Siemens CNC Milling | G75 Code | Fixed Point Approach

G75 Code Introduction

By using G75 code, 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.

G75 Code Format

G75 FP=<n> X=0 Y=0 Z=0

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.


G75 : Fixed point approach
FP=<n> : Fixed point that is to be approached. The fixed point number is specified: <n> Value range of <n>: 1, 2, 3, 4 ; MD30610$NUM_FIX_POINT_POS should be set if fixed point number 3 or 4 is to be used. If no fixed point is specified, fixed point 1 is approached automatically.
X=0 Y=0 Z=0 : 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.

G75 Code Example

N05 G75 FP=1 Z=0 ; Approach fixed point 1 in Z
N10 G75 FP=2 X=0 Y=0 ; Approach fixed point 2 in X and Y, e.g. to change a tool
N30 M30 ; End of program

Note: The programmed position values for X, Y, Z (any value, here = 0) are ignored, but must still be written.