Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 317)

Chapter 11
Coordinate System Offsets
11-11
There are 3 methods to change the value of an external offset in the work
coordinate system table. Two methods can be found in the following
sections:
Method: Chapter:
manually alter the external offset value in the work
coordinate system table
3
alter the paramacro system parameter values 5201- 5206 28
The third method, and the one described in this section, alters the external
system table through G10 programming. Changing these values in the
table using any of these methods does not cause axis motion. It does
immediately shift the active coordinate system by the amount entered.
The values entered into the external offset are added to the work coordinate
system zero point values each time a work coordinate system is called.
The format for altering the external offset using G10 is:
G10 L2 P0 O__ X__ Z__;
Where : It :
L2 tells the control that you want to alter the coordinate system tables.
P0 designates the external offset as the offset to update.
O__ specifies whether the value entered for the diameter axis is a radius or diameter
value. (O is non-modal.)
O1
=value entered for the diameter axis is a radius value.
O2 =value entered for the diameter axis is a diameter value.
Important: If you program O1 or O2 in a G10 code, the G10 code is not
affected by a previously programmed G07 or G08 (radius/diameter
programming). However, if no O-code is specified, or if the O-code is out of
range (for example, O3), then the G10 code is affected by a G07/G08.
X_Z_ specifies the location of the zero point of the specified work coordinate system
relative to machine coordinate system.
When you execute this block, the control immediately shifts the currently
active work coordinate system by the new external offset amount.
Example 11.4 and Figure 11.9 illustrate how the work coordinate system is
shifted using G10.
11.3.1
Altering External Offset
(G10L2)