Download User Manual

GSK928MA CNC SYSTEM OPERATION MANUAL
3
3.1
G Function (Preparatory Function)
G Function for Defining Programming State of the System
Programming state of system is specified by these G functions as follows. They are modal which
means they are valid unless the programming state is changed. The initial is the programming state
that the part program is to be executed. The following G can be used in one program block with
other G functions and at most 6 G functions can be used in the same block.
G17 — Initial state, select X-Y plane for circular interpolation
G18 — Select Z-X plane for circular interpolation
G19 — Select Y-Z plane for circular interpolation
G40 — Initial state, cancel tool radius compensation
G43 — Tool length compensation +
G44 — Tool length compensation –
G49 — Initial state, cancel tool length compensation
G54 — Initial state, select the 1st workpiece coordinate system
G55 — Initial state, select the 2nd workpiece coordinate system
G56 — Initial state, select the 3rd workpiece coordinate system
G57 — Initial state, select the 4th workpiece coordinate system
G58 — Initial state, select the 5th workpiece coordinate system
G59 — Initial state, select the 6th workpiece coordinate system
G80 — Initial state, cancel the modal data of fixed cycle (use G98 instruction simultaneously)
G90— Initial state, do programming with absolute coordinate. X, Y, Z word values mean the
absolute coordinate values.
G91— programming with incremental coordinate. X, Y, Z word values mean the incremental
coordinate values (the increment relative to the starting point of the current block).
G94— Initial state, set the feedrate per minute. The unit of cutting feedrate set by F word is
mm/min, i.e. the millimetres of feeding per minute
G95 — Set the feedrate per rev. The unit of cutting feedrate set by F word is mm/r, i.e. the
millimetres of feeding per rev of spindle. The spindle pulse encoder (1200 pulses per rev)
must be fixed firstly before using G95 function.
G98 — Initial state, return to the start plane in fixed cycle.
G99 — Return to the R reference plane in fixed cycle.
G09，G60，G61，G64 ：Invalid compatible function.
3. 2
G0 Rapid Positioning (Modal, Initial)
Format : N_ G0 X _Y_ Z _ C_( or A_)↙
X, Y,Z, C(or A) is the coordinate absolute value (G91) or relative value(G90) of end point to be
positioned in work coordinate system. The needless axis can be omitted. The rapid traverse speed
is specified by parameter No.1 and can be modified by pressing parameter key. The sequence of
positioning is as follows:
Position Z, X, Y, 4th axis in turn when Z axis is positive (the cutter rising off the workpiece).
14