Siemens SINUMERIK 802D sl Programming Manual page 48

Movement Control Commands
3.1 The coordinate system
p=1 to 93:
X, Y, Z:
Changing by G92:
G92 X... Y... Z... ;
Explanations
Changing by using G10
Each workpiece coordinate system can be changed separately by using the G10
command.
If G10 is executed in the main run, G10 must execute an internal STOPRE com-
mand before writing the value.
In MD $MC_EXTERN_FUNCTION_MASK Bit 13, you can configure whether the
G10 command shall execute an internal STOPRE. The machine data bit affects all
G10 commands in ISO--Dialect--T and ISO--Dialect--M.
Changing by using G92
A workpiece coordinate system (selected with a code from G54 to G59 and G54
P{1 ...93}) is shifted to set a new workpiece coordinate system by specifying G92
X... Y... Z.... This way, the current tool position is made to match the specified
coordinates. If X, Y, Z, is an incremental command value, the work coordinate
system is defined so that the current tool position coincides with the result of
adding the specified incremental value to the coordinates of the previous tool
position (coordinate system shift). Subsequently, the value of the coordinate sy-
stem shift is added to each individual workpiece zero point offset value. In other
words, all of the workpiece coordinate systems are systematically shifted by the
same value amount.
3-48
Workpiece zero point offset value correspond to workpiece coordi-
nate system G54 P1 ... P93
For an absolute command (G90), workpiece zero point offset for
each axis.
Value to be added to the set workpiece zero point offset for each
axis in case of an incremental command (G91).
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) - - 04.07 Edition
© Siemens AG 2007 All rights reserved
04.07