Rockwell Automation 8520-GUM 9/Series CNC Grinder Operation and Programming Manual Documentation Set - Manual (Page 319)

Chapter 11
Coordinate Control
11-3
In Figure 11.1, your system installer has defined the zero point of the
machine coordinate system by assigning the machine home point to have
the coordinates X=10 and Z=15 in the machine coordinate system.
Important: The coordinate values assigned to the machine home point do
not affect the position of machine home. The position of machine home is
fixed by your system installer.
Normally the control displays the current position of the axes in respect to
the active work coordinate system. The control can display the position in
the machine coordinate system if you select the absolute screen as
described in chapter 8.
Although axis motion is usually commanded in the work coordinate
system, axis motion by referencing coordinate values in the machine
coordinate system is possible when a G53 is programmed in a block.
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 wheel travels to this
position in G00 or G01 mode depending on which is active when the
control executes the G53 block. Any attempt to execute a G53 block in
G02 or G03 mode generates an error.
The G53 code is not modal and 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 it executes
the G53 block. If you execute a G53 while in incremental mode (G91), the
control generates the error “G53 NOT ALLOWED IN INCREMENTAL
MODE” and the block is not executed.
11.1.1
Motion in the Machine
Coordinate System (G53)