Siemens SINUMERIK 840D sl Programming Manual page 398

Supplementary commands
14.5 Fixed-point approach (G75, G751)
Examples
Example 1: G75
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
...
Note
If the "Tool management with magazines" function is active, the auxiliary function T... or M...
(typically M6) will not be sufficient to trigger a block change inhibit at the end of G75 motion.
Reason: With "Tool management with magazines is active", auxiliary functions for tool
change are not output to the PLC.
Example 2: G751
Position X20 Z30 is to be approached first, followed by the fixed machine axis position 2.
Program code
...
N40 G751 X20 Z30 FP=2
...
398
Comment
; Activate adjustable work offset.
; Approach positions in workpiece coordinate system.
; The X axis moves to 151.6 and the Z axis moves to
17.3 (in the machine coordinate system). Each axis
travels at the maximum velocity it is capable of
reaching. No additional movements are permitted to
be active in this block. To continue to prevent any
additional movements once the end positions have
been reached, a stop is inserted here.
; The position of N110 is approached again. The work
offset is reactivated.
Comment
; Position X20 Z30 is approached first in rapid traverse
as a path. Then the distance from X20 Z30 to the
second fixed point in the X and Y axis is traversed,
as with G75.
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Fundamentals