Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 309)

Chapter 11
Coordinate System Offsets
11-3
Although axis motion is usually commanded in the work coordinate
system, axis motion is possible when a G53 is programmed in a block if
you reference coordinate values in the machine coordinate system.
G90G53X___Z___;
The X- and Z-words above specify coordinate positions in the machine
coordinate system. These coordinate values indicate the end point of the
next move in the machine coordinate system. The tool travels to this
position in either G00 or G01 mode, depending on which is active when
the G53 block is executed. Any attempt to execute a G53 block in G02 or
G03 mode generates an error.
The G53 code is not modal. It is effective only in the block in which it is
called. After a G53 block, the control returns to the coordinate system that
was in effect prior to the G53 blocks execution.
Important: The control must be in absolute mode (G90) when the G53
command is executed. If a G53 is executed while in incremental mode
(G91), the control ignores the G53 code and any axis words in the G53
block.
Example 11.1
Motion In The Machine Coordinate System.
Program block Comment
N1 G00X30Z30; axis motion in work coordinate system.
N2 G53X25Z10; axis motion in machine coordinate system.
N3 X20Z50; axis motion in work coordinate system.
11.1.1
Motion in the Machine
Coordinate System (G53)