Download CNC PILOT 4290
Transcript
4.7 Turning Cycles Face roughing G820 G820 machines the contour area defined by “NS, NE.” The CNC PILOT uses the tool definition to distinguish between external and internal machining. With “NS – NE” you specify the machining direction. If the contour to be machined consists of one element, then: ■ If you program only NS, machining is in contour definition direction ■ If you program NS and NE, machining is against the contour definition direction If required, the area to be machined is divided into several sections, for example, for machining contour valleys. The simplest way of programming is specifying NS, NE and P. Parameters NS: Starting block number (beginning of contour section) NE: End block number (end of contour section) P: Maximum infeed I: Oversize in X direction (diameter value)—default: 0 K: Oversize in Z direction—default: 0 E: Approach behavior ■ E=0: Descending contours are not machined ■ E>0: Approach behavior ■ No input: Feed rate reduced depending on approach angle—maximum reduction: 50% X: Cutting limit in X direction (diameter value)—default: no cutting limit Z: Cutting limit in Z direction—default: no cutting limit H: Type of contour smoothing—default: ■ H=0: smoothing after each cut ■ H=1: lift off at under 45°, smoothing after last cut ■ H=2: lift off at under 45°, no smoothing A: Approaching angle (reference: Z axis)—default: 90°/270° (perpendicular to Z-axis) W: Departing angle (reference: Z axis)—default: 0°/180° (parallel to Z-axis) Q: Type of retraction after machining—default: 0 ■ Q=0: Return to starting point (first in X direction, then in Z) ■ Q=1: Position in front of finished contour ■ Q=2: Move to clearance height and stop V: Identifier beginning/end—default: 0 A chamfer/rounding arc is being machined: ■ V=0: At beginning and end ■ V=1: At beginning ■ V=2: At end Cycle run 1 Calculate the areas to be machined and the cutting segmentation (infeeds). 2 Approach workpiece for first pass from starting point, taking the safety clearance into account (first in X direction, then in Z). 3 Move at feed rate to target point X. 4 Depending on H: ■ H=0: Cut along the contour ■ H=1 or 2: Retract at 45° 5 Return at rapid and approach for next pass. 6 Repeat 3 to 5 until target point Z has been reached. 7 If required, repeat 2 to 6 until all areas have been machined. 8 H=1: Smoothen contour. 9 Retract according to “Q.” Cutting limitation: The tool position before the cycle call determines the effect of a cutting limit. The CNC PILOT machines the area to the right or to the left of the cutting limit, depending on which side the tool has been positioned before the cycle is called. Cutter radius compensation: Active G57 oversize: “Enlarges” the contour (also inside contours) G58 oversize: ■ >0: “enlarges” the contour ■ <0: is not considered G57/G58 oversizes are deleted after cycle end Continued 124 4 DIN PLUS
Related documents
CNC Pilot 4290
User manual
smart.Turn MANUALplus 620 / CNC PILOT 640
CNC Pilot 4290
354 100-22 - heidenhain
Oregon Scientific EW96 Clock User Manual
Robur Line F1 Series Specifications
XC100 Series Monitor & XT300 Series Dehydrator User Manual
D GB # 26 4251
1.0 Introduction - Case Western Reserve University
354 267-24 - heidenhain
Electronic sourcing system