Siemens SINUMERIK 840D sl Programming Manual page 360

Fundamentals
2.14 Supplementary commands
FP=:
Note
Multiple axes can be programmed in one G75 block. The axes are then traversed
simultaneously to the specified fixed point.
Note
The value of the address FP must not be greater than the number of fixed points specified for
each programmed axis (MD30610 $MA_NUM_FIX_POINT_POS).
Example
For a tool change, axes X (= AX1) and Z (= AX3) need to move to the fixed machine axis
position 1 where X = 151.6 and Z = -17.3.
Machine data:
● MD30600 $MA_FIX_POINT_POS[AX1,0] = 151.6
● MD30600 $MA_FIX_POINT[AX3,0] = 17.3
NC program:
Program code
...
N100 G55
N110 X10 Y30 Z40
N120 G75 X0 Z0 FP=1 M0
N130 X10 Y30 Z40
...
360
Fixed point that is to be approached
Fixed point number
<n>:
Range of values:
Note:
In the absence of FP=<n> or a fixed point number, or if FP=0 has been
programmed, this is interpreted as FP=1 and fixed point 1 is approached.
Comment
; Activate settable zero offset.
; Approach positions in the WCS.
; The X axis moves to 151.6
; and the Z axis moves to 17.3 (in the MCS).
; Each axis travels at its maximum velocity.
; No additional movements are permitted to be active in
this block.
; A stop is inserted here so that after reaching
; the end positions,
; no additional motion takes place.
; The position of N110 is approached again.
; The zero offset is reactivated.
1, 2, 3, 4
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming