Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 324)

Coordinate System Offsets
Chapter 11
11-8
Where : Is :
L2 tells the control that you want to alter the coordinate system tables.
P specifies which coordinate system (G54 through G59.3) you want to work on. P1
through P9 correspond to the work coordinate systems G54 through G59.3.
P1 = G54 work coord. system P6 = G59 work coord. system
P2 = G55 work coord. system P7 = G59.1 work coord. system
P3 = G56 work coord. system P8 = G59.2 work coord. system
P4 = G57 work coord. system P9 = G59.3 work coord. system
P5 = G58 work coord. system
X_Y_Z_ specify the location of the zero point of the specified work coordinate system
relative to machine coordinate system.
Important: G10 blocks may not be programmed when TTRC is active.
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
G54X25.Y25.; X25 Y25 X50 Y45
G91;
G10L2P1X10.Y10.; X15 Y15 X50 Y45
G90;
G10L2P1X3O.Y35.; X15 Y15 X50 Y45
Important: This modification is permanent. The new table values for the
work coordinate systems are saved even when the control power is turned
off.