Rockwell Automation 8520-GUM 9/Series CNC Grinder Operation and Programming Manual Documentation Set - Manual (Page 333)

Chapter 11
Coordinate Control
11-17
To offset a work coordinate system an incremental amount from its zero
point, program a G52 block that includes the axis names and distances to
be offset.
G52 X___ Z___ ;
The above command offsets the current work coordinate system by the
axis values that follow the G52 command.
Example 11.7
Work Coordinate System Offset by G52
Program Block Machine Coordinate Position Work Coordinate Position
G01X25.Z25.; X25 Z25 X25 Z25
G52X10.Z10.; X25 Z25 X15 Z15
In Example 11.7, no axis motion takes place when the G52 block is
executed; however, the work coordinate system position values change.
See Figure 11.12.
Figure 11.12
Results of Example 11.7
10
25 15
wheel position
10 25
15
Work coordinate system
after G52 offset
Original work coordinate system
X X
Z
Z
12178-I
The G52 work coordinate system zero point offset can be canceled by
programming a G52 block with zero values for the axes to be canceled.
The following block would cancel the work coordinate system offset for
the X axis only:
G52 X0;
11.4.2
Offsetting Coordinate Zero
Points (G52)