Siemens Sinumerik 840D sl Programming Manual page 39

Format
Modified by G10:
G10 L2 Pp X... Y... Z... ;
p=0:
p=1 to 6:
X, Y, Z:
G10 L20 Pp X... Y... Z... ;
p=1 to 93:
X, Y, Z:
Modified by G92:
G92 X... Y... Z... ;
Explanations
Modified by G10:
G10 can be used to change each workpiece coordinate system individually. If the work offset
with G10 is to be written only when the G10 block is executed on the machine (main run
block), then MD20734 $MC_EXTERN_FUNCTION_MASK, Bit 13 must be set. An internal
STPPRE is executed in that case with G10. The machine data bits affect all G10 commands
in the ISO Dialect T and ISO Dialect M.
Modified by G92:
By specifying G92 X... Y... Z..., a workpiece coordinate system that was selected earlier with
a G command G54 to G59 or G54 P{1 ...93}, can be shifted and thus a new workpiece
coordinate system can be set. If X, Y and Z are programmed incrementally, the workpiece
coordinate system is defined in such a way that the current tool position matches the total of
the specified incremental value and the coordinates of the previous tool position (shift of
coordinate system). Finally, the value of the coordinate system shift is added to each
individual value of the workpiece work offset. To put it another way: All workpiece coordinate
systems are shifted systematically by the same value.
ISO Milling
Programming Manual, 06/09, 6FC5398-7BP10-1BA0
External workpiece work offset
The value of the workpiece work offset corresponds to the workpiece
coordinate system G54 to G59 (1 = G54 to 6 = G59)
Workpiece work offset for each axis during an absolute command (G90).
Value that must be added during an incremental command (G91) for each
axis to the specified workpiece work offset.
The value of the workpiece work offset corresponds to the workpiece
coordinate system G54 P1 ... P93. The number of work offsets (1 to 93)
can be set through MD18601 $MN_MM_NUM_GLOBAL_USER_FRAMES
or MD28080 $MC_MM_NUM_USER_FRAMES.
Workpiece work offset for each axis during an absolute command (G90).
Value that must be added during an incremental command (G91) for each
axis to the specified workpiece work offset.
Motion commands
3.1 The coordinate system
39