Rockwell Automation 8520-GUM 9/Series CNC Grinder Operation and Programming Manual Documentation Set - Manual (Page 325)

Chapter 11
Coordinate Control
11-9
Incremental/Absolute Mode and the G10L2 Command
When you program in incremental mode (G91), any values entered into
the work coordinate system table using the G10 command are added to the
currently active work coordinate system values. When you program in
absolute mode (G90), any values entered into the work coordinate system
table using the G10 command replace the currently active work coordinate
system values.
Example 11.3 and Figure 11.7 illustrate how the work coordinate system is
shifted using G10.
Example 11.3
Work Coordinate System Shift Using G10
Program block Work coordinate Position Absolute coordinate Position
G54G01X25.Z25.;
G91;
G10L2P1O2X10.Z10.; X25 Z25
X15 Z15
X50 Z45
X50 Z45
or
G54G01X25.Z25.;
G90;
G10L2P1O2X35.Z30.; X25 Z25
X15 Z15
X50 Z45
X50 Z45
Important: This modification is permanent. The control saves the new
table values for the work coordinate systems even when control power is
turned off.
Figure 11.7
Results of Example 11.3
Wheel position
G54 Work coordinate system
after changing table value
Machine coordinate system zero point
20 30 40 50
G54 Work
coordinate system
Z
X
X
X
Z
Z
15
25
15 25
20
30
40
50
12173-I