Rockwell Automation 8520-GUM 9/Series CNC Grinder Operation and Programming Manual Documentation Set - Manual (Page 331)

Chapter 11
Coordinate Control
11-15
Example 11.5
Work Coordinate System Offset (G92)
Program Block Comment
G54 G00; G54 work coordinate system.
X35. Z25.; Rapid move to X35, Z25 in the G54
work coordinate system.
G92X10.Z10.; Redefines current axis position to have
the coordinates X10, Z10
The zero point of the offset G54 work coordinate system is 10 units away
from the current wheel location in both the X and Z directions. If the Z
value had not been entered in the G92 block, the Z coordinate location
would have remained unchanged (Z25).
Figure 11.10
Results of Example 11.5
Machine coordinate system zero point
Zero point for the G54
work coordinate system
New zero point established
by the G92 block
10
20 30
10
30
20
wheel position
Z
Z
X
X
12176-I
ATTENTION: G92 offsets are global. This means that
changing from one coordinate system to another does not cancel
the offset. Do not program a change in coordinate systems
(G54-G59.3) unless the effects of the offset have been
considered.