Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 336)

Coordinate System Offsets
Chapter 11
11-20
5. Return to Automatic or MDI mode. When the <CYCLE START>
button is pressed, execution will continue from the new tool location,
at the jogged offset.
Important: When the jog offset move is made the axis position displays
do not change on the screen (unless the currently active screen is
displaying absolute position coordinates as described in section 8.1). This
is because the coordinate values in the work coordinate system are being
offset as the axes are being jogged.
The G92.1 command cancels the following offsets:
G92 work coordinate system offset
G52 zero point offset
{SET ZERO} offset
Jog offset
Reset G54 - G59.3 coordinate system to default condition
It will not cancel an external offset (see section 11.3).
The G92.1 block will also reestablish the default work coordinate system
as set in AMP by the system installer. It will cancel or activate the
coordinate system (G54-G59.3) as as set in AMP to establish the default
coordinate system.
The G92.1 block must be programmed with no axis words. Axis words in
a G92.1 block will generate an error. When the G92.1 block is executed all
G92, G52, {SET ZERO}, and Jog offsets are canceled on all axes. It is not
possible to cancel the offsets on only one or more of the axes.
No axis motion takes place during execution of a G92.1 block. Axes
remain at their last programmed position while the work coordinate system
is adjusted to remove all offsets.
The following example demonstrates the G92.1 offset cancel.
Example 11.9
G52 Offset Cancelled By a G92.1
Program Blocks Comment
N1 G01Y25.X25.; move to Y25, X25
N2 G52Y10.X10.; work coordinate system is offset by Y10, X10
N3 Y25.X25.; move to Y25, X25 in the offset coordinate system
N4 G92.1; G52 offset is cancelled, program position dis-
plays axis position at X35Y35.
11.4.5
Canceling Coordinate
System Offsets (G92.1)