Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 375)

Axis Motion
Chapter 14
14-17
If an attempt is made to execute a G27 before the axes have been homed,
the control goes to cycle stop and displays this error message:
“MACHINE HOME REQUIRED OR G28”
The G30 command is similar to the G28 command. The main difference is
the axis or axes move to an alternate home position instead of machine
home. The command format determines whether the axes return to a
second, third, or fourth alternate home position. Any axis programmed in
the G30 block must have been homed prior to G30 execution.
The alternate home positions are defined for each axis in AMP by your
system installer.
To use the G30 command follow this format:
G30 X__ Z__;
or (second alternate home position)
G30 P2 X__ Z__;
G30 P3 X__ Z__; (third alternate home position)
G30 P4 X__ Z__; (fourth alternate home position)
The axis words in the above block establish the intermediate point in the
same manner as the G28 code described on page 14-13. Axes move to the
intermediate point defined in the G30 block prior to moving to the
alternate home position. This intermediate point is the same intermediate
point as the one discussed with the G28 code. When intermediate values
are programmed in a G28 block, they replace G30 intermediate point
values and visa-versa. This intermediate point is used by the G29
automatic return code.
Only those axes included in the G30 block are sent to the alternate home
position.
A typical application for the G30 command would be if the automatic tool
changer were located at a position other than machine home.
If an axis included in the G30 block has not been homed, block execution
stops and this error message appears:
“MACHINE HOME REQUIRED OR G28”
14.2.5
Move To Alternate Home
(G30)