velocities
ACCN+
Nodal accelerations
STRS
Element stresses (or fluxes for field element)
STRN
Element (total) strains (or field gradients for field element)
INST
Element plastic strains
ELAS
Element elastic strains
SRES
Element stress resultants (beams and shells only)
RESN
Element strain resultants ( ”
CRSN
Element creep strains
ISP
Element stress point indicators
TEMP
Element temperatures
NULL
Null vector
TMSN
Element (total) mechanical strains
REAC+
Nodal reactions
ADD
Form new identifier by adding any 3 quantities already selected
SUB
Form new identifier by subtracting any 2 quantities from a third, all of which have
already been selected
DMAX*+
Maximum displacement
VMAX*+
Maximum velocity
AMAX*+
Maximum acceleration
RSUM*+
Reaction sum
PSUM*+
Sum of reactions associated with prescribed displacements
ITER*
Accumulated iterations to date
ISTF*
Accumulated stiffness reformations to date
ILIN*
Accumulated line searches to date
NTER*
No. of iterations in current increment
NSTF*
No. of stiffness reformations in current increment
NLIN*
No. of line searches in current increment
”
”
” )
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-16
Appendix I
ASAS (Non-Linear) User Manual
* These quantities are saved using the identifier ‘SUMR’ with the POST command in the Preliminary data.
+
With option to input rotation and translation factors.
Table I.4 Valid Identifiers for Time Histories
Component number
1
2
3
4
5
6
7
8
9
10
Freedom
X
Y
Z
RX
RY
RZ
WRR
EZZ
R
T
Table I.5 Nodal Component Numbers
Notes
1.
For axisymmetric solid analysis only. Component number 1 may also be used to represent freedom R.
2.
For field analysis only. Component number 1 may also be used to represent freedom T.
Component Number
Element
Type
1
2
3
4
5
6
7
8
9
10
11
12
PN1
PN2
PM1
PM2
QUM4
QUM8
XX
YY
XY
ZZ
EQ
-
P1
P2
RR
ZZ
HH
RZ
EQ
P1
P2
XX
YY
ZZ
XY
YZ
ZX
EQ
TCS6
XX
YY
XY
XZ
YZ
EQ
P1
P2
TCS8
NXX
NYY
NXY
MXX
MYY
MXY
SXY
SXZ
XX
XY
XZ
EQ
STF4
FXX
TXX
MYY
MZZ
SXY
SXZ
FLA2
XX
EQ
GAP2
RG23
RG24
XX
YY
GAPX
RGX3
RGX4
RR
ZZ
SST4
RR
RM
TRM3
TRM6
QUX4
QUX8
TRX3
TRX6
BRK6
BRK8
BR15
BR20
LB15
LB20
QUS4
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-17
Appendix I
ASAS (Non-Linear) User Manual
Component Number
Element
Type
WST4
1
2
3
FRR
SRS
SRT
4
MSS
5
6
MTT
MWP
7
TSV
8
TWP
9
10
11
12
10
11
12
TRQ
Table I.6 Element Quantity Component Numbers
Component Number
Element
Type
1
2
XREL
VREL
BM2D
FXX
SQY
MZZ
BM3D
FXX
SQY
SQZ
TXX
MYY
MZZ
LSP3
N1
M1
N2
M2
N3
M3
XX
YY
RR
ZZ
XX
YY
SPR1
3
4
5
6
7
8
9
SPR2
JP
JTOT
LSP6
QMT4
QMT8
TMT3
TMT6
QXT4
QXT8
TXT3
TMT6
BRT6
BRT8
ZZ
BT15
BT20
FAT2
XX
FAT3
Table I.6 Element Quantity Component Numbers (continued)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-18
Appendix I
ASAS (Non-Linear) User Manual
The various prompts encountered using the TIME option are detailed below.
6.1
ENTER VIEW FOR SCREEN COPY ELSE BLANKS
Type in VIEW for plotting data to be echoed to the screen, or press return.
6.2
ENTER C(CREATE)/A(APPEND) AND FILENAME FOR PLOT FILE (A1,1X,12A1),
ELSE BLANKS
Enter C and a filename to create a new plotfile.
Enter A and an existing filename to append to a plotfile.
Press return to continue without opening a plotfile.
6.3
INPUT INCREMENT NOS/GENERATOR, OR ALL
Type in a list of increments to be plotted, use the free format generator (see Section 4.2.3) or ALL to select all
increments on the interface file.
6.4
ALLOWABLE IDENTIFIERS
DISP STRS STRN INST ELAS SRES RESN CRSN ISP
REAC ADD
SUB
TEMP NULL TMSN
DMAX RSUM PSUM ITER ISTF ILIN NTER NSTF NLIN
INPUT NO OF IDENTIFIERS MAX = 10
Enter the number of identifiers to be plotted.
6.5
INPUT IDENTIFIER NO ‘n’ (OR NULL)
Input identifier n
DISP
6.6, 6.7, 6.7.1, (6.7.2, 6.7.3, 6.7.4, 6.7.5), 6.8, (6.9)
VELO
6.6, 6.7, 6.7.1, (6.7.2, 6.7.3, 6.7.4, 6.7.5), 6.8, (6.9)
ACCN
6.6, 6.7, 6.7.1, (6.7.2, 6.7.3, 6.7.4, 6.7.5), 6.8, (6.9)
REAC
6.6, 6.7, 6.8, (6.9)
STRS
6.13, (6.14, 6.15, 6.16, (6.17, 6.18)), (6.10)
STRN
6.13, (6.14, 6.15, 6.16, (6.17, 6.18)), (6.10)
INST
6.13, (6.14, 6.15, 6.16, (6.17, 6.18)), (6.10)
ELAS
6.13, (6.14, 6.15, 6.16, (6.17, 6.18)), (6.10)
SRES
6.13, (6.14, 6.15, 6.16, (6.17, 6.18)), (6.10)
RESN
6.13, (6.14, 6.15, 6.16, (6.17, 6.18)), (6.10)
CRSN
6.13, (6.14, 6.15, 6.16, (6.17, 6.18)), (6.10)
ISP
NOT CURRENTLY AVAILABLE
TEMP
NULL
No further prompt
TMSN
NOT CURRENTLY AVAILABLE
ADD
6.11
SUB
6.11
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-19
Appendix I
ASAS (Non-Linear) User Manual
DMAX
6.12, 6.7, (6.9)
BMAX
6.12, 6.7, (6.9)
AMAX
6.12, 6.7, (6.9)
RSUM
6.12, 6.7, (6.9)
PSUM
6.12, 6.7, (6.9)
ITER
No further prompt
ISTF
No further prompt
ILIN
No further prompt
NTER
No further prompt
NSTF
No further prompt
NLIN
No further prompt
All return to 6.5 until the number of identifiers requested have been input. The program then exits from the
TIME option and returns to the main menu.
6.6
INPUT ‘GLOBAL’ FOR VECTORS TO BE UNSKEWED, ELSE BLANKS
Type in GLOBAL or press return for output in skew systems.
6.7
INPUT ‘FACT’ IF ROTATION AND TRANSLATION FACTORS TO BE INPUT, ELSE
BLANKS
Type in FACT or press return.
6.7.1
INPUT ‘POINT’ IF DISPLACEMENTS AT USER DEFINED POINT ARE REQUIRED,
ELSE BLANKS
Press return to continue to 6.8. If POINT is entered, the following prompts are made:
6.7.2
ENTER ELEMENT NUMBER WITHIN WHICH THE POINT LIES
Enter user element number (or system element number if no user element numbers specified).
6.7.3
ENTER
‘GLOB’
OR
‘CURV’
FOR
INPUT
OF
GLOBAL
OR
CURVILINEAR
COORDINATES OF POINT
The position of the point within the element may be specified using global cartesian coordinates or in terms of
the element curvilinear coordinate system.
See Appendix -G for definitions of the element curvilinear
coordinate systems.
6.7.4
ENTER GLOBAL (CURVILINEAR) COORDINATE OF POINT
Sufficient coordinate values must be given to specify the point. One, two or three values will be required
depending on the element and the coordinate system specified.
6.7.5
INPUT COMPONENT NO. (1-7)
Type in the component number (depends on the nodal freedoms, see Table I..
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-20
ASAS (Non-Linear) User Manual
6.8
Appendix I
INPUT COMPONENT NO (1-7), NODE NO
Type in the component no (depends on nodal freedoms, see Table I.) and the node number e.g. 1,2.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-21
Appendix I
ASAS (Non-Linear) User Manual
6.9
INPUT ROTATION FACTOR A AND TRANSLATION FACTOR B
Input two values A,B such that value output will be
A*VALUE+B
6.10
INPUT COMPONENT NO., USER EL. NO., INTEGRATION POINT NO.
Enter the component number (depends on element type, see Table I.7), user element number and the integration
point number for which data is to be output.
6.11
INPUT 3 IDENTIFIER NO.S (OR ZEROS)
Input three numbers of columns A,B,C such that for ADD, VALUE = A+B+C and for SUB, VALUE = A-B-C
6.12
INPUT FREEDOM NAME (A3)
Enter name of freedom for which maximum values are to be plotted.
6.13
INPUT ‘POINT’ IF VALUES AT A USER DEFINED POINT ARE REQUIRED, ELSE
BLANKS
Press return to continue to 6.10. If POINT is entered, the following prompts are made:
6.14
ENTER ELEMENT NUMBER WITHIN WHICH THE POINT LIES
Enter user element number (or system element number if no user element numbers specified).
6.15
ENTER ‘GLOB’ OR ‘CURV’ FOR INPUT OF GLOBAL OR CURVLINEAR COORDINATES
OF POINT
The position of the point within the element may be specified using global cartesian coordinates or in terms of
the element curvilinear coordinate system.
See Appendix -G for definitions of the element curvilinear
coordinate systems.
6.16
ENTER GLOBAL (CURVILINEAR) COORDINATES OF POINT
Sufficient coordinate values must be given to specify the point. One, two or three values will be required
depending on the element and the coordinate system specified. Next prompt is 6.7.5 for all output types except
SRES. If output type SRES has been specified and the current element is a shell element, the following prompt
is made.
6.17
ENTER ‘TTVL’ IF THROUGH THICKNESS STRESSES ARE REQUIRED, ELSE BLANKS
Press return to continue to prompt 6.5. If TTVL is entered, the following prompt is made.
6.18
ENTER THROUGH THICKNESS COORDINATE (ZITA) AT POINT
The value entered for zita should be between +/- 1.0. Next prompt is 6.5.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-22
Appendix I
ASAS (Non-Linear) User Manual
I.7 Rotation of Element Based Variables for Shells
I.7.1 Introduction
Generally curved finite elements are most effectively formulated using a reference frame that follows the
naturally curved shape of the element. Stresses and strains (and stress resultants for structural elements) are
calculated with respect to this reference frame at the integration points for each element. As this reference frame
changes orientation (with respect to some other fixed reference frame) not just from element to element but from
integration point to integration point, so the directions of the stresses and strain vary. A graphical representation
of stresses and strains may be achieved in many ways but one of the most popular is to draw a contour map
where each contour line is the locus of points of equal stress or strain. As stresses and strains are vectors, such
contour maps are only meaningful if the stresses and strains are oriented in a consistent manner over the area of
interest. For simple geometries, this can often be achieved by judicious meshing and ordering of the element
topology. In general, however, a facility is needed to transform the stresses and strains into a predefined
direction before contouring is carried out.
This section details the procedures implemented into POSTNL, to
achieve these transformations.
I.7.2 Restrictions
The procedures outlined here are applicable to membrane, axisymmetric solid and shell elements. In the current
version of POSTNL, these procedures are only implemented for the shell elements TCS6 and TCS8 with the
default surface integration rule.
I.7.3 The Plane Stress Transformation
The transformation of interest here is the rotation about a surface normal of the stresses in each layer of a shell.
In the thick shell elements these are the plane stress components σxx, σyy and τxy and the two orthogonal
transverse shear stresses τyz and τzx. The rotation of a general state of plane stress through an angle θ is a
standard exercise in mechanics (reference 0) and the stresses in the new (primed) system are given by:
σ′xx
=
(cos2 θ) σxx + (sin2θ) σyy + (2 sin θ cos θ) τxy
σ′yy
=
(sin2 θ) σxx + (cos2θ) σyy - (2 sin θ cos θ) τxy
τ′xy
=
(sin θ cos θ) (σyy - σxx) + (cos2 θ - sin2 θ) τxy
(1)
The transverse shear components transform according to the usual transformation rule for vectors, that is:
τ′yz
=
(cos θ) τyz
+
(sin θ) τzx
τ′zx
=
(-sin θ) τyz
+
(cos θ) τzx
(2)
Exactly the same transformations may be employed for the corresponding strain components except that the
definition of the in-plane shear strain requires a factor of one half to be applied to this term.
Similarly for the stress resultants the in-plane forces and in-plane shear and the bending moments and twist may
all be transformed using the same relationships. Also, the transverse shear forces will transform like the
transverse shear stresses.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-23
Appendix I
ASAS (Non-Linear) User Manual
I.7.4 Determination of the Rotational Angle, θ
The direction into which the stresses are to be rotated is defined by the user. There are several ways in which
this direction may be specified and these will be dealt with in the following section. For the purposes of deriving
a suitable algorithm to compute the angle of rotation, θ, it is assumed that a unit vector in the required direction,
p̂ ( î , ĵ , k̂ ) where î , ĵ , and k̂ are unit vectors in the global (fixed) reference frame, has been defined. The
stress state before rotation is given with respect to a local orthogonal cartesian system x,y,z (see Figure I.7.1.)
with unit vectors
x̂ ( î , ĵ , k̂ ), ŷ ( î , ĵ , k̂ ), ẑ ( î , ĵ , k̂ ) respectively.
Figure I.7.1. Local axis system
p̂ on the x,y plane, q, is given by
q = x x̂ + y ŷ
The projection of
where
x and y are determined from the dot products
x = p̂.x̂
y = p̂.ŷ
A further dot product between a unit vector in the direction of q,
q̂ , and the local x direction unit vector x̂ ,
yields the angle θ, i.e.
cos θ = q̂.x̂
where
q̂ = q / |q|
I.7.5 User Definition of New Local Axes Direction
Two different methods of defining the local axes directions are available to the user of POSTNL. The first, and
simplest, requires the user to define the coordinates of a point P, with respect to the global reference frame.
Taking P as the terminal point of a vector starting at the origin of the global reference frame and denoting it as
P( î , ĵ , k̂ ) then a unit vector in the direction of P,
p̂ , is given by
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-24
ASAS (Non-Linear) User Manual
Appendix I
p̂ = P / |P|
Using this method, the local x′ axis direction is constant for all elements in the groups specified (see
FigureI.7.2.) i.e. all parallel to
p̂ and in the direction of p̂ .
Figure I.7.2. Rotated directions in global axis system
The second method requires the user to define the coordinates of a point, P, with respect to the global reference
frame which acts as the centre point for a radial axis system. Using this method, the local x′ axis direction points
from the global position at which the stresses are defined, i.e. the integration point, towards the point P.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-25
ASAS (Non-Linear) User Manual
Appendix I
Denoting the position vector of the integration point G as g (see Figure I.7.3.) and the position vector of the point
P as P then a vector, p, from the integration point G to the point P is given simply as
p=P-g
and a unit vector in this direction,
p̂ , is obtained by normalisation in the usual manner.
Figure I.7.3. Rotated directions with radial option
This method is invoked by responding RADI to the required prompt when using POSTNL.
I.7.6 User Definition of Element Top and Bottom Surfaces
The definition of the top and bottom surface of 2-D finite elements such as membranes, shells and axisymmetric
solids is associated with the node order in which the element topology is specified in the analysis. In general,
adjacent elements in a mesh may have a mismatch of surfaces, i.e. the top surface of one element is coincident
with the bottom surface of an adjacent element. Thus when post-processing the element results, a consistent
convention must be adopted if meaningful plotting of, for example, stress contours is to be carried out.
In POSTNL, the specification of the top surface of an element is achieved by prompting the user to define the
global coordinates of a reference point, R, which is used to define a control vector, d (see Figure I.7.4.). This
control vector starts at R and terminates at the integration point, G, at which results are being processed. The
convention adopted is that the control vector enters the element at the bottom surface and exits through the top
surface. Computationally, this procedure is very simple. Knowing the global coordinates of G (interpolated from
the element nodal coordinates using the element shape functions).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-26
Appendix I
ASAS (Non-Linear) User Manual
Z,k̂
ẑ
d̂
Y, ĵ
θ
ŷ
G
G
g
x̂
d
r
R
X,î
Figure I.7.4. Construction of Control Vector for Element Surface Definition
the vector d is determined as
d=g-r
d̂ , is obtained by normalisation in the usual manner. The angle θ between the
vector d̂ and the unit normal to the shell surface, ẑ , is easily calculated from the definition of the dot product,
and a unit vector in this direction,
i.e.
cos θ =
d̂.ẑ
If 1 ≥ cos θ ≥ 0, then the top surface defined in the analysis is assumed to coincide with that specified by the user
in POSTNL. However, if cos θ < 0, it is assumed that the surfaces need to be reversed or flipped.
I.7.7 References
I.1
Timoshenko, S.P. and Gere, J.M., Mechanics of Materials, van Nostran Reinhold, 1973.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-27
ASAS (Non-Linear) User Manual
Appendix I
I.8 Fracture Mechanics Processing
I.8.1 Introduction
The facility to request the calculation of the fracture mechanics parameters J and J* and creep fracture
parameters C and C* is available in POSTNL.
To enable fracture mechanics processing, results for displacements (DISP), stresses (STRS), total strains
(STRN), elastic strains (ELAS) and, if PLAS, inelastic strains (INST) must be saved on the post-processing file.
For C and C*, creep strains (CRSN) must also be saved. In addition, all the results for C and C* must be saved
for a neighbouring state as well as the required increment in order to enable the calculation of rate quantities.
The facility is invoked via the PRINT option. When the user is prompted for output type and increment, the
output type should be either:
JAY
for J integral calculation
JAYS
for J* integral calculation
CEE
for C integral calculation
CEES
for C* integral calculation
Having made the appropriate response, the user is then prompted for the name of the contour definition file.
This file must be created before the POSTNL run. The contour definition file is a formatted ASCII file, details
of which are given in Section I.8.4.
Once the contour definition file name has been entered, POSTNL echoes the data to the screen and then
computes and prints out J and/or J* or C and/or C* as requested. From this point on the process may be repeated
for further contour definitions.
I.8.2 Restrictions
The fracture parameter calculations in POSTNL are currently subject to a number of restrictions. These are:
(a)
Elements on and within the contour must be axisymmetric solid elements or membrane elements in 2-D.
Surface flaws on shells can be analysed using the line-spring elements.
(b)
Elements on and within the contour must not be subject to body forces (including centrifugal loading).
(c)
The analysis must be carried out using global stresses, i.e. stress calculation for the elements must be
related to the global axis system. Note that this is the default for the axisymmetric solid elements.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-28
ASAS (Non-Linear) User Manual
Appendix I
I.8.3 Notes on the use of Fracture Parameters
It is assumed that the user is fully conversant with the theory and application of the J(C) and J*(C*) integrals.
The following offers some practical guidance to their use within the finite element method.
For linear elastic fracture mechanics, J(C) is path independent and should thus give the same value regardless of
the contour specified. This is only approximately true with a finite element discretisation. However, providing
the variation of stresses and strains within the elements on the contour is not too severe (as they are at the crack
tip), the value of J(C) should not vary by more than a few percent. The further the contour is from the crack tip,
the more path independent J(C) should be in a finite element discretisation. It is also advisable to avoid distorted
elements (which in themselves may cause a sharp variation in the stress field) or unstressed elements which, in
effect, increase the length of the contour path but add nothing to the strain energy.
For elasto-plastic fracture mechanics, J(C) is path independent only if the entire contour passes through an
elastic region. It is for this reason that J*(C*) was introduced and this integral should be independent of the path
and area of integration. It is well known that including the elements surrounding the crack-tip in the evaluation
of J*(C*) introduces significant errors and therefore these elements should be excluded from the area of
integration.
I.8.4 Format of Contour Definition File
The contour definition file contains the information required to define the contour for the J(C) integral
calculation and the elements to be included in the J*(C*) integral calculation. It also contains the angle of
orientation of the crack with respect to the global axis directions. The format of the file is as follows:
THETAD (EN)
NODS
NODCNT(1) NODCNT(2)........
............................
...........NODCNT(NODS)
NELS
NELCNT(1)
NELCNT(2)........
...........NODCNT(NELS)
THETAD is the angle the crack x1 axis direction makes with the global R (or X) direction and is specified in
degrees. EN is only required for C and C* calculation and is the Creep law exponent, n, in the expression
εcr = B σ n .
NODS is the number of nodes defining the contour. Element mid-side nodes should not be
included. NODCNT(I) are the node numbers lying on the contour, from one end to the other end. Note that the
contour integration is always performed in an anti-clockwise fashion inside the program. NELS is the number of
elements lying on the contour for J(C) and on and within the contour for J*(C*). NELCNT(I) are the user
element numbers.
I.8.5 Example
The following example demonstrates the form of the data required.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-29
ASAS (Non-Linear) User Manual
Appendix I
Figure I.8. shows the section of interest in an axisymmetric model with the crack angle and contour path. Figure
I.9. shows the finite element mesh used with node and element numbers. The contour data definition file for J
integral calculation would be as follows:
220.0
19
251 217 183 181 179 177
175 173 207 241 292 326
328 330 332 334 336 302 268
14
49 50 51 52 53 57 61
65 69 73 74 75 76 77
If J* also was to be calculated, the above data file could be used with the addition of 2 elements, 60 and 68.
Note that the elements surrounding the crack tip have been excluded from this J* calculation.
Figure I.8. Crack Angle and Contour Path
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-30
ASAS (Non-Linear) User Manual
Appendix I
Figure I.9. Finite Element Mesh Node and Element Numbers
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page I-31
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix I
Page I-32
Appendix J
ASAS (Non-Linear) User Manual
Appendix - J
Creep Analysis
J.1 Overview
The following data are required in addition to the normal description of a model when conducting a creep
analysis.
1.
A creep analysis is initiated by the four character directive CREP with the PROBLEM/TITLE command
in the Preliminary data. The job type should also be set to TRAN (time dependent analysis) with the JOB
command. Currently only one material non-linearity can be modelled in any one restart stage, i.e. any
instantaneous (‘plasticity’) effects must be isolated from time dependent (‘creep’) effects and treated in a
separate restart.
2.
For creep analysis the ‘pseudo’ times used for the ASAS-NL incremental solution procedure become real
times, representing the period for which creep behaviour is to be calculated. The solution must therefore
be controlled by SOLVE and RESTART commands with lists of real times at which solutions are to be
calculated. In addition to the times at which results are desired it is likely that a number of intermediate
times should also be requested in order to achieve acceptable accuracy and stability. This can be done
either manually (simply by defining a list of solution times) or automatically by the program (see Section
J.4).
3.
Three solution methods are available for creep and are explained in Section J.2. They are set as follows:
Explicit:
This is the default and so no additional information is
necessary.
Implicit, elastic stiffness:
Specify a non-zero implicit weighting factor VALPHA with
the TEMPORAL command.
Implicit, updated stiffness:
Specify a non-zero implicit weighting factor VALPHA with
the TEMPORAL command, and set OPTION VISC.
4.
If automatic selection of timesteps (see Section J.4) is required then OPTION AUCR should be set. A
sufficient number of timestep controlling parameters should also be selected to achieve the desired
control. If AUCR is not set the program defaults to manual timestep selection and only solves at the
times specified with the SOLVE or RESTART command.
5.
The creep material behaviour is defined by specifying a creep law for each material type in the creep
material properties data block, see Section 5.2.4.3. For any particular material type there is a choice of
four laws in-built to the program, NORT, LAW2, LAW3, LAW4. Alternatively a creep law can be
defined directly in a user supplied subroutine, directives USE1, USE2, USE3, USE4, USE5 on the creep
material-properties data block. Details of the various creep material models are given in Appendix B.4.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page J-1
Appendix J
ASAS (Non-Linear) User Manual
J.2 Creep Solution Methods
The three creep time integration methods currently available in the program are:
(i)
Explicit
This is also known as the Euler Forward Method or Forward Difference Method. The incremental
equivalent creep strains are calculated simply from the equation
ε c = ε(i)
c ∆tc
Where the superscript (i) denotes that the equivalent creep rate ε c is calculated using the values of stress,
strain, temperature and time at the start of the timestep, and
∆ t is the time increment.
No iteration is necessary for this calculation because it is based entirely on known quantities at the start of
the timestep.
(ii)
Implicit, elastic stiffness
For this method the equivalent incremental creep strains are calculated from
(i+1)
∆t
ε c = (1 - VALPHA) ε(i)
c ∆ t+ (VALPHA) ε c
Where the superscript (i+1) denotes that the creep rate is calculated using the values of stress, strain,
temperature and time at the end of the timestep.
Stresses and strains are not known a priori for the end of the timestep and so iteration is necessary over
the increment, each time using the latest estimate of these quantities, until no change is observed in
consecutive iterations.
If VALPHA is set to 1.0 this method is known as the Euler Backward Method or Backward Difference
Method. If VALPHA is 0.5 this is known as the Central Difference Method. If VALPHA is zero it
defaults to the Explicit method.
(iii)
Implicit, updated stiffness
This method uses the implicit equation in (ii) above except that the solution is estimated without iteration,
by calculating a tangential material stiffness each increment. This effectively approximates the change to
the creep rate from changing stress over the increment but does not account for any such changes due to
changing total creep strain, temperature or time.
This method is derived as a Viscoplastic solution procedure in reference J.1.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page J-2
ASAS (Non-Linear) User Manual
Appendix J
Currently the creep model is limited to the von Mises potential function and associative flow rule when
extending the above uniaxial creep descriptions to multiple axes. The term ‘equivalent’ therefore always denotes
von Mises equivalent quantities.
Note that for all three methods there is no need for the user to specify any UPDATE information if creep is the
only non-linearity being considered. The first two methods use the elastic material stiffness exclusively and the
third method automatically UPDATES the stiffness on all iterations. If large displacements are considered
concurrently with creep then additional updating should be requested as required, see the UPDATE command.
Note also that because creep analysis is a timestepping procedure modelling transient behaviour through real
time, solution is always by the SOLVE method with pseudo times representing real times. The special solution
(SOLU) methods are therefore not available for creep.
J.3 Convergence of Creep Solutions
Although the type of Norm and the tolerance value specified with the CONVERGENCE command can in
general be specified freely for creep analysis, control of the Reference Variable is limited as follows.
(i)
Explicit method
The Residual Forces (RESF) Variable remains the default as with other types of analysis. No residual
forces are present for creep increments when other non-linearities are not involved and so in such cases
no iteration will take place. The DISP variable may be selected but STRN and STRS may not.
(ii)
Implicit Method, elastic stiffness
Two convergence checks are made:
(a)
Convergence of the creep rate calculations is automatically monitored by a STRS check
with EUCN. The convergence tolerance is 0.001.
(b)
The RESF (or alternatively DISP) check described in (i) above is also made and again the
residual forces will always be zero unless other non-linearities are involved. STRS and
STRN may not be selected with the CONVERGENCE command.
(iii)
Implicit Method, updated stiffness
Convergence checking is the same as for the Explicit Method.
J.4 Automatic Timestepping
The purpose of the automatic control of timestepping is to enable the program to choose timestep lengths
according to user supplied criteria so as to achieve consistent accuracy over the period of solution. The basic
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page J-3
Appendix J
ASAS (Non-Linear) User Manual
philosophy is that the program solves at all times specified with the SOLVE or RESTART commands and
additionally at as many intermediate times as is necessary for the given criteria. The automatic timestep facility
operates independently of the selection of creep solution method.
Note that although solutions at intermediate times follow identical theory to those at SOLVE or RESTART
times, they are hidden to the user with the exception of a brief summary of each step. Thus OUTPUT, POST,
SAVE, RESTART etc. commands may only refer to SOLVE or RESTART times. If ‘ALL’ is specified on such
a command then all times specified with the SOLVE or RESTART command will be inferred (but no
intermediate times).
The automatic timestepping facility is controlled by the following OPTION and TEMPORAL identifiers:
Controlling Options using the OPTION command
AUCR
Autocreep.
This activates the automatic control facility (Default: manual control,
solutions only at SOLVE or RESTART times).
FCRO
Full Creep Output. A half page performance summary is printed for each automatically
selected timestep (Default: a two line summary is printed).
Controlling parameters using the TEMPORAL command
Any number of these parameters may be set to control the timestep length. After each solution the next solution
time will be chosen from the shortest time implied by all of the parameters, or the next SOLVE or RESTART
time; whichever is the sooner.
DCSTMX
Maximum change of creep strain. In each timestep the maximum equivalent change of
creep strain for all integration points is recorded. If this quantity for the previous step
(step size t(i)) is denoted MAX then the new timestep length t(i+1) will be:
∆ t (i+1) = ∆ t (i) .
DCESMX
DCSTMX
MAX
Maximum relative change of creep strain. The same method of control as for DCSTMX
is used but in this case the control quantity is the ratio of equivalent incremental creep
strain to current equivalent elastic strain.
DSIGMX
Maximum relative change of stress. The same method of control as for DCSTMX is
used but in this case the control quantity is the ratio of equivalent change of stress to
current equivalent stress.
FINCMX
Maximum ratio of new timestep length to previous timestep length.
TINCMX
Maximum timestep length.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page J-4
ASAS (Non-Linear) User Manual
Appendix J
Supplementary parameters
FIRSTP
First timestep length. Specifies the first solution time in a run. If omitted the first
solution will be at the first time given with the SOLVE or RESTART command.
TINCMN
Minimum acceptable timestep length. If the controlling parameters imply a timestep
length less than TINCMN then the solution will be stopped.
MXINCS
Maximum number of timesteps in a run. If this number is exceeded in any run then the
solution will be stopped.
J.5 Example Preliminary Data
The following two examples indicate additional Preliminary data used when analysing a model for creep
behaviour.
(i)
Explicit integration; Manual control (solutions at SOLVE times only); No large displacement effects.
JOB TRAN
TITL CREP * ....
SOLV ..........
(ii)
Implicit integration; Weighting factor = 0.7; Updated stiffness method; Automatic timestep control; First
intermediate solution at 10.0 time units; Timesteps to limit incremental creep strain to half of elastic
strain; Results could be printed (or post-processed or saved for further restarts) at times 100.0, 300.0
and/or 1000.0; No large displacement effects.
Note - this example assumes that information is available from a previous analysis for a restart from time
5.0.
JOB TRAN ....
TITL CREP * ....
REST 5.0 100.0 300.0 1000.0
TEMP VALPHA 0.7 FIRSTP 5.0 DCESMX 0.5
OPTI AUCR VISC
J.6 Recommendations for Creep Analysis
The choice of method and parameters for conducting a creep analysis depends strongly on the characteristics of
the problem. It is therefore not possible to propose fixed rules. However the following generalisations may be
useful.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page J-5
ASAS (Non-Linear) User Manual
(i)
Appendix J
The accuracy of solution is sensitive to timestep sizes and great caution should be exercised in their
selection. In the limit of diminishing timestep size, all three solution methods will converge on the same
results. These results will be correct within the limitations of the material definition.
(ii)
If accuracy of solution is lost through excessive timestep length it should be assumed (in general) that the
solution will not recover subsequently, even if the step length is reduced.
(iii)
The implicit method with updated stiffness is much more tolerant of long timesteps than the two other
methods (by an order of magnitude or more for a given accuracy) provided that the only creep rate
variable which changes during the step is stress (i.e. no hardening, no temperature change). This method
is therefore normally to be preferred for such situations.
For rapid changes in temperature loading or hardening the implicit method with elastic stiffness takes best
account of changes during the step. However the convergence of iterations when using this method can
be poor and in general the use of the explicit method with short steps is therefore to be preferred for these
problems.
(iv)
The choice of value for the implicit weighting factor (VALPHA) has influence on the results in both of
the implicit methods. (Note that convergence of iterations with the implicit elastic stiffness method is not
convergence to a ‘correct’ solution, but only signifies satisfaction of the weighted creep strain equation in
Section J.2.) A value between 0.5 and 0.8 is recommended.
(v)
Given the necessity for consistent accuracy throughout the solution, the use of automatic control of
timesteps is strongly recommended. The values of control parameters depend very much on the problem
being considered but as a rough guide the new user is advised to start by limiting creep strains to the same
order of magnitude as elastic strains for the implicit updated stiffness method and an order of magnitude
lower for the two other methods.
J.7 References
J.1
Hinton, E. and Owen, D.R.J., ‘Finite Elements in Plasticity’, Pineridge Press, 1981.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page J-6
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix J
Page J-7
ASAS (Non-Linear) User Manual
Appendix - K
K.1
Appendix K
Transient Dynamics Analysis
Overview
The following are particular information concerning the run control of a transient dynamic analysis.
(i)
A transient analysis is initiated by setting the job type to TRAN with the JOB command.
(ii)
For transient analysis, the ‘pseudo’ times used in ASAS-NL become real times. The times at which
solutions are attempted can be specified manually or automatically determined by the program. When the
SOLV/REST command is specified, solutions will be obtained at times explicitly prescribed by the user
as in a static analysis. If a constant timestep is used throughout an analysis, an automatic time generation
facility TGEN with the SOLV/REST command is available which can significantly reduce the data
preparation work.
procedure.
Alternatively, an analysis can be performed using the automatic timestepping
This is invoked by setting directive DOMFRQ or MAXFRQ with the SOLU/SREST
command. Further details about the adaptive timestepping schemes are given in Section K.3.
(iii)
The time integration algorithm developed for transient dynamics analysis is an element partitioned
implicit-explicit scheme. By default, all element groups are implicit. Groups can be made explicit by
specifying directive EXPL with the GROU/PROB command. It should, however, be noted that the
definitions of implicit-explicit groups cannot be altered during any restart analysis.
(iv)
Rayleigh damping is assumed in which the damping matrix C is given by:
C = αmM+αkKL
where M is the mass matrix, KL is the linear stiffness matrix, and αm and αk are mass and stiffness
damping factors, respectively, that are specified as material properties.
The factors αm and αk are usually chosen to give correct damping at two frequencies. For a specified
damping factor ξ (i.e. ratio of actual damping to critical) at a frequency ω, then
α

ξ = 12  m + α kω 
 ω

Typically, for structural materials, the value of ξ is in the range 0.01 to 0.07. The two frequencies selected
should cover all the important response modes. Thus, one value is normally taken at the fundamental
mode, while the other is taken more arbitrarily at some higher frequency mode.
(v)
Any non-zero initial displacements and velocities should be specified in data block INIT. Initial loadings
can be given using the load function facility. When any of the above initial conditions is specified,
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page K-1
Appendix K
ASAS (Non-Linear) User Manual
solution at time 0.0 must be performed in order to compute the consistent acceleration vector to start the
time integration.
(vi)
In transient analysis, it is often necessary to predict the response of structures subjected to some known
velocity or acceleration time histories. To facilitate this, the user can use the data block VELO and
ACCN to enter prescribed velocities or accelerations at any specified freedoms. However, there is a
restriction that mixed prescribed types are not allowed in the same analysis. It should also be noted that
any non-zero prescribed value at time 0.0 will lead to erroneous results unless the governing equation of
motion is satisfied.
K.2
Time Integration Algorithm
The time integration algorithm in ASAS-NL is based on the implicit Bossak’s method, Ref K.1, and this is given
by the following equations.
(1 - α ) Ma n+1 + α M a n + N(d n+1 , vn+1) = Fn+1
d n+1 = d n + ∆ t vn +
K.2.1
∆ t2
[(1 - 2 β ) a n + 2 β a n+1]
2
K.2.2
vn+1 = vn + ∆ t [(1 - γ ) a n + γ a n+1]
K.2.3
where dn, vn and an are known displacements, velocities and accelerations, respectively, at time tn and dn+1, vn+1
and an+1 are the corresponding unknowns at time tn+1 which are obtained from solutions of equations K.2.1 to
K.2.3; M is the mass matrix; N is the internal force vector; Fn+1 is the external force vector at time tn+1; ∆t is the
timestep. The time integration parameters α, β,and γ determine the stability and accuracy characteristics of the
algorithm and it has been shown that unconditional stability, second-order accuracy and maximal high frequency
dissipation are achieved if
α≤0
;
γ=
1
-α
2
;
1
4
β = (1 - α )2
K.2.4
In ASAS-NL, the default settings of these parameters are α=0, γ=0.5, and β=0.25 which correspond to the
trapezoidal rule without any numerical damping. These defaults can be reset by specifying TALPHA (α),
TBETA (β) or TGAMMA (γ) with the TEMP command. If only TALPHA is given, the values of β and γ will be
computed according to equations K.2.4.
The explicit scheme is constructed from similar governing equations but with the an+1 terms dropped in the
expressions for displacements and velocities when solving equation K.2.1. Using a lumped mass matrix, the
solution of this equation becomes trivial and no matrix inversion is required. It should, however, be noted that
the explicit scheme is only conditionally stable and the timestep size is limited by the stability limit.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page K-2
ASAS (Non-Linear) User Manual
Appendix K
Two different methods are available to define the predictor at the beginning of a new time step. The default
scheme assumes that the predictor acceleration is zero and this works well for linear problems. The alternative
predictor is constructed by assuming that the predictor displacement is the same as the displacement at the end of
the previous time step. This is recommended for non-linear analysis since the convergence is usually faster. The
alternative predictor may be selected by specifying IPDICT 2 with the TEMP command. Note, however, that
this scheme will break down when β=0.0 and the default scheme must be used in this case. In addition, the
alternative predictor is not applicable to explicit time integration algorithms.
K.3
Automatic Timestepping
The purpose of the automatic timestepping procedures is to enable the program to determine the timestep sizes in
a manner which will achieve better computational efficiency while maintaining a consistent level of accuracy
over the solution period. Schemes based on the control of current dominant frequency and current maximum
apparent frequency are available and their definitions are as follows:
(i)
Dominant Frequency (Ref K.2, K.3)
The dominant frequency is estimated at each converged timestep using the displacement and internal
force increments by
ωn =
2
∆ dT K ∆ d
∆ dT ∆ F
≈
∆ dT M ∆ d ∆ dT M ∆ d
where ∆d is the incremental displacement vector, K is the current stiffness matrix, M is the mass matrix
and
∆ F is the incremental internal force vector due to the stiffness terms.
The dominant frequency obtained above is dictated by spurious mass or stiffness terms when artificially
low or high masses or stiffnesses are used. This adverse effect can be avoided by eliminating all
displacement components in ∆d which have an extremely small or large apparent frequency compared to
the dominant frequency. If we define the modified incremental displacement vector as ∆d*, the modified
dominant frequency is given by:
ω 2n =
(ii)
∆ d* T ∆ F
∆ d* TM ∆ d
Maximum Apparent Frequency (Ref K.4, K.5)
The apparent frequency of the ith freedom is defined as
ω i2 =
M∆a
∆F
≈
M∆d i M∆d i
where ∆a is the incremental acceleration vector and all other quantities have their previously defined
meanings.
The maximum apparent frequency is the highest frequency value among all the apparent frequencies.
Thus,
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page K-3
ASAS (Non-Linear) User Manual
Appendix K
ω 2max = max{ω i2}
When directive DOMFRQ is specified with the SOLU command, the automatic timestepping procedure
will be activated using
ω 2n
as the controlling factor and this is applicable to implicit time integrations.
Alternatively, the maximum apparent frequency adaptive scheme will be activated by specifying
MAXFRQ with SOLU and this is suitable for explicit time integrations. Note that because the nature of
implicit and explicit schemes are quite different, the timestepping control procedure for one type of time
integration scheme should not be applied to the other.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page K-4
Appendix K
ASAS (Non-Linear) User Manual
Upon determining ω from the response (ω can be
2
2
ω 2n
or
ω 2max
depending on the control parameter
selected), the desired timestep for the next step is
∆ t* = FP x
2π
ω
where FP is the desired timestep factor which is expressed as a fraction of the controlling period.
However, the continuous adjustment of the step size at every timestep is not effective because it requires
excessively frequent matrix decompositions even for linear problems. To overcome this deficiency and
to account for the effect of non-linearities on the solution convergence, the timestep adjustment is made
according to the following formula instead:
where
ITER is the number of iterations for convergence in the nth step and ITERD is the user specified desired
number of iterations as in a static analysis. The function f(ξ) which determines the timestep adjustment is
shown diagrammatically as follows:
The form of f(ξ) indicates that there is a range of ξ (between ξlo and ξhi) in which the timestep will remain
unchanged. This avoids the need for making small adjustments. In addition, fmax defines the maximum
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page K-5
ASAS (Non-Linear) User Manual
Appendix K
timestep ratio which is used to limit the size of increase between steps and ξrj defines the lower limit on ξ
for accepting the current solution as a good one. It is often desirable that a time adaptive scheme is
conservative on making timestep increases in order to maintain better numerical stability. In this respect,
any increase in timestep will only be made after the increasing signals have been recorded for KSIGNL
consecutive steps, where KSIGNL is a user input parameter.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page K-6
Appendix K
ASAS (Non-Linear) User Manual
The current solution is rejected when convergence cannot be obtained or ξ is less than ξrj. The analysis
will then be restarted from the previous converged solution with a reduction in step size. The reduction
factor, RF, will depend on the reason for rejecting the solution and is given by
(i)
RF=ξrj
for ξ<ξrj
(ii)
RF=STEPRF
for convergence failure
where STEPRF has the same meaning of the auto-recovery factor in static analyses. The timestep used
for restart is thus given by
∆ t n = RF* ∆ t n
Similar to the static load adaptive scheme, the number of possible restarts within a step is governed by the
parameter MXAUTO.
There are a number of control parameters for automatic timestepping and these are listed below together
with their default values:
Parameter
Default
TINCMN
Minimum timestep
0.0
TINCMX
Maximum timestep
1.0x1015
FINCMX
Maximum timestep ratio
10.0
TFACLO
Lower limit of plateau in f(ξ)
0.75
TFACHI
Upper limit of plateau in f(ξ)
1.35
TFACRJ
Limit on ξ below which the current solution will be rejected
0.10
FRAPRD
Desired fraction of the characteristic period for the timestep
0.05
KSIGNL
The number of consecutive timestep increasing signals required
before the increase is made
2
MXAUTO
Limit for number of restarts in any step
3
STEPRF
Step reduction factor after convergence failure
0.5
To a certain extent, the performance of the automatic timestepping scheme will depend on the setting of
the control parameters. Although it is not possible to propose fixed rules because of the possible different
characteristics of each new problem, the following general guidelines may be useful.
(i)
A conservative initial timestep is generally preferred as this provides greater accuracy at the start of the
time integration process.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page K-7
ASAS (Non-Linear) User Manual
(ii)
Appendix K
In non-linear analysis, it is advisable to set the maximum timestep ratio, FINCMX, to a realistic value, for
example, 2.0. It helps to improve the numerical stability as too drastic a change in step size may cause
divergence due to the presence of non-linearities. The improvement in numerical stability can also be
achieved by increasing the value of KSIGNL.
(iii)
The default setting of FRAPRD is adequate for linear analysis. This number may need to be decreased
(ie more steps per characteristic period) for highly non-linear problems.
(iv)
When the loading is changing very rapidly (eg in earthquake problems), it may be necessary to limit the
timestep by an upper value TINCMX in order to secure that the load intensity at sufficiently close
intervals is sampled.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page K-8
ASAS (Non-Linear) User Manual
Appendix K
K.4
References
K.1
Wood, W.L., Bossak, M. and Zienkiewicz, O.C., ‘An Alpha Modification of Newmark’s Method,’
International Journal for Numerical Methods in Engineering, Vol. 15, 1980, pp1562-1566.
K.2
Bergan, P.G. and Mollestad, E., ‘An Automatic Time-stepping Algorithm for Dynamic Problems,’
Comp. Meth. Appl. Mech. Eng., Vol. 49, 1985, pp299-318.
K.3
Lee, S.H. and Hsieh, S.S., ‘Expedient Implicit Integration with Adaptive Time Stepping Algorithm for
Non-linear Transient Analysis,’ Comp. Meth. Appl. Mech. Eng, Vol. 81, 1990, pp151-172.
K.4
Park, K.C. and Underwood, P.G., ‘A Variable-Step Central Difference Method for Structural
Dynamics Analysis - Part 1. Theoretical Aspects,’ Comp. Meth. Appl. Mech. Eng., Vol. 22, 1980,
pp241-258.
K.5
Underwood, P.G. and Park, K.C., ‘A Variable-Step Central Difference Method for Structural
Dynamics Analysis - Part 2. Implementation and Performance Evaluation,’ Comp. Meth. Appl. Mech.
Eng., Vol 23, 1980, pp259-279.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page K-9
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix K
Page K-10
ASAS (Non-Linear) User Manual
Appendix - L
Appendix L
References
1.
‘ASAS-NL - Theory and Implementation’ Atkins Research and Development, December, 1981.
2.
Ahmad, S., Irons, B.M., Zienkiewicz, O.C. ‘Analysis of Thick and Thin Shell Structures by Curved
Elements’. Int. J. Num. Meth. Eng., Vol.2, pp.413-451 (1970).
3.
Bathe, K.J. ‘Finite Element Procedures in Engineering Analysis’. Prentice-Hall, 1982.
4.
Bushnell, D. ‘A Strategy for the Solution of Problems Involving Large Deflections, Plasticity and
Creep’. Int. J. Num. Meth. Eng., Vol. 11, pp.683-708 (1977).
5.
Bushnell, D. ‘Stress, Stability and Vibration of Complex Branched Shells of Revolution’. Comput.
Struct., Vol.4, pp.399-435 (1974).
6.
Cook, Robert D. ‘Concepts and Application of Finite Element Analysis’. John Wiley, 1974.
7.
Crisfield, M.A. ‘A Fast Incremental/Iterative Solution Procedure that Handles Snap-Through’. Comput.
Struct., Vol. 13, pp.55-62 (1981).
8.
Crisfield, M.A. ‘Ivanov’s Yield Criterion for Thin Plates and Shells Using the Finite Element Method’.
TRRL, Rep. 919, D.o.E., 1979.
9.
Gallagher, R.H. ‘Finite Element Analysis Fundamentals’. Prentice Hall, 1972.
10.
Gierlinski, J.T. and Graves Smith, T.R. ‘A Variable Load Iteration Procedure for Thin-walled
Structures’. Comput. Struct., Vol.21, pp.1085-1094 (1985).
11.
Hill, R. ‘The Mathematical Theory of Plasticity’. Clarendon Press, 1980.
12.
Hinton E. and Owen D.R.J. ‘Finite Elements in Plasticity’. Pineridge Press, 1981.
13.
Irons, B. et al. ‘Analysis of Thick and Thin Shell Structures by Curved Finite Elements’. Int. J. Num.
Meth. Eng., Vol. 2, 1970.
14.
Johnson, W. and Mellor, P.B. ‘Engineering Plasticity’. Van Nostrand, 1978.
15.
Malvern, L.E. ‘Introduction to the Mechanics of Continuous Medium’. Prentice-Hall, 1969.
16.
Owen, D.R.J. and Gomez, C.M.B. ‘An Appraisal of Numerical Solution Techniques for Elasto-Plastic
and Elasto-Viscoplastic Material Problems’. 6th International Conference SMIRT, Vol. M M3/1.
17.
Powell, G. and Simons, J. ‘Improved Iteration Strategy for Non-linear Structures’. Int. J. Num. Meth.
Eng., Vol.17, pp.1455-1467 (1981).
18.
Przemieniecki, J.S. ‘Theory of Matrix Structural Analysis’. McGraw-Hill, 1968.
19.
Riks, E. ‘An Incremental Approach to the Solution of Snapping and Buckling Problems’. Int. J. Solids
Struct., Vol. 15, pp 529-551 (1979).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page L-1
Appendix L
ASAS (Non-Linear) User Manual
20.
Robotnov, Y.N. ‘Creep Problems in Structural Mechanics’. North-Holland, 1969.
21.
Smith, I.M. ‘Programming the Finite Element Method with Applications to Geomechanics’. John Wiley,
1982.
22.
Stolarski, H. and Belytschko, T. ‘Membrane Locking and Reduced Integration of Curved Elements’. J.
Appl. Mech., Vol.49, pp.172-176 (1982).
23.
Washizu, K. ‘Variational Methods in Elasticity and Plasticity’. Pergamon Press, 1975 (2nd Edition).
24.
Waszczyszyn, Z. ‘Numerical Problems of Non-linear Stability Analysis of Elastic Structures’. Comput.
Struct., Vol.17, pp.13-24 (1983).
25.
Zienkiewicz, O.C. ‘The Finite Element Method in Engineering Science’.
Edition).
26.
Zienkiewicz, O.C., Too, J., Taylor, R.L. ‘Reduced Integration Techniques in General Analysis of Plates
and Shells’. Int. J. Num. Meth. Eng., Vol.3, pp. 235-256 (1971).
27.
O.R.N.L. - ‘Guidelines and Procedures for Design of Nuclear System Components at Elevated
Temperature’ - RDT Standard F9-5T Division of Reactor Research and Development, United States
Atomic Energy Commission, September, 1974.
28.
Chang, S.C. and Chen, J.J. ‘Effectiveness of Linear Bifurcation Analysis for Predicting the Non-linear
McGraw-Hill, 1977 (3rd
Stability Limits of Structures’. Int. J. Num. Meth. Eng., Vol. 23, pp. 831-846 (1986).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page L-2
ASAS (Non-Linear) User Manual
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Appendix L
Page L-3
ASAS (Non-Linear) User Manual
Appendix - M
M.1
Appendix M - Wave Loading
Wave Loading On Offshore Jacket Structures
Introduction
The wave loading capability in ASAS-NL is incorporated from the program WAVE within the ASASOFFSHORE system. This facility enables the calculation of wave, wind and current loading on fixed offshore
structures where the structural members are of relatively small section size compared with the wave length.
Only TUBE and BM3D elements will have environmental loads generated and all other element types will be
ignored.
For natural frequency or transient dynamics analysis, additional inertia due to various hydrodynamic effects is
also included. This is similar to the facility offered by the program MASS.
In addition to the description of the structure, the calculation of wave loading requires environmental data, which
defines the position of the jacket relative to the mean water-level and sea-bed together with wave height and
direction, current profile and direction, wind direction and velocity. The description also defines the presence of
flooded or sealed members, the presence of marine growth, and the drag and inertia force coefficients for the
loaded members.
A number of different wave theories have been implemented for the user to select from. These include the linear
(Airy), Solitary (Cnoidal), Stokes Vth order and stream function wave theories. For conditions not covered by
these theories, a facility exists for supplying the wave kinematics as a grid of velocities and accelerations,
together with a free surface profile. Facilities are also provided to permit wave loading to be computed within
the requirements of the API codes of practice (RP2A-WSD and RP2A-LRFD) including the effects of apparent
wave period, non-linear current stretching, current blockage factor and wave kinematics factor. Extreme wave
kinetics may be developed using the Shell New Wave model, which utilises statistical analysis of sea state
information. Wave loading may also be generated from a random sea state. For details of various wave theories
and the wave force calculation, please refer to the WAVE user manual.
In this Appendix, the descriptions of the valid wave load commands in ASAS-NL are presented. These
commands are a subset of the commands available in WAVE and generally have identical meanings (except
where noted).
M.2
Water Axes
Water axes Xw, Yw and Zw are defined separately to the structure Global Axes. The position of the water axes
relative to the global axes is specified in the ‘WAVE LOAD’ data. All of the ‘hydrodynamic’ quantities such as
wave direction, current direction, mean water level, etc. are then defined relative to the Water Axes.
The water axis Zw is always vertical and positive upwards.The water axis Xw lies in a plane parallel to the global
plane with the water axis Yw on the positive side of the XY plane, Yw is positive in the direction of positive Y
(see also the GRAV and MOVE commands in Appendix M.6).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-1
ASAS (Non-Linear) User Manual
Appendix M - Wave Loading
This facility enables the global structure axes to be defined to ‘best fit’ the structure but, in general, for most
offshore structures one axis is nearly always vertical and by convention this is usually denoted as the Global Z
axis. For this situation the directions of the global and water axes are related simply by supplying ‘-g’ in the Z
field of the wave loading GRAVity data command (where g is the gravitational acceleration in consistent units).
The facility of being able to vary the position of the structure relative to the water is used to the full in the
LAUNCH program which investigates the behaviour of the structure as it is launched from a barge, tilted and
installed.
M.3
Wave Theories
M.3.1 Conventional wave theories
For the wave loading, a suitable wave theory is used to calculate the water particle kinematics. The following
wave theories are currently available in ASAS-NL:
•
Linear Wave Theory (Airy)
•
Solitary Wave Theory (Cnoidal)
•
Stokes 5th Order Theory
•
Stream Function Theory
For guidance on selection of the appropriate wave theory, reference should be made to Figure M.1.
For conditions not covered by the above wave theories, a facility exists for supplying the wave kinematics in the
form of a grid of velocities and accelerations, together with a free surface profile. The program utilises linear
interpolation for determining kinematic values at locations between the grid positions. See Section M.6.13 GRID
Wave Data for further details.
M.3.2 Shell New Wave
The Shell NewWave wave model is incorporated into WAVE as an alternative to the conventional deterministic
wave theories described in Section NO TAG. The NewWave wave model was developed by Shell Research
(Reference NO TAG) in order to produce a more realistic description of the physical processes which occur
under extreme design waves in real seas, something which cannot be accurately described by traditional
deterministic wave theories. NewWave is not appropriate for harmonic analyses.
In the NewWave model, the water particle kinematics are generated from a wave spectrum using linear theory.
It uses a statistically-based superposition of linear wavelets to define the wave profile and associated kinematics
representing the most likely maximum condition of a real sea. The unique features of the theory are illustrated in
Figure 2.1 below. This figure shows that the wave crest is significantly higher than the neighbouring troughs,
which is consistent with observations of extreme waves.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-2
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
By definition the NewWave model is dispersive (or evolving) in that the crest height varies with time. In order
that analyses may be undertaken in a similar mode to that employed in deterministic wave studies, the wave may
be ‘frozen’ and stepped through the structure in the same way that conventional wave theories are processed.
Key features of the NewWave model in WAVE are:
•
Delta stretching of wave kinematics under the crest
•
Current blockage may be included using the BLOC command
•
Wave spreading for nearly uni-directional seas may be selected using the WPAR command
•
Doppler shift effects may be incorporated to account for wave/current interaction using the APIW
option
•
Both evolving and non-evolving waves are facilitated
•
Morison force coefficients may be specified as a function of the characteristic amplitude to tube
diameter ratio using the AMPL table definition
M 6.0
5.0
4.0
3.0
2.0
1.0
0.0
-1.0
-2.0
-3.0
-500.0
-400.0
-300.0
-200.0
-100.0
0.0
100.0
200.0
300.0
400.0
500.0
Distance in wave direction
PSMZ wave surface elevation - Shell NewWave - EVOLVING
•
Facilities to tune the solution method, where appropriate, using the WPAR command
Figure 2.1 NewWave Surface Profile
M.3.3 Irregular Wave
The irregular wave model provides a facility to analyse loading that takes into full account the randomness of the
sea state.
In the irregular wave model implemented, the wave particle kinematics are assumed to be generated from a wave
spectrum using linear theory. The wave spectrum can be defined in one of the three forms: JONSWAP, PiersonMoskowitz or user defined.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-3
ASAS (Non-Linear) User Manual
Appendix M - Wave Loading
The irregular wave is created by adding together the parameters (wave height, velocity and acceleration) of a
number of regular Airy wavelets with random phases and with amplitudes that correspond to the required
spectrum. The default number of wavelets is 50 and this may be re-specified using the WPAR command,
subject to an upper limit of 1000.
The wavelet phases are generated by a random number generator. The initial seed (default 1) for this process
may be modified using the WPAR command, which will enable a different set of random phases to be generated.
On a subsequent run, the same initial seed will generate the same sequence of random phases again.
Delta stretching of kinematics as implemented in the Shell New Wave model is also available in irregular wave.
Figure M.1 The Range of Validity of Various Wave Theories
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-4
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Notes
1.
None of these theories is theoretically correct at the breaking limit.
2.
Wave theories intended for limiting height waves should be referenced for waves higher than 0.9Hb when
stream function theory may underestimate the kinematics.
3.
Stream function theory is satisfactory for wave loading calculations over the remaining range of regular
waves. The suggested order of stream function is shown above but should be checked by comparison with
the results from a higher order solution.
M.4
Wave load data format
The wave load data generally assigns additional properties to elements, or groups of elements, which are
specifically required for the load generation. The data syntax is similar to that employed for the structural data
but consists of individual command lines, each of which assigns the additional parameters to the element(s). The
typical syntax of a command line is as follows:
KEYWORD
ELEM
elem
GROU
group
PROP
prop
real
ALL
Once a command has been defined, the value(s) specified remain assigned to the appropriate element(s) until
modified by a subsequent command. Basic data, such as drag and mass coefficients, need only to be supplied
once within the data set to remain constant throughout the analysis (unless required to be overridden).
The data values may be assigned to all elements using the keyword ALL or to specific elements using the
keywords ELEM, PROP or GROU followed by a list of user element numbers, geometric property numbers or
element group numbers. The list may be continued onto subsequent lines using the special symbol : (see Section
4.1.3).
The list may be abbreviated using the keyword TO in the form i TO j to create a list of all values between i and j
inclusive.
Not all the element, property or group numbers defined need to exist in the structure. Only those elements in the
list which correspond to elements in the structure will be included.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-5
ASAS (Non-Linear) User Manual
M.5
Appendix M - Wave Loading
WAVE LOAD Data
Many of the commands described in this section are optional and merely change default values within the
program. Once a default value has been changed, by the input of the appropriate command, it remains at the
new value until altered again. A list of the WAVE LOAD commands valid for ASAS-NL is given in Table M.1.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-6
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Command
Meaning
Comments
AMAS
Additional mass on element
Default - none
BLOC
Current blockage factors
Optional for use with API codes (use APIW option)
BUOY
Buoyancy
Default - none
CURR
Current from any direction
DRAG
Drag coefficients
Default - 0.0, 0.7, 0.7
ELEV
Water elevation
Mandatory
END
End of all wave load data
Mandatory
EXEC
Execute
Optional. Generally not required
FREE
Free flooding
Default - none
GRAV
Gravity components
Mandatory
GRID
Grid wave kinematics
User defined waves
GROW
Marine growth
Default - none
HYDR
Hydrodynamic dimensions
Optional
KC
KC dependent drag and mass
coefficients
Default - none
KINE
Wave kinematics factor
Optional for use with API codes (use APIW option)
LFUN
Wave load function
Optional. Default is no scaling
MASS
Inertia coefficients
Default - 0.0, 2.0, 2.0
MOVE
Water axes
Default - coincident with jacket axes
NANG
Number of angle steps
Optional for use with RENL and KC tables. Default
-8
NOBO
No buoyancy
Overrides BUOY command
NOFR
No free flooding
Overrides FREE command
NOLO
No loads
Overrides loading commands. Should be specified
after all loading commands
NOSW
No self-weight
Overrides SLWT command
NOWI
No wind load
Overrides WIND command
NOWL
No wave load
Overrides WAVE command
OFFS
Member offsets
Default - none
OUTP
Print control
Default - jacket totals only
PCUR
Any current
PEXT
External pressure for buoyancy
Default - pressure computed from sea water density
and elevation including wave action effect
PHAS
Phase
Default - 0.0
PRIN
Element printing
Default - none
RENL
Reynolds dependent drag and mass
coefficients
Default - none
Table M.1 Command words and their defaults for WAVE
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-7
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Command
Meaning
Comments
SLWT
Self-weight
Default - none
SPEC
Seastate spectrum definition
Mandatory for irregular wave or New Wave
SPRE
Wave spreading power
Optional for use with API codes (use APIW option)
TIDE
Current in wave direction
TOLS
Tolerance command
Default 0.1, 0.0
UNIT
Define new units
Optional
VAXS
Define orientations of
hydrodynamic axes
Default - water axes
VISC
Kinematic viscosity
Must be defined if RENL command used
VPOS
Define reference point for
hydrodynamic data
Default - origin of water axes
WAVE
Wave data
Must not precede ELEV command
WIND
Wind data
Default - none
WPAR
Wave parameters
XMAS
Extra mass/unit length
ZONE
Define zones for DRAG, MASS
and GROW command
Default - none
Table M.1 Command words and their defaults for WAVE (continued)
M.6
Description of the Wave Load Data Block
M.6.1 WAVE LOAD Data
WAVE LOA
data
END
Parameters
WAVE LOA : compulsory keyword to denote start of the wave data
data
: wave load data
END
: compulsory keyword to denote end of the wave data
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-8
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Notes
1.
Wave load data should not be defined more than once in the entire load check. The loading specified will
be applied to all load sets.
2.
The wave loading generated can be scaled, but using command LFUN only.
3.
Arc-length type SOLU procedure can be used but wave load must be attached to the proportional load
function using LFUN.
4.
If modification of wave environment is required during an analysis, this can be achieved by restarting
with modified wave data supplied.
M.6.2 AMAS Command
This facility enables non-structural mass such as stiffening rings, anodes, etc. to be included. Extra mass is input
as a value per element.
AMAS
ELEM
elem
GROU
group
PROP
prop
mass
ALL
Parameters
AMAS
: keyword
mass
: extra mass per element. (Real)
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-9
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Notes
1.
Extra mass may be specified per unit length per element using the XMAS command.
2.
Masses are not cumulative. Subsequent AMAS definitions for a particular element will overwrite
previous values.
3.
XMAS may be specified in addition to AMAS for a given element, in which case the XMAS mass and
the AMAS mass are cumulative.
M.6.3 BEAM Element Command
The BEAM command is replaced by the HYDR command.
M.6.4 Current BLOCKAGE Factor Command
The BLOC command specifies a user defined current blockage factor for use within the API codes of practice.
The factor can be varied at different heights on the structure.
BLOC
FACTOR
factor
( zmin
zmax )
Parameters
BLOC
: keyword
FACTOR : keyword to define that a user defined current blockage is to be supplied
factor
: current blockage factor. (Real)
zmin
: minimum height on structure (in water axes) to which this blockage factor applies. (Real)
zmax
: maximum height on structure (in water axes) to which this blockage factor applies. (Real)
Notes
(a)
Several BLOC commands can be supplied to vary the blockage factor at different heights on the
structure.
(b)
If zmin and zmax are omitted, the blockage factor is applied between the seabed and still water level.
(c)
A default value of 1.0 is used for any region of the structure not covered by a user defined factor.
(d)
BLOC commands are cumulative and a table is built up as each command is read. To reinitialise the table
use the RESEt command.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-10
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
(e)
For a fatigue analysis API requires that a factor of 1.0 be used.
(f)
For a factor not within the range 0.7 ≤ factor ≤ 1.0, a warning will be issued but the user defined value
will be used.
(g)
This command will only be utilised when used in conjunction with the APIW option.
Example
BLOC
1.0
.
EXEC
.
RESE 3
BLOC
BLOC
0.9 0.0 10.0
0.95 10.0 15.0
BLOC
0.97 15.0 20.0
M.6.5 BUOYANCY Command
The BUOY command specifies those members for which buoyancy loads are to be calculated. The elements
may be filled, either wholly or partially, with an internal fluid either by specifying the density and proportion of
flooding or, where the members are free flooding, using the FREE command (see Note 4 below). The command
is optional and no buoyancy is calculated if omitted.
BUOY
density
flood
ELEM
elem
GROU
group
PROP
prop
(elev )
ALL
Parameters
BUOY
: keyword
density
: mass density of internal fluid. (Real)
flood
: proportion of flooding of internal fluid. (Real)
elev
: elevation used for computing internal pressure. (Real) If elev Zb, the sea bed level, internal
pressure is computed assuming fluid pressure to elevation elev. If elev <Zb, internal pressure is
computed to the elevation of the water surface vertically above the point in question.
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-11
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Notes
1.
The weight of any internal fluid is automatically included in the buoyancy calculation.
2.
Buoyancy forces are calculated for members below the sea bed. For members above the water surface
only the weight of internal fluid is computed if elev is omitted.
3.
The proportion of flooding varies between 0.0 for no flooding and 1.0 for full flooding.
4.
If the member is free flooded (FREE) the internal fluid details (density and flood) should be omitted
otherwise the mass of the internal fluid may be duplicated.
5.
The buoyancy calculations are based on the outer diameter of the members including any marine growth
which may be present.
6.
There are two methods of applying the buoyancy forces to a member. The choice is governed by the
BRIG option. See also Section NO TAG.
7.
Internal pressure due to internal fluid is only included for the BRIG option.
8.
If elev is omitted in both the BUOY and FREE commands, internal pressure will be ignored. If elev is
specified more than once for an element, the last specification will be assumed.
M.6.6 CURRENT Command
The CURR command specifies a predetermined current profile in a given direction.
CURR
iprofile
v el-s
v el-b
elev
dir
Parameters
CURR
: keyword
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-12
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
iprofile
: profile type integer
1
linear profile
2
exponential profile
vel-s
: current velocity at still water level. (Real)
vel-b
: current velocity at sea bed. (Real)
elev
: elevation relative to water axis at which current becomes constant. (Real)
dir
: direction of current relative to water axis system. (Real)
Notes
1.
The current may vary either linearly or exponentially between the seabed and a predefined elevation
elev
elev
v el-s
Zw
v el-s
Zw
v el-b
v el-b
Linear current variation
Exponential current variation
above which the current is assumed to remain constant.
2.
Direction and elevation are in the ‘water’ axis system. Direction is in degrees around the water Zw axis,
zero degrees being in the positive Xw direction, and ninety degrees being in the positive Yw direction.
Yw
Current Direction
q
Xw
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-13
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
3.
Options exist to modify the current profile using either mass conservation or relative velocities. See
Appendix M.7.
4.
The CURR command remains operative until overridden by a subsequent TIDE, CURR or PCUR
command. If it is required to return to having no current or tide loading then a dummy TIDE command
should be provided with zero velocity.
M.6.7 DRAG Coefficients
The DRAG command defines the drag coefficients, Cd, for the members used in the calculation of wave and
wind forces.
DRAG
cdx
cdy
TABL
ELEM
elem
GROU
group
PROP
prop
cdz
tablename
ZONE
zonename
ALL
Parameters
DRAG
: keyword
cdx
: drag coefficient in element local x-direction. (Real)
cdy
: drag coefficient in element local y-direction. (Real)
cdz
: drag coefficient in element local z-direction. (Real)
TABL
: keyword to indicate that a table is to be utilised for determining the hydrodynamic coefficient
tablename
: name of table containing drag coefficients
ZONE
: keyword to indicate drag coefficients apply only to elements or part of elements in the zone
zonename
: name of zone
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-14
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
ALL
: keyword to indicate selection of all elements
Notes
1.
The command is optional and if omitted the program defaults to the following values:
2.
Axial,
x
Cd = 0.0
Transverse,
y and z
Cd = 0.7
Drag coefficients may be made dependent on Reynolds number or Keulegan-Carpenter number by use of
the TABL keyword. See RENL and KC commands for details of how to set up the tables.
Examples
DRAG
0.0
DRAG
RENL
0.7
0.75
TABLE1
ELEM
ZONE
10
20
GROWTH
30
ALL
M.6.8 ELEVATION Command
The ELEV command defines:
(a)
The Mean Water Level relative to the Water Axes Origin
(b)
The Sea Bed Level relative to the Water Axes Origin
(c)
The density of the sea water
(d)
The density of the air
This command is mandatory in the first loadcase, but need not reappear thereafter.
ELEV
selev
belev
water density
( air density )
Parameters
ELEV
: keyword
selev
: elevation of mean water level relative to water axes origin. (Real)
belev
: elevation of sea bed relative to water axis. (Real)
water density
: mass density of sea water (e.g. 1025Kg/m3). (Real)
air density
: mass density of air (e.g. 1.23 kg/m3). (Optional). (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-15
ASAS (Non-Linear) User Manual
Appendix M - Wave Loading
Note
The density is multiplied by the acceleration due to gravity as input by the GRAV command, and so must be
input in units of MASS per unit volume e.g. 1025 Kg/m3
Example
ELEV
100
-25
1025
M.6.9 END Command
An END command terminates the WAVE LOAD data block.
END
Parameters
END
: keyword
M.6.10 EXECUTE Command
The EXEC command signifies the end of data for a given wave case. Since there can only be one single case in
each ASAS-NL data, the use of EXEC to break up different wave cases is therefore not required and the
command is only retained for compatibility with WAVE. If EXEC is specified, this must appear immediately
before the END command.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-16
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
EXEC
Parameters
EXEC
: keyword
M.6.11 FREE Flooding Command
The FREE command may be used to specify those members which are flooded with the external fluid up to the
actual water surface thus inducing additional loading due to the weight of the contained fluid on the members
concerned. The command is optional and no free flooding is assumed if omitted.
FREE
ELEM
elem
GROU
group
PROP
prop
elev
ALL
Parameters
FREE
: keyword
elev
: elevation used for computing internal pressure. (Real)
If elev Zb, the sea bed level, internal pressure is computed assuming fluid pressure to elevation
elev. If elev <Zb, internal pressure is computed to the elevation of the water surface vertically
above the point in question.
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-17
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
ALL
: keyword to indicate selection of all elements
Notes
1.
Free flooding effects are calculated for members below the sea bed.
2.
If elev is omitted in both the BUOY and Free commands internal pressure will be ignored. If elev is
specified more than once for an element, the last specification will be assumed.
3.
Internal pressure, if any, is only included for the BRIG option.
M.6.12 GRAVITY Command
The GRAV command defines the relationship of the jacket axes to the water axes by specifying the value and
direction of the gravitational acceleration relative to the jacket axis system. This command is mandatory. It
must appear only once.
GRAV
gx
gy
gz
Parameters
GRAV
: keyword
gx
: gravitational vector component in x direction (global jacket axis). (Real)
gy
: gravitational vector component in y direction (global jacket axis). (Real)
gz
: gravitational vector component in z direction (global jacket axis). (Real)
Notes
1.
If the components of gravitational acceleration are given as (0,0,-g), the jacket and water axes are
coincident, with the Z-axis directed vertically upwards.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-18
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
ZG
YG
XG
ZW
YW
XW
Jacket and water axes coincident
2.
The GRAV command defines the direction of the gravitational vector (-Zwater) with respect to the jacket
(global) axis system. The convention adopted for the X and Y axes of the water axes system is as
follows:
Xwater always lies in the global XY plane with Ywater on the positive side of the global XY plane. In
the special case where Ywater is also in the global XY plane Ywater lies in the global Y direction.
YG
ZG
XG
ZW
YW
XW
General orientation of water axes
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-19
ASAS (Non-Linear) User Manual
Appendix M - Wave Loading
M.6.13 GRID Wave Command
This data is used as an alternative means for defining the wave kinematics (i.e. particle velocities and
accelerations) instead of adopting one of the wave theories detailed in Section M.6.46 WAVE DATA. Typically
this data is used when the structure is to be loaded with waves that are outside of the conventional wave theory
applicability limits (see Figure M.1) and an alternative source of wave kinematics has been found. The wave is
described by defining the surface profile together with velocities and accelerations at regular intervals or grid
points throughout the wave. The location of the horizontal and vertical grid lines may be selected to coincide
with oceanographic/measured data. The general form of the data shown below.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-20
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
SYMM
GRID
nloc
nhgt
w av elength
ASYM
GPHS
phase
GLOC
location
SURF
surface
VELH
v alue
VELV
v alue
ACCH
v alue
ACCV
v alue
GHGT
height
VELH
v alue
VELV
v alue
ACCH
v alue
ACCV
v alue
GRID Wave Header
SYMM
GRID
nloc
nhgt
w av elength
ASYM
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-21
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Parameters
GRID
: keyword to indicate beginning of grid data
SYMM
: keyword. The wave is considered to be symmetric in profile about the crest position.
Horizontal velocities and vertical accelerations are assumed symmetric about the crest position.
Vertical velocities and horizontal accelerations are antisymmetric about the crest. Only half the
wave period needs to be defined (see Note 1 below). This is the default option.
ASYM
: keyword. The wave is considered to be asymmetric in both profile and wave kinematics. The
whole wave period must be defined.
nloc
: number of horizontal grid locations to be defined (see Figure M.2). (Integer)
nhgt
: number of vertical grid positions to be defined (see Figure M.2). (Integer)
wavelength : wavelength. This must be supplied in order to establish the phase relationship between the
structural elements and the wave. (Real)
SURF(1)
HEIGHT(5)
SURF(2)
HEIGHT(4)
SURF(3)
HEIGHT(3)
nhgt
vertical
grid
locations
SURF(4)
SURF(5)
HEIGHT(2)
HEIGHT(1)
PHASE(1)
PHASE(2)
PHASE(3)
PHASE(4)
PHASE(5)
nloc horizontal grid locations
Figure M.2 Grid definitions
Example
A symmetric wave of 110 m wavelength is defined using 5 horizontal and 4 vertical grid points.
GRID
SYMM
5
4
110.
Horizontal Grid Definition
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-22
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
GPHS
phase
GLOC
location
Parameters
GPHS
: keyword to indicate that phase angles are to be used in defining the horizontal grid locations
phase
: phase angle from crest position. (Real)
nloc values must be supplied to fully define the grid. See Note 2 for sign convention
GLOC
: keyword to indicate that distances are to be used in defining the horizontal grid locations
location
: distance from the crest position. (Real)
nloc values must be supplied to fully define the grid. See Note 2 for sign convention
Example
Horizontal locations of 9 grid lines are defined.
GPHS
GPHS
0.0 -10.0 -20.0 -40.0
-120.0 -150.0 -180.0
-60.0
-90.0
or, assuming the wavelength is 180 m,
GLOC
0.0
GLOC
60.0
5.0 10.0
75.0
20.0
30.0
45.0
90.0
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-23
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
SURFACE Profiles and Kinematics
SURF
surface
VELH
v alue
VELV
v alue
ACCH
v alue
ACCV
v alue
Parameters
SURF
: keyword to denote that surface elevations and kinematic definitions are to follow
surface
: wave surface elevation relative to the water axes for each of the horizontal grid locations defined
on the GPHS or GLOC commands. nloc values in total must be supplied. (Real)
VELH
: keyword to indicate horizontal particle velocities
VELV
: keyword to indicate vertical particle velocities
ACCH
: keyword to indicate horizontal particle accelerations
ACCV
: keyword to indicate vertical particle accelerations
value
: wave kinematics for the surface for each of the horizontal grid locations defined on the GPHS or
GLOC command. nloc values in total must be supplied. (Real)
Example
Surface profile and kinematics for 4 phase locations.
SURF 8.75
8.65
8.37
8.0
VELH 2.2
VELV 0.0
1.82
1.05
0.93
1.61
0.0
1.51
ACCH 0.0
2.2
3.37
3.29
ACCV -2.44 -1.83 -0.39 1.11
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-24
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
GRID Kinematics
This block of data should be repeated nhgt times
GHGT
height
VELH
v alue
VELV
v alue
ACCH
v alue
ACCV
v alue
Parameters
GHGT
: keyword to denote that kinematic definitions for the specific elevation are to follow
height
: grid elevation relative to the water axes. (Real)
VELH
: keyword to indicate horizontal particle velocities
VELV
: keyword to indicate vertical particle velocities
ACCH
: keyword to indicate horizontal particle accelerations
ACCV
: keyword to indicate vertical particle accelerations
value
: wave kinematics for the given grid height for each of the horizontal grid locations defined on the
GPHS or GLOC command. (Real)
Values corresponding to grid positions above the water surface need not be defined. See Note 3.
Example
Velocities and accelerations for elevation 10.0 for 4 phase locations
GHGT
10.0
VELH
VELV
0.645
0.0
0.322
0.553
0.0
0.639
ACCH
ACCV
0.0
0.674 1.17
-1.15 -0.974 -0.485
1.35
0.185
0.558
0.315
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-25
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Notes
1.
For symmetric waves, only half the wave period needs to be defined, the program will automatically
generate wave kinematics for the symmetric part of the wave. The generated kinematics are shown in
FigureM.3 below.
PHASE = 0
VELV
VELH
VELH
VELV
ACCV
ACCV
ACCH
ACCH
GENERATED
DEFINED
Figure M.3 Generated symmetric wave kinematics
2.
In common with all phase definitions in WAVE, a positive phase angle indicates that the wave crest has
passed the point of interest; conversely, this corresponds to a negative linear distance, as shown in Figure
M.4 below.
+180
-L/2
PHASE = 0
DISTANCE = 0
-180
+L/2
Figure M.4 Sign convention of phase and distance definitions
3.
Where grid points occur at or above the surface elevation, the kinematic values may be set to zero or, if at
the end of the line, may be ignored. Thus only sufficient number of values to define the subsurface grid
need be supplied.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-26
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
M.6.14 Marine GROWTH Command
The GROW command defines the thickness of marine growth. The command is optional and zero thickness is
assumed if omitted. A number of such commands may be used to define varying growth thickness with depth.
New drag and inertia coefficients may be defined to take account of the roughness of marine growth.
elem
ELEM
GROW
thick
density
ZONE
zonename
upper
cd
GROU
group
PROP
prop
cm
low er
ALL
Parameters
GROW
: keyword
thick
: thickness of marine growth. (Real)
density
: saturated density of marine growth. (Real)
ZONE
: keyword to indicate growth values apply only to elements or parts of elements in the zone
zonename
: name of zone
upper
: upper level of growth relative to water axes. (Real)
lower
: lower level of growth relative to water axes. (Real)
cd
: drag coefficient in element local y and z directions. If not defined the appropriate element drag
coefficient is used. (Real)
cm
: mass coefficient in element local y and z directions. If not defined the appropriate element
mass coefficient is used. (Real)
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-27
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Notes
1.
The self weight of marine growth is automatically included in the total weight reported. If self weight of
the growth is not required then the density should be set to zero.
2.
If defined, the drag and inertia coefficients supplied on the GROW command override those defined on
the DRAG and/or MASS commands for a given element irrespective of the order of the data.
M.6.15 HYDR Command
The HYDR command defines section dimensions and marine growth values for a part of an element. The
command is optional and existing section dimensions and growth values are used if omitted. A number of such
commands may be used to define specific section dimensions which will supersede existing dimensions. The
same applies for marine growth.
DIAM
dy
HYDR
dz
AREA
at
as
ai
SURF
perimeter
DENS
density
GROW
ag
ECAP
NONE
ain
aout
(FACT)
len1
len2
ELEM
elem
GROU
group
PROP
prop
dg
Parameters
HYDR
: keyword
DIAM
: keyword to indicate that revised section dimensions are supplied
dy
: Overall dimension in local-y direction (see Note 3), including marine growth (if present)
dz
: Overall dimension in local-z direction (see Note 3), including marine growth (if present)
AREA
: keyword to indicate that revised section areas are supplied
at
: total area, including marine growth (if present). This is used in Morison’s equation
as
: cross-sectional area of element (ie annulus area for a tube). This is used for self-weight
calculations
ai
: cross-sectional area of internal void of tube. This is used for buoyancy calculations
SURF
: keyword to indicate that a revised surface perimeter is supplied
perimeter : surface perimeter, including marine growth (if present). This is used for axial drag calculations
DENS
: keyword to indicate that a revised element material density is supplied
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-28
ASAS (Non-Linear) User Manual
Appendix M - Wave Loading
density
: element material density. This is used for self-weight calculations
GROW
: keyword to indicate that revised marine growth data is supplied
ag
: cross-sectional area of growth (ie area of annulus of growth on a tube)
dg
: saturated density of marine growth. These are used to calculate the weight of the growth for the
section
NONE
: keyword to indicate that there is no marine growth on this section
ECAP
: keyword to indicate that revised end cap area are supplied
aout
: outer enclosed area of end cap. This is used to calculate end cap face due to external pressure
ain
: inner enclosed area of end cap. This is used to calculate end cap face due to internal pressure
FACT
: keyword to indicate that the lengths following are proportions of the element length (ie a
maximum of 1.0)
len1
: distance along the element to the start of the revised data
len2
: distance along the element to the end of the revised data. If FACT has been specified, then len1
and len2 are the proportion of the element lengths
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer). ALL may not be specified.
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer). ALL may not be specified.
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer). ALL may not be specified.
Notes
1.
If a section is to be respecified because of a local change in dimension or area, then the following values
MUST be specified.
No growth - DIAM, AREA, SURF
Growth
- DIAM, AREA, SURF, GROW
GROW NONE should be included if no growth is required on an element that is within a marine growth
zone.
2.
If the length information is omitted, the properties are applied along the complete length of the element.
3.
The dimensions supplied are given in terms of the local axes of the element, as shown below.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-29
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Y
dy
Z
Z
dz
Y
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-30
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
4.
Beam elements that have sections assigned to them via their geometry definition will automatically adopt
appropriate properties for the calculation of wave loading and added mass. The following tables provide
information regarding the terms used in the load and mass computations.
where
d
is beam depth
b
is beam width
tf
is flange thickness
tw
is web thickness
t
is plate thickness
tg
is thickness of any attached marine growth
The above assumes that the top and bottom flanges for the BOX and FBI section types are the same. The
program will correctly account for different bottom flange dimensions if specified. Any specified fillet radius is
ignored in these calculations.
Section type Drag load
TUB
BOX
RHS
Inertia load
Self weight
Buoyancy/
Free flooding
Hydrodynamic
mass
End cap force
Cdydyρw
Cdzdzρw
Cmyatρw
Cmzatρw
ρsas
ρwat - ρiai
ρw(Cmy - 1)at
ρw(Cmz - 1)at
ρi ain-ρo aout
Cdydyρw
Cdzdzρw
Cmyatρw
Cmzatρw
ρsas
ρwat
ρw(Cmy - 1)at
ρw(Cmz - 1)at
N/A
N/A
N/A
N/A
N/A
N/A
N/A
WF
CHAN
ANGL
TEE
FBI
PRI5
FAB5
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-31
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
5.
Prismatic and fabricated sections that are required to be wave loaded must have explicit HYDR
commands supplied.
Example
A tube with diameter 1.4 and thickness 0.07 has a marine growth applied of 0.2 and density 1.5 over a length of
1.5 starting 2.1 from the first end. The following commands would need to be specified to reflect this.
HYDR DIAM
1.8
HYDR AREA
2.5446900
1.8
2.1
0.2924823
3.6
HYDR SURF
HYDR GROW
5.6548668
1.0053096
2.1
1.5
3.6
2.1
ELEM
3
1.2468981
ELEM 3
3.6 ELEM
2.1
3.6
ELEM
3
3
= π(1.4 + 2 x 0.2)2/4 = 2.5446900
where at
as
= π(1.42 - (1.4 - 2 x 0.07)2)/4 = 0.2924823
ai
= π(1.4 -2 x 0.07)2/4 = 1.2468981
perim = π(1.4 +2 x 0.2) = 5.6548668
= π((1.4 + 2x 0.2)2 - 1.42)/4 = 1.0053096
ag
M.6.16 Keulegan-Carpenter Number Tables
The KC command defines tables of Keulegan-Carpenter numbers with corresponding values of drag and mass
coefficients so that for each element the drag and mass coefficients can be calculated as a user-defined function
of the Keulegan-Carpenter number. The table can, optionally, be made to be dependent on Reynolds number
KC
tablename
RENL
r
DRAG
kc
cd
MASS
kc
cm
DRAG
MASS
kc
cd
cm
allowing bilinear interpolation of drag and mass coefficients.
Parameters
KC
: keyword
tablename : name of the Keulegan-Carpenter table (up to 32 alphanumeric characters)
RENL
: keyword to indicate Reynolds number is to be supplied
r
: Reynolds number. (Real)
DRAG
: keyword to indicate drag value is supplied after Keulegan-Carpenter number
MASS
: keyword to indicate mass value is supplied after Keulegan-Carpenter number
kc
: Keulegan-Carpenter number. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-32
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
cd
: corresponding drag coefficient. (Real)
cm
: corresponding mass coefficient. (Real)
Notes
1.
For each element the Keulegan-Carpenter number KC and (optionally) Reynolds number Re are
calculated as follows:
Re
=
Diameter x velocity / Kinematic viscosity
KC
=
Wave period x velocity / Diameter
where the velocity is the maximum water particle velocity throughout a wave cycle normal to the
member. The calculated value of KC defines a position in the array of KC commands and linear
interpolation is used to obtain values for the drag and mass coefficients for the member. If the Reynolds
number is also given, bilinear interpolation is utilised.
2.
For values of KC outside the defined range, the related parameter is assumed constant and equal to the
Cd
•
•
•
Kc
extreme values defined, eg
3.
The drag and/or mass coefficients must be in the order of the DRAG and MASS keywords.
4.
The kinematic viscosity (VISC) must be specified, if Reynolds number dependency is required.
5.
Note that this command is not applicable to the NewWave model.
Examples
KC KCTABLE1 DRAG MASS
:
4.0 0.3
1.95
:
8.0 0.48 1.8
: 12.0 0.75 1.6
: 20.0 1.05 1.2
M.6.17 Wave KINEMATICS Factor Command
The KINE command specifies a user defined wave kinematics factor for use within the API codes of practice.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-33
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
KINE
factor
Parameters
KINE
: keyword
factor
: user defined wave kinematics factor. (Real)
Notes
1.
If the KINE command is not used, factor =
power+ 1
where power is the wave spreading power
power + 2
defined on the SPREAD command.
2.
If neither KINE nor SPREAD command is used, a default factor of 1.0 is used.
3.
If both the KINE and SPREAD commands are used, the value of the KINE command takes precedence.
4.
This command will only be utilised when used in conjunction with the APIW option.
M.6.18 LFUN Data
The LFUN command enables scaling of the wave load by associating a load function with the wave loading.
This command is optional and, if omitted, a unit load factor is assumed.
LFUN
lfunno
Parameters
LFUN
: keyword
lfunno
: load function number
Notes
1.
For proportional loading (i.e. PROP), lfunno should be set to 1.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-34
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
M.6.19 MASS Inertia Coefficients
The MASS command defines the inertia coefficients, Cm, for the members used in the calculation of wave
forces.
MASS
cmx
cmy
TABL
ELEM
elem
GROU
group
PROP
prop
cmz
tablename
ZONE
zonename
ALL
Parameters
MASS
: keyword
cmx
: inertia coefficient in element local x-direction. (Real)
cmy
: inertia coefficient in element local y-direction. (Real)
cmz
: inertia coefficient in element local z-direction. (Real)
TABL
: keyword to indicate that a table is to be utilised for determining the hydrodynamic coefficient
tablename
: name of table containing mass coefficients
ZONE
: keyword to indicate mass coefficients apply only to elements or parts of elements in the zone
zonename
: name of zone
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Notes
1.
The command is optional and if omitted the program defaults to the following values:
Axial,
x
Cm = 0.0
Transverse,
y and z
Cm = 2.0
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-35
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
2.
Inertia coefficients may be made dependent on Reynolds number, Keulegan-Carpenter number or A/D
ratio by use of the TABL keyword. See RENL and KC commands for details of how to set up the
tables.
Examples
MASS
0.0
MASS
RENL
2.0
2.2
TABLE1
ELEM
ZONE
10
20
GROWTH
30
ALL
M.6.20 MOVE Command
The MOVE command defines the origin of the Water Axes relative to the structure Global Axes. The command
is optional and if omitted, the origins of the Water and the Global axes are assumed coincident.
MOVE
x
y
z
Parameters
MOVE
: keyword
x,y,z
: coordinates of origin of water axis in the global coordinate system. (Real)
Example
MOVE
0.0
0.0
-∆z
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-36
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
ZG
YG
XG
ZW
∆Z
YW
XW
Water axis relative to jacket axis
M.6.21 NANG Command
This command defines the number of angle steps a wave is to be divided into for determining the maximum
velocity experienced by a submerged element in a wave cycle. The maximum velocity is used for calculating the
drag and mass coefficients for an element if Reynolds or Keulegan-Carpenter tables are used. See the notes in
M.6.16 and M.6.35 on how the computed velocity is utilised.
nangle
NANG
Parameters
NANG
: keyword
nangle
: the number of equal phase angles a wave is to be divided into for evaluating the maximum
velocity. The angle increment used is 360/nangle degrees
Example
NANG
20
Notes
1.
The value for nangle must be greater than zero.
2.
The default value for nangle is 8.
3.
No more than one NANG command is allowed for each wave case.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-37
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
M.6.22 NOBM Command
The NOBM command is replaced by the NOLO command.
M.6.23 NOBO Command
The NOBO command specifies elements for which buoyancy loads are excluded. The command overrides any
previous BUOY command associated with the specified elements. The buoyancy loading may be reactivated at
any later stage by using another BUOY command.
ELEM
elem
GROU
group
PROP
prop
NOBO
ALL
Parameters
NOBO
: command keyword
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Note
Any number of BUOY and NOBO commands may be used to activate and deactivate loading for different
elements. The commands are processed in user input order.
M.6.24 NOFR Command
The NOFR command specifies elements for which free flooding loads are excluded. The command overrides
any previous FREE command associated with the specified elements. The free flooding loading may be
reactivated at any later stage by using another FREE command.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-38
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
ELEM
elem
GROU
group
PROP
prop
NOFR
ALL
Parameters
NOFR
: keyword
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Note
Any number of FREE and NOFR commands may be used to activate and deactivate loading for different
elements. The commands are processed in user input order.
M.6.25 NOLO Command
The NOLO command specifies elements for which all loads are excluded. The command overrides any previous
load command associated with the specified elements. The loading may be reactivated at any later stage by using
appropriate load commands.
ELEM
elem
GROU
group
PROP
prop
NOLO
ALL
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-39
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Parameters
NOLO
: keyword
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Note
Any number of LOAD and NOLO commands may be used to activate and deactivate loading for different
elements. The commands are processed in user input order.
M.6.26 NOSW Command
The NOSW command specifies elements for which structural self weight loads are to be ignored. The command
overrides any previous SLWT command associated with the specified elements. The self weight loading may be
reactivated at any later stage by using another SLWT command.
ELEM
elem
GROU
group
PROP
prop
NOSW
ALL
Parameters
NOSW
: keyword
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-40
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Notes
1.
Any number of SLWT and NOSW commands may be used to activate and deactivate loading for
different elements. The commands are processed in user input order.
2.
The weight of marine growth is automatically calculated if a GROW command is present. It is unaffected
by SLWT/NOSW commands.
3.
The weight of any internal fluid is automatically calculated if BUOY/FREE commands are present. It is
unaffected by SLWT/NOSW commands.
M.6.27 NOWI Command
The NOWI command specifies tubular elements for which wind loads are excluded. The command overrides any
previous WIND command for the specified elements. The wind loading may be reactivated at any later stage by
using another WIND command.
ELEM
elem
GROU
group
PROP
prop
NOWI
ALL
Parameters
NOWI
: keyword
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-41
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Note
The NOWI command is overridden by subsequent WIND definitions. It is important, therefore, to respecify the
NOWI commands after each use of the WIND command.
M.6.28 NOWL Command
The NOWL command specifies tubular elements for which wave loads are excluded. The command overrides
any previous WAVE command for the specified elements. The wave loading may be reactivated at any later
stage by using another WAVE command.
ELEM
elem
GROU
group
PROP
prop
NOWL
ALL
Parameters
NOWL
: keyword
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Notes
1.
The NOWL command is overridden by subsequent WAVE definitions. It is important, therefore, to
respecify the NOWL commands after each use of the WAVE command.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-42
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
2.
Use of NOWL ALL does not nullify the existing WAVE definition. The wave surface profile is still
applied and this may affect other loading such as buoyancy. To return to the still water condition, a
WAVE command with zero wave height must be specified.
M.6.29 OFFSET Command
The OFFS command defines offsets of member ends from the nodal positions. In this way the thicknesses of
joints can be taken into account when calculating the loading on these members. The offset is taken as a
shortening of the member along its axis.
OFFS
off1
ELEM
elem
GROU
group
PROP
prop
off2
ALL
Parameters
OFFS
: keyword
off1
: offset at end one of element. (Real)
off2
: offset at end two of element. (Real)
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Note
The offsets defined on this command are additive to any member offsets which may have been defined in the
Geometric Properties data. See ASAS User Manual for details.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-43
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
M.6.30 OUTPUT Control Command
The OUTP command controls the amount of printed output for each wave case.
OUTP
iout
Parameters
OUTP
: keyword
iout
: output control integer
0
No output
1
Total forces and moments and total jacket mass are reported
(default)
2
Total forces and masses on each member are reported
3
Water particle velocities, accelerations, drag and mass
coefficients and the individual forces on each member
are reported. Individual masses on each section of a member
are reported.
Notes
1.
Output 3 produces a large quantity of output and should be used with caution.
M.6.31 PEXT Command
The PEXT command specifies those members where the external pressures are to be calculated from the given
density and elevation. The command is optional and, if omitted, the external pressure (if applicable) will be
PEXT
density
elev
ELEM
elem
GROU
group
PROP
prop
ALL
calculated from the sea water density and surface elevation including the effect of wave action.
Parameters
PEXT
: keyword
density
: mass density of external fluid (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-44
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
elev
: elevation used for computing external pressure (Real)
If elev Zb the sea bed level, external pressure is computed assuming fluid pressure to elevation
elev. If <Zb, external pressure is computed to the elevation of the water surface vertically above
the point in question.
ELEM
: keyword to indicate element selection
elem
: list of user element numbers (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers (Integer)
ALL
: keyword to indicate selection of all elements
Notes
1.
External pressure calculation is only carried out for the BRIG option
M.6.32 POINT Current Command
The PCUR command specifies a user defined current profile. Each PCUR (point current) command defines a
single point on a current profile. The profile may vary in both magnitude and direction with depth.
PCUR
v elocity
direction
elev ation
Parameters
PCUR
: keyword
velocity
: current velocity. (Real)
direction : current direction relative to water axis system. (Real)
elevation : elevation of this point value relative to water axis. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-45
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Notes
1.
Direction and elevation are in the ‘water’ axis system. Direction is in degrees around the water Zw axis,
zero degrees being in the positive Xw direction and ninety degrees being in the positive Yw direction.
SWL
elevation
Yw
current
velocity
Current Direction
Zw
q
2.
Xw
PCUR commands are cumulative and a table is built-up as each command is read. To reinitialise the
table, supply another type of current command (i.e. TIDE or CURR), which can have magnitude zero, or
use the RESEt command.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-46
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
3.
All locations above the uppermost level defined have a constant current magnitude and direction equal to
the defined values. Similarly, the values below the lowest defined value are constant. Thus one PCUR
command will define a constant current magnitude and direction at all water depths.
4.
Options exist to modify the current profile using either mass conservation or relative velocities (see
Appendix M.7).
M.6.33 PHASE Command
The PHAS command determines the position of the wave crest relative to the origin of the water axis system.
The command is optional and an initial phase position of zero will be assumed if not specified.
PHAS
npos
pos
inc
Parameters
PHAS
: keyword
npos
: number of wave positions in this case. (Integer) (Always set to 1)
pos
: position of wave crest relative to water axis (degrees). (Real)
Notes
1.
A phase position of zero corresponds to the wave crest at the origin of the water axis system. A positive
ZW
..
..
..
..
.. -10 °
.
..
..
..
..
..
.
+30º
Direction of
wave advance
wave position indicates that the wave crest has passed the water origin.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-47
ASAS (Non-Linear) User Manual
2.
Appendix M - Wave Loading
There is no phase increment in a static analysis (i.e. the phase position will remain unchanged even if a
solution is attempted at more than one pseudo-time).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-48
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
3.
In a transient dynamics analysis, the phase increment at each solution step is given by
∆φ = ∆ t
2π
T
∆φ
phase increment
∆t
time increment
T
wave period
4.
The PHASE command is not available for irregular wave analysis since the wave kinematics at a given
time are no longer sinusoidal.
M.6.34 PRINT Command
The PRIN command may be used to override the OUTP command for specific elements.
PRIN
iout
elem
Parameters
PRIN
: keyword
iout
: output control integer
1
No elemental information is reported
2
Total forces and masses on each member are reported
3
Water particle velocities, accelerations, drag and mass
coefficients, and the individual forces on each member are
reported. Individual masses on each section of a member are
reported.
elem
: user element number. (Integer)
Note
Option 3 produces a large quantity of output and should be used with caution.
M.6.35 Reynolds Number Tables
The RENL command defines tables of Reynolds numbers with corresponding values of drag and mass
coefficients so that for each element the drag and mass coefficients can be calculated as a user-defined function
of Reynolds number. The table can, optionally, be made to be dependent on the Keulegan-Carpenter number
allowing bilinear interpolation of drag and mass coefficients.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-49
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
RENL
tablename
KC
kc
DRAG
r
cd
MASS
r
cm
DRAG
MASS
r
cd
cm
Parameters
RENL
: keyword
tablename : name of the Reynolds table (up to 32 alphanumeric characters)
KC
: keyword to indicate Keulegan-Carpenter number is to be supplied
kc
: Keulegan-Carpenter number. (Real)
DRAG
: keyword to indicate drag value is supplied after Reynolds number
MASS
: keyword to indicate mass value is supplied after Reynolds number
r
: Reynolds number. (Real)
cd
: corresponding drag coefficient. (Real)
cm
: corresponding mass coefficient. (Real)
Notes
1.
For each element the Reynolds number Re and (optionally) Keulegan-Carpenter number KC are
calculated as follows:
Re
=
Diameter x velocity / Kinematic viscosity
KC
=
Wave period x velocity / Diameter
where the velocity is the maximum water particle velocity throughout a wave cycle normal to the
member. The calculated value of Re defines a position in the array of RENL commands and linear
interpolation is used to obtain values for the drag and mass coefficients for the member. If the KeuleganCarpenter number is also given, bilinear interpolation is utilised.
2.
For values of Re outside the defined range, the related parameter is assumed constant and equal to the
extreme values defined, eg
Cd
•
•
•
Re
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-50
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
3.
The drag and/or mass coefficients must be in the order of the DRAG and MASS keywords.
4.
The kinematic viscosity (VISC) must be specified.
5.
Note that this command is not applicable to the NewWave model.
Examples
RENL REYNOLD1
: 30000 1.2
: 40000 1.0
: 80000 0.8
: 100000 0.65
: 200000 0.6
KC 10
1.15
1.3
1.65
1.70
1.75
DRAG
MASS
20000
1.6
1.0
M.6.36 SLWT Command
The SLWT command may be used to include the structural weight of members. If the command is omitted then
no structural weight will be calculated.
SLWT
ELEM
elem
GROU
group
PROP
prop
density
ALL
Parameters
SLWT
: keyword
density
: structural material density of member(s). (Real)
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-51
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Notes
1.
To prevent the calculation of element self weight use the NOSW command.
2.
The calculation of the self-weight of any marine growth or internal fluid is not affected by this command.
See BUOY, GROW, NOFR and NOBO commands.
M.6.37 SPECTRAL Command
This command is used to define the wave spectrum to be employed in a New Wave or irregular wave analysis.
SPEC
JONS
peak
PMOS
peak
UDEF
freq
energy
UWAV
height
period
gamma
phase
w av elength
Parameters
SPEC
: keyword
JONS
: keyword to select a JONSWAP wave spectrum
PMOS
: keyword to select a Pierson Moskowitz wave spectrum
UDEF
: keyword to indicate that a user defined spectrum is to be supplied
UWAV
: keyword to indicate that user defined wavelet details are to be supplied
peak
: peak period (Tp) for the spectrum. (Real)
gamma
: enhancement factor for the spectrum. Defaults to 3.3 if not defined. (Real)
freq
: frequency ordinate (Hz) for user defined spectrum
energy
: corresponding energy density ordinate (length2/Hz) for user defined spectrum
height
: height of wavelet. (Real)
period
: period of wavelet. (Real)
phase
: phase of wavelet. (Real)
wavelength:length of wavelet. If zero, the wavelength will be computed internally by the program. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-52
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Notes
1.
Only one such command should be defined for a given New Wave / irregular wave case.
2.
For user defined spectra sufficient pairs of ordinates must be provided to adequately define the sea state.
3.
For UWAV spectrum, phase is unused in a New Wave analysis.
4.
For UWAV spectrum, the number of wavelet data defined in this command determines the number of
wavelets to be used to model the wave spectrum. This will override any WPAR WAVELET data
specified.
Example
SPEC
PMOS
SPEC
UDEF
10.0
:
:
0.04
0.0654
0.004
7.650
0.0477
0.0724
0.458
8.2405
0.0547
0.0794
3.089
7.4185
:
:
0.0865
....
6.1053
0.0936
4.8084
0.1006
3.7133
M.6.38 Wave SPREADING Command
The SPRE command specifies a user defined wave spreading power for use with the API codes of practice.
This command is used to enable the program to compute a wave kinematics factor.
SPRE
power
Parameters
SPRE
: keyword
power
: user defined wave spreading power. (Real)
Notes
(power+ 1)
(power+ 2)
1.
If the SPRE command is used, wave kinematics factor =
2.
If the SPRE command is not used (and KINE is not used) a default value of 1.0 is used for the wave
kinematics factor.
3.
If both the KINE and SPREAD commands are used, the value of the KINE command take precedence.
4.
This command will only be utilised when used in conjunction with the APIW option.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-53
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
5.
Note that this command is not applicable to the NewWave model.
M.6.39 STOP Command
A STOP command is needed to signify the end of the data.
STOP
Parameters
STOP
: keyword
M.6.40 TIDE Command
The TIDE command specifies a predetermined current profile in the same direction as an associated wave.
TIDE
iprofile
v el-s
v el-b
elev
Parameters
TIDE
: keyword
iprofile
: profile type integer
1
linear profile
2
exponential profile
vel-s
: current velocity at still water level. (Real)
vel-b
: current velocity at sea bed. (Real)
elev
: elevation relative to water axis at which current becomes constant. (Real)
Notes
1.
The tide current may vary either linearly or exponentially between the seabed and a predefined elevation
above which the current is assumed to remain constant.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-54
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
SWL
elev
elev
v el-s
ZW
v el-s
ZW
v el-b
Linear current variation
v el-b
Exponential current variation
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-55
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
2.
Options exist to modify the current profile using either mass conservation or relative velocities (see
Appendix M.7).
3.
The TIDE command remains operative until overridden by a subsequent TIDE, CURR or PCUR
command. If it is required to return to having no current or tide loading then a dummy TIDE command
should be provided with zero velocity.
M.6.41 TOLERANCE Command
The TOLS command defines the tolerances to be used to decide between linear and quadratic distributed loads
and for the subdivision of elements. The command is optional and, if omitted, a default value of 0.1 is used to
decide between linear and quadratic and no sub-division will occur.
The water particle force is calculated at the centre point of the element or subdivision and compared with a value
interpolated linearly between the end values. If this lies within the given tolerance then linear distributed loads
are used and no subdivision occurs. If the calculated force lies outside the given tolerance, quadratic distributed
loads are used and the second tolerance is checked to decide whether or not to subdivide the element. If the
value lies outside the second tolerance then both halves of the element have separate quadratic distributed loads.
TOLS
tload
tsub
Parameters
TOLS
: keyword
tload
: tolerance for linear/quadratic distributed loads. (Real)
tsub
: tolerance for element subdivision. (Real)
Note
If tsub is omitted then no subdivision occurs.
M.6.42 UNITS Command
If global units have been defined using the UNITS command in the Preliminary data (Section 5.1.42) the wave
input data units may be locally overridden by the inclusion of an UNITS command.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-56
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
UNITS
unitnm
Parameters
UNITS
:
keyword
unitnm :
name of unit to be utilised (see below)
Notes
1.
Force, length, and angular units may be specified. Only those terms which are required to be modified
need to be specified, undefined terms will default to those currently active.
2.
The default input angular unit for waveload data is degrees.
3.
A list of valid unit names can be found in Section 5.1.42.1.
4.
The mass unit is derived from the force and length unit currently defined. In order to determine the
consistent mass unit the force and length terms must both be either metric or imperial. This requirement is
only necessary where mass or density data is being specified, in other cases inconsistencies are permitted.
M.6.43 VAXS Command
This command defines the orientations of the hydrodynamic axes with respect to the water axes. By default, the
hydrodynamic axes are assumed to be coincident with the water axes.
VAXS
x’x
x’y
x’z
y’x
y’y
y’z
Parameters
VAXS
: keyword
x’x
: direction cosine of the hydrodynamic x’ axis w.r.t. the water x axis. (Real)
x’y
: direction cosine of the hydrodynamic x’ axis w.r.t. the water y axis. (Real)
x’z
: direction cosine of the hydrodynamic x’ axis w.r.t. the water z axis. (Real)
y’x
: direction cosine of the hydrodynamic y’ axis w.r.t. the water x axis. (Real)
y’y
: direction cosine of the hydrodynamic y’ axis w.r.t. the water y axis. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-57
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
y’z
: direction cosine of the hydrodynamic y’ axis w.r.t. the water z axis. (Real)
Notes
1.
Since both the AQWA hydrodynamic and ASAS water z axis are vertically upwards, the direction cosines
should define a transformation in the x-y plane, i.e. x’z=y’z=0.0.
2.
The hydrodynamic data (e.g. RAO) are given in the hydrodynamic axis system.
M.6.44 VISCOSITY Command
The VISC command defines the kinematic viscosity for the sea water for Reynolds number calculations.
VISC
viscosity
Parameters
VISC
: keyword
viscosity : kinematic viscosity
Note
This command must be present if Reynolds numbers (RENL commands) are used in the definition of drag and
mass coefficients.
Example
VISC
1.3E-06
M.6.45 VPOS Command
This command defines the reference positions (typically the CoG) for the hydrodynamic data (e.g. RAO and
phase). If not specified, the reference points are assumed to be at the origin of the water axes.
VPOS
xg
yg
zg
xpoff
ypoff
zpoff
Parameters
VPOS
: keyword
xg
: x reference position for RAO in water axis system. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-58
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
yg
: y reference position for RAO in water axis system. (Real)
zg
: z reference position for RAO in water axis system. (Real)
xpoff
: x offset of phase origin from the RAO reference origin in water axis system. (Real)
ypoff
: y offset of phase origin from the RAO reference origin in water axis system. (Real)
zpoff
: z offset of phase origin from the RAO reference origin in water axis system. (Real)
Note
The RAO and phase origins are assumed to be identical if the hydrodynamic information is provided by AQWA.
In this case, the phase origin offset data are always ignored
M.6.46 WAVE Command
The WAVE command defines the wave theory, and the Height, Period and Direction of the wave. This
command is optional, but if it appears must come after the ELEV command.
WAVE
theory
height
crest
NEWW
period
direction
sigheight
IRRE
direction
direction
Parameters
WAVE
: keyword
theory
: wave theory keyword
AIRY
Linear wave theory (Airy)
CNOIDAL
Solitary wave theory (Cnoidal 1st)
STOKE5
Stokes 5th order theory
GRID
Grid wave
STREAMn Stream function theory of order n (3 ≤ n ≤ 9)
height
: wave height. (Real)
period
: wave period in seconds. (Real)
direction : wave direction. (Real)
NEWW
: keyword to denote the New Wave wave model is to be used
crest
: maximum crest elevation measured from the mean water level. (Real)
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-59
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
IRRE
: keyword to denote an irregular wave spectrum is to be used.
sigheight : significant wave height of the spectrum. (Real)
Notes
1.
Direction and elevation are in the ‘water’ axis system. Direction is in degrees around the water Zw axes,
zero degrees being in the positive Xw direction and ninety degrees being in the positive Yw direction.
Yw
Wave Direction
q
2.
3.
Xw
For backward compatibility, the theory may be given as an integer with the following correspondence:
1
AIRY
2
CNOIDAL
5
STOKES
10
GRID WAVE
-n
Stream function theory of order n
New Wave is a dispersive wave, i.e. it is not cyclic as with the other deterministic waves. The crest
height given is the maximum that can occur when the linear wavelets which constitute the wave are all in
place at their respective peaks.
4.
Irregular wave, by definition, is a dispersive wave, i.e. it is not cyclic as with the other deterministic
waves.
5.
For a user defined wave spectrum (i.e. UDEF specified in the SPECTRAL command), the significant
wave height is computed from the area under the defined spectrum. In this case, sigheight specified here
is used for the stretching depth calculation only.
M.6.47 WIND Command
The WIND command enables wind loading to be input on members above the water surface. This command is
optional, but if omitted no wind loads are applied.
WIND
v elocity
direction
density
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-60
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Parameters
WIND
: keyword
velocity
: wind velocity. (Real)
direction : wind direction. (Real)
density
: mass density of air. (Real)
Notes
1.
Direction is in the ‘water’ axis system. Direction is in degrees around the water Zw axes, zero degrees
being in the positive Xw direction and ninety degrees being in the positive Yw direction.
Yw
Wind Direction
q
2.
Xw
The wind velocity is assumed constant for all elevations. Should a variation with elevation be required
this can be modelled by modifying the drag coefficients of the appropriate elements.
M.6.48 WPAR Command
This command permits user control over the default parameters adopted for the NewWave and/or irregular wave
computations. Unless guided otherwise, it is suggested that the default values embodied within WAVE are
adopted.
WPAR
STRETCH
dsa
DELTA
delta
SPREAD
alpha
SHIFT
theta
OFFSET
offset
EVOLVING
WAVELET
nw av e
SEED
iseed
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-61
ASAS (Non-Linear) User Manual
Appendix M - Wave Loading
Parameters
WPAR
: keyword
STRETCH : keyword to indicate that the delta stretching depth parameter is to be defined. If this parameter is
not defined a default value of 0.5 is used (New Wave and irregular wave)
dsa
: stretching depth factor. (Real). Stretching begins at a depth of dsa.Hs below the mean water
level (MWL) up to the water surface, where Hs is the maximum crest elevation or significant
wave height measured from MWL and is specified in the WAVE command. No stretching
occurs below this depth, or if the wave surface is below MWL
DELTA
: keyword to indicate that the delta stretching parameter is to be defined. If this parameter is not
defined a default value of 0.3 is adopted (New Wave and irregular wave)
delta
: delta parameter. (Real). A value of 0.0 corresponds to Wheeler stretching under wave crests, 1.0
corresponds to linear extrapolation of kinematics at mean water level to crest (0.0 ≤ delta ≤ 1.0)
SPREAD
: keyword to indicate that the wave spreading constant is to be defined. If this parameter is not
defined no wave spreading will be considered (alpha = 0.0). See Note 2 below. (New Wave
only)
alpha
: wave spreading constant in degrees (0.0 ≤ alpha ≤ 40.0). (Real)
SHIFT
: keyword to indicate that a common phase shift is to be applied to all the component wavelets. If
this parameter is not defined then no phase shift will be applied, and all the wave frequency
components will come into phase at x = t = 0.0 (New Wave only)
theta
: phase shift to be applied in degrees. (Real)
OFFSET
: keyword to denote an offset is to be applied to an evolving wave to define where the wave crests
come into phase along the direction of wave propagation. If this parameter is not defined for an
evolving wave then no offset will be applied (New Wave only)
offset
: offset distance from the origin in the direction of the wave. (Real)
EVOLVING
:
keyword to indicate that an evolving wave is required. If this keyword is not specified
then a non-evolving wave is generate (New Wave only)
WAVELET : keyword to denote the number of regular wavelets to be used to model the wave spectrum. If this
parameter is not defined, the default value is 50 (New Wave and irregular wave)
nwave
: number of regular wavelets used to model the wave spectrum (1 ≤ nwave ≤ 1000) (Integer)
SEED
: keyword to denote the random seed is to be defined. If this parameter is not defined, the default
seed is 1
iseed
: seed to start the generation of random phases (Integer)
Notes
1.
Before utilising any of the options described above for shell New Wave, the user is directed to Reference
NO TAG
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-62
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
2.
The SPREAD constant alpha is used to modify the horizontal wave kinematics for nearly uni-directional
seas. It must not be confused with the SPREAD command used for API analyses which utilises a quite
different parameter and methodology to determine the spreading characteristics.
3.
The SPREAD command must not be used in conjunction with the NewWave model.
Example
WPAR
SPREAD
WPAR
WPAR
EVOLVING
WAVELET 100
10.0
M.6.49 XMAS Data
This facility enables distributed masses such as that due to the effects of internal fluids where buoyancy loading
is being ignored. Extra mass is input per unit length of each selected element.
XMAS
ELEM
elem
GROU
group
PROP
prop
mass
ALL
Parameters
XMAS
: keyword
mass
: extra mass per unit length. (Real)
ELEM
: keyword to indicate element selection
elem
: list of user element numbers. (Integer)
GROU
: keyword to indicate group selection
group
: list of group numbers. (Integer)
PROP
: keyword to indicate geometric property selection
prop
: list of geometric property numbers. (Integer)
ALL
: keyword to indicate selection of all elements
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-63
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
Notes
1.
Extra mass may be specified per element using the AMAS command.
2.
Masses are not cumulative. Subsequent XMAS definitions for a particular element will overwrite
previous values.
3.
AMAS may be specified in addition to XMAS for a given element.
M.6.50 ZONE Data
ZONE
zonename
limname
limit
The ZONE command defines the limits of a specified zone in any or all of the X, Y and Z directions.
Parameters
ZONE
: keyword
zonename
: name of zone (up to 32 alphanumeric characters)
limname
: keyword which may be one of the following:
XMIN, XMAX, YMIN, YMAX, ZMIN, ZMAX
limit
: coordinate value associated with the corresponding limname. Values must be specified in the
water axis system. (Real)
Notes
1.
Undefined values are assumed to be at +/- infinity.
2.
The zonenames can be used with the DRAG, MASS and GROW commands.
Examples
ZONE
ZONE1
ZMIN
-2.0
ZONE
ZONE2
ZMIN
1.5
ZMAX
ZMAX
27.5
31.7
YMAX
147.5
XMIN
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
-25.5
Page M-64
Appendix M - Wave Loading
ASAS (Non-Linear) User Manual
M.7
Valid Options Controlling Wave Load Calculation
In addition to the options listed below, which affect the WAVE or MASS run, options which are valid for ASAS
will also be accepted but no action will be taken. For further details see the ASAS User Manual.
Option
Name
Application
HYDR
Requests detailed elemental hydrodynamic information for each wave case. This is useful
for ensuring that complex data assignments have been correctly applied.
APIW/AP20
Selects analysis to the requirements of API RP2A.
MCON
For current loads (CURR, TIDE, PCUR) vary the current profile to maintain mass
conservation. The input current profile must relate to the still water. The velocities are
scaled with depth to give a constant transfer of mass, for the instantaneous surface height,
whilst retaining the overall shape of the profile.
This is not recommended for use with API analyses.
RELC
For current loads (CURR, TIDE, PCUR) vary the current profile such that the velocities are
not at absolute depths, but relative depths. This does not give mass conservation. The
current velocities at x% of the water depth are the same for still water as for water with
waves.
APIC
For current loads (CURR, TIDE, PCUR) vary the current profile using non-linear
stretching as recommended in the API RP2A Code of Practice. The relationship is
given by
z = z′ + η
where
sinh (2π (z′ + d) / λ n
sinh (2π d/ λ n )
z
is the elevation of the point of interest
z’
is the effective elevation corresponding to z
d
is the still water depth
λn
is the wave length
η
is the wave surface elevation above the point of interest
z, z’, η are measured from the mean still water level
This is the default option when APIW is selected.
VEXT
For current loads (CURR, TIDE, PCUR) the current profile is not modified in the presence
of a wave, simple vertical extrapolation is used above still water level.
This is the default option for all non-APIW analyses, and is provided to override the
standard non-linear stretching when APIW is active.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-65
ASAS (Non-Linear) User Manual
BRIG
Appendix M - Wave Loading
The default method of calculating buoyancy loads is to determine the volume of fluid
displaced by a member and to apply the equivalent force as a distributed load in an upward
direction ( z - water ). An alternative approach is available using the BRIG option. With this
more rigorous approach the hydrostatic forces are calculated at the member ends and are
applied as nodal forces in the direction of the member. Thus all components of hydrostatic
force are included.
CONV
API RP2A states that the convective acceleration components of the wave kinematics
should be ignored.
If APIW option is selected the convective acceleration terms are
removed by default. The CONV option allows these terms to be included when APIW is
operative. For all non-APIW analyses this is the default.
RVOF
The wave drag forces in a transient analysis are calculated using the relative velocity
formulation of Morison’s equation by default. This option switches off the relative velocity
effect, thus ignoring the structural velocities in the load calculations
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-66
ASAS (Non-Linear) User Manual
Appendix M - Wave Loading
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page M-67
Appendix N
ASAS (Non-Linear) User Manual
Appendix - N
N.1
Heat Analysis
Introduction
Heat analysis is used to determine the temperature distribution on a structure. ASAS(NL) is capable of
modelling all three major modes of heat transfer: conduction, convection and radiation. ASAS(NL) can
perform both steady state and transient heat analyses.
N.2
Heat Equations
The finite element transient thermal equations can be written in the form:
C
dT
+HT = F
dt
where C is the heat capacity matrix, H is the conductivity matrix, F is the applied heat flux vector and T is
the nodal temperature vector. Both C and H can be functions of temperature and the equations will become
non-linear in such circumstances.
Discretising the governing equations in time, the nodal temperatures can be solved incrementally in time by
the direct time integration method as follows:
dT n+1
+ HT n+1 = F n+1
dt
dT
dTn
+ γ h n +1 ]
Tn +1 = Tn + ∆t[(1 - γ h )
dt
dt
C
where the subscripts n and (n+1) denote the step number, ∆t is the time step and
Yh is
the transient thermal
time integration parameter.
The time integration parameter Υh controls the accuracy and stability of the solution. For linear problems,
the solution is unconditionally stable if 1/2 ≤γh ≤ 1. The scheme with γh = 1/2 is called the Crank-Nicholson
scheme or the trapezoidal rule. It is second order accurate but may suffer from wild oscillations. The
choice γh = 1 is called the backward Euler scheme. It provides the desirable numerical damping to damp
out the unwanted oscillations but is only first order accuate. The backward Euler is the only scheme that is
unconditionally stable in non-linear problems. In ASAS(NL), the default setting for γh is 1.0, i.e. the
backward Euler scheme. Other setting may be specified using parameter HGAMMA in the TEMP
command. The HGAMMA value specified must be between 0.5 or 1.0 or else a warning will be flagged and
the value of HGAMMA will be reset to the nearest value in the valid range.
For steady state problems, the governing equations simplify to the form:
HT = F
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page N-1
ASAS (Non-Linear) User Manual
Appendix N
This form is identical to that for a static stress analysis and thus both can be solved using the same nonlinear solution procedure.
N.3
Convection
The heat flow per unit area for a general convection law is given by:
q = h (T2 - T1)r
where h is the film coefficient, r is the power index of the heat tranfer law, T1 and T2 are temperatures on
surfaces 1 and 2.
This heat transfer law is implemented as material CVEC in ASAS(NL) (see Sec 5.2.4.1.10). At present,
CVEC material can only be used with FAT2 element.
N.4
Radiation
The heat flow per unit area for radiation is given by:
q=σε(Τ24-Τ14)
where σ is the Stefan-Boltzmann constant, ε is the effective surface emissivity, Τ1 and Τ2 are temperatures
on surfaces 1 and 2. Note that Τ1 and Τ2 are values relative to absolute zero temperature.
In general, the effective surface emissivity is equal to the product of surface emissivity on both surfaces, i.e.
ε = ε1.ε2. If the two surfaces are directly opposed and close to each other, the effective emissivity is given
by:
ε=
ε 1ε 2
ε 1+ ε 2- ε 1 ε 2
This heat transfer law is implemented as material RADI in ASAS(NL) (see Sec 5.2.4.1.11). At present,
RADI material can only be used with FAT2 element.
N.5
Controlling a Heat Analysis
The following run control information is relevant for a heat analysis:
1.
A steady state job is invoked by setting job type to HEAT in the JOB command. The job type
should be set to HTRA for a transient heat job.
2.
Only field element types are valid for heat analysis but the program will also accept stress elements
defined in the element topology deck and automatically convert them into corresponding field
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page N-2
Appendix N
ASAS (Non-Linear) User Manual
elements (e.g. BRK8 beomces BRT8). This conversion is carried out as soon as all the element
topology data are read in and therefore all the material and geometric properties data supplied must
refer to the field element type.
3.
Three different types of heat input (c.f. loading in stress analysis) may be specified in a heat analysis.
These are nodal flux, prescribed field variable and flux density.
4.
In transient thermal analysis, the initial temperature distribution on the structure is defined in the
INIT data block. All nodes without initial condition specified (including those with prescribed
temperatures) are assumed to have an initial temperature equal to the reference temperature
TREFLD. If any non-zero initial condition (heat flux or temperature) is specified, a solution should
be performed at the initial time in order to provide a consistent set of starting conditions for the time
integration process.
5.
The parameter TREFLD specifies the temperature assumed initially at all nodes on the model for
evaluating the material properties and hence the conductivity matrix. If not given, TREFLD is
assumed to be zero.
6.
The parameter TAZERO specifies the absolute zero temperature. By default, TREFLD is assumed
to be equal to -273.15, which is consistent with temperature measures specified in Centigrade. If
other temperature units are used in an analysis, the absolute zero temperature in the appropriate units
must be defined using the PARA TAZERO command in order to incorporate the radiation effect
correctly.
7.
Option LOWE reduces any higher order elements defined in the data to their corresponding low
order element types (e.g. BT20 becomes BRT8). In this case, however, any reference to element
mid-side nodes in the boundary conditions or load data is also invalid.
8.
Option SURF asks the program to use the surface temperatures on the structure to determine
temperature dependent material properties. If not specified, the average element temperature will be
assumed instead. This option only has effect on FAT2 elements with FLNS option or CVEC/RADI
material.
9.
Units command will only have effect on input variables with temperatue or length units. All heat
associated properties (e.g. conductivity) do not have units conversion facility implemented and
therefore they must be supplied in consistent units.
N.6
Saving Heat Analysis Results
Like all other analysis types, the results from a thermal analysis can be saved using the RESU command.
The table below shows the types of results saved together with the keywords required.
Result name
Keyword on RESU
Result type on database
Temperature
DISP
FIELD VARIABLE
Temperature rate
VELO
VELOCITY
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page N-3
Appendix N
ASAS (Non-Linear) User Manual
Heat flux
STRS
FLUX
Heat field
STRN
FIELD
Reactive heat flow
REAC
REACTION
N.7
Interfacing with Stress Analysis
A thermal analysis is very often followed by a stress analysis that studies the effect of thermally induced
stresses on the structure. A facility is available in the program to allow import of temperature distribution
obtained in a heat analysis into the subsequent stress analysis.
In the stress analysis, the temperature results are read in from the results database via a GRES command
within the nodal temperature (i.e. TEMPERAT) data block (see Sec 5.4.7.1). In order to use this feature, it
is essential to have the temperature results saved using RESU in the thermal analysis.
It is also a requirement that the thermal and stress runs must come from the same project. This means that
the stress job must be an old job, i.e. JOB OLD, with the same project name as defined in the thermal run.
As the results database file is standard across the ASAS suite, the stress job can be performed using either
ASAS or ASAS(NL).
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Page N-4
ASAS (Non-Linear) User Manual
Appendix - O
Wind Turbine
O.1
Appendix O
Coupled Wind and Wave Load Analysis of Offshore
Introduction
This Appendix describes the facilities available within ASAS(NL) that enable it to perform integrated
wind and wave load analyses for offshore wind turbines with a specialised wind loading software
package called Flex 5. The purpose of using ASAS(NL) is to provide a realistic foundation model that
can accurately model the foundation structural behaviour under the influence of wave loading. Note that
foundation here refers to the whole sub-structure that is under the influence of wave loading, i.e. from the
sea surface down.
The Appendix is presented as an addendum to the main ASAS-NL User Manual, and reference should be
made to the main sections of that manual where appropriate.
The following sections are included:
The Analysis .................................................................................................................. O.2
Data for FLXG job ......................................................................................................... O.3
JOB command ................................................................................................................ O.3.1
Generalized Mode Definition ......................................................................................... O.3.2
Output from FLXG job .................................................................................................. O.4
Generalized Matrix Files ................................................................................................ O.4.1
Generalized External Force File..................................................................................... O.4.2
O.2
The Analysis
The integrated wind and wave load analysis is carried out with the following series of runs:
1.
An initial ASAS(NL) static analysis of the foundation structure is carried out to determine the
deflected shapes that define the transformation between nodal freedoms of the foundation model
and the generalized freedoms required by Flex 5 In this run, unit deflection and rotation load cases
(a total 6 cases) are applied at the foundation top node
using normal ASAS prescribed
displacement loading data. Displacements from these load cases form the transformation matrix
and therefore these must be saved to the database using the RESU DISP command to ensure that
they can be assessed in the subsequent runs
2.
A second ASAS(NL) analysis is run to produce the generalized mass, damping and stiffness
matrices of the foundation structure together with a time series of the generalized foundation
external loading. Wave and other external loadings on the foundation are applied as normal
loading data in this run. The generalized matrices are written to 3 separate files (one each for
mass, damping and stiffness) and the generalized load time series is written to another file. The
job type of this analysis is called FLXG to indicate its special nature.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
O-1
ASAS (Non-Linear) User Manual
3.
Appendix O
A Flex 5 solution is then carried out with the foundation effects included through utilising the
generalized matrices and loading vector derived in step 2. The forces or displacements at the
foundation top node at each solution time step are written to a file.
4.
A final ASAS(NL) analysis is performed to recover the member forces in the foundation structure
by applying the foundation top node force or displacement time series obtained from Flex 5
together with the foundation external loading as specified in step 2. The analysis can be carried
out statically or dynamically.
•
The transformation matrix required in the FLXG job is formed from the displacements of unit
deflection load cases in the initial static analysis. In order to read back these results, both runs
must come from the same project. This means that the FLXG job must be an old job, i.e. job
status is either OLD or REPL, with the same project name as specified the initial static run.
•
The generalized matrices (stiffness etc) are computed based on the initial undeformed
geometry and assuming small displacement, linear behaviour. It is thus implicitly assumed that
the foundation is linear with small deformations throughout the entire solution.
•
Likewise, when computing the generalized foundation external load time history in step 2, it is
assumed that the structural displacement and velocity are zero since such information is not
available when the loading is generated.
•
The hydrodynamic mass in ASAS(NL) is formed assuming that the water elevation is at the
still water level.
•
If the foundation internal forces are recovered statically in step 4, the dynamic forces (e.g.
inertial force) in the foundation will be ignored. The dynamic effects can be accounted for by
running this step as a transient job. However, it should be noted that the following effects may
affect the accuracy of the solution: The following points should be noted for this analysis
approach:
1.
The generalized mass used in Flex 5 is only an approximation to the true mass matrix
(static reduction is exact but not dynamic).
2.
Different time integration schemes are adopted by Flex 5 and ASAS(NL). Hence,
while the displacement time histories are identical in both runs (for the prescribed
displacement case), it may not be the case for the velocity and acceleration time
histories.
•
There should be little difference between applying forces or displacements to recover the
foundation forces. The two methods should yield identical results in a linear static analysis.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
O-2
ASAS (Non-Linear) User Manual
O.3
Appendix O
Data for FLXG job
The following commands and data sets are supplement to those required for undertaking a conventional
structural analysis. Reference should be made to Section 5 of this manual for the main data definitions.
O.3.1 JOB Command
Defines analysis type and for restart jobs the old archive file name and required checkpoint number on
the old archive file. Compulsory.
oldarch
(OLD)
(REPL)
JOB
(nchkpt)
Parameters
JOB
: compulsory keyword
OLD
: optional keyword indicating that this run will add to an existing project database
REPL
: optional keyword indicating that this run will replace a previous run of the same structure
on the project database
FLXG
: keyword indicating an analysis to generate data for Flex 5
oldarch
: old archive name up to 8 characters. This is only required for restarts.
(nchkpt) : number of the required restart checkpoint on the old archive file (brackets must appear). If
omitted the highest checkpoint on the old archive file is taken. This is only required for
restarts. (Integer)
Notes
1.
The default project status for FLXG job is old.
O.3.2 Generalized Mode Definition
This data defines the generalized modes. The data block must be the last in the data file before the STOP
command.
TVEC
sname
lc
(isub)
END
Parameters
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
O-3
ASAS (Non-Linear) User Manual
Appendix O
TVEC
: compulsory header keyword to denote the start of the generalized mode definition data
sname
: 4 character structure name that contains deflected shape of the generalized mode.
lc
: user load case number where displacements are required. (Integer)
isub
: load sub-case number. Default is 0. (Integer)
END
: compulsory keyword to denote the end of the generalized mode definition data
Notes
1.
Since the foundation has six generalized degrees of freedom in Flex 5, there should always be six
modes defined in the TVEC data.
2.
The defined generalized mode must have been saved in a previous analysis under the same
project.
3.
The model used for generating the generalized modes must have identical structural properties
with the model created in the present analysis.
4.
The order in which the load cases are specified defines their order in the transformation matrix,
i.e. the first load case defines the first generalized mode etc.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
O-4
ASAS (Non-Linear) User Manual
Appendix O
Example
An example of utilising the displacements from user load cases 1 to 6 of structure S001 as the
generalized modes.
TVEC
S001
S001
S001
S001
S001
S001
END
O.4
1
2
3
4
5
6
0
0
0
0
0
0
Output from FLXG job
Four formatted ASCII files will be generated from each FLXG job. These are:
4.
5.
xxxx.gnm
xxxx.gnc
generalized mass matrix file
generalized damping matrix file
6.
xxxx.gnk
generalized stiffness matrix file
7.
xxxx.gnf
generalized external force time series file
where xxxx is the 4 character structure name of the FLXG job that produces the files.
O.4.1 Generalized Matrix Files
In the very first load step, the generalised mass, damping and stiffness matrices are calculated and written
to 3 separate files. The files are written with the following format:
ngenfr
(val(i,1), i=1,ngenfr)
(val(i,2), i=2,ngenfr)
.
.
(val(i,ngenfr), i=1,ngenfr)
(1x, I6)
(6(1x,E12.5))
(6(1x,E12.5))
(6(1x,E12.5))
where ngenfr is the number of generalized freedoms, which is always 6 at present and val is the
generalized matrix.
The row and column order in the generalized matrix corresponds to the order in which the generalized
modes are defined in the TVEC data.
Note that there is currently a restriction that the generalized damping matrix ignores contributions from
damping specified for the spring elements SPR1/2.
O.4.2 Generalized External Force File
A time series of the generalized foundation external loading vector is written to a force file. At each
solution time, the time (t) and the associated generalized load vector (f) will be output to this file. The
force file has the following format:
ngenfr
t1
(f1(i), i=1,ngenfr)
t2
(f2(i), i=1,ngenfr)
.
(1x, I6)
(1x,E12.5)
(6(1x,E12.5))
(1x,E112.5)
(6(1x,E12.5))
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
O-5
ASAS (Non-Linear) User Manual
.
.
.
tn
(fn(i), i=1,ngenfr)
Appendix O
(1x,E12.5)
(6(1x,E12.5))
As before, the load values are ordered in the same way as the columns of the transformation matrix are
arranged.
Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
O-6