Fixed Point Approach: G75 - Siemens SINUMERIK 802D sl Programming And Operating Manual

Programming
10.3 Axis movements
10.3.6

Fixed point approach: G75

Functionality
By using G75, a fixed point on the machine, e.g. tool change point, can be approached. The
position is stored permanently in the machine data for all axes. A maximum of four fixed
points can be defined for each axis.
No offset is effective. The speed of each axis is its rapid traverse.
G75 requires a separate block and is non-modal. The machine axis identifier must be
programmed!
In the block after G75, the previous G command of the "Interpolation type" group (G0,
G1,G2, ...) is active again.
Programming
G75 FP=<n> X1=0 Y1=0 Z1=0
Note
FPn references with axis machine date MD30600 $MA_FIX_POINT_POS[n-1]. If no FP has
been programmed, then the first fixed point will be selected.
Table 10- 3
Command
G75
FP=<n>
X1=0 Y1=0 Z1=0
Programming example
N05 G75 FP=1 Z1=0
N10 G75 FP=2 X1=0 Y1=0
N30 M30
236
Explanation
Significance
Fixed point approach
Fixed point that is to be approached. The fixed point number is specified: <n>
Value range of <n>: 1, 2, 3, 4
If no fixed point is specified, fixed point 1 is approached automatically.
Machine axes to be traversed to the fixed point.
Here, specify the axes with value "0" with which the fixed point is to be
approached simultaneously.
Each axis is traversed with the maximum axial velocity.
; Approach fixed point 1 in Z
; Approach fixed point 2 in X and Y,
e. g. to change a tool
; End of program
Programming and Operating Manual, 11/2012, 6FC5398-5CP10-3BA0
Surface grinding