Owner's manual

Axis Motion
Chapter 14
14-34
If an attempt is made to execute a G27 before the axes have been homed
the control will go to cycle stop and the following error message will be
displayed:
“MACHINE HOME REQUIRED OR G28”
The G30 command is similar to the G28, with the main difference being
that the a xis 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, in reference to the machine coordinate
system, are predefined for each axis in AMP by the system installer.
To use the G30 command follow this format:
G30 X__ Y__ Z__ ;
or (second alternate home position)
G30 P2 X__ Y__ Z__ ;
G30 P3 X__ Y__ Z__ ; (third alternate home position)
G30 P4 X__ Y__ Z__ ; (fourth alternate home position)
Important: The c ontrol generates the error “P VALUE OUT OF RANGE”
if the P value is illegal. For example, a P1 or P5 would be illegal and
generate the error.
The axis words in the a bove block establish the intermediate point in the
same manner as the G28 code. That i s, the axes will move to the
intermediate point defined in the G30 block prior to moving to the
alternate home position. When intermediate values are programmed in a
G28 block they replace G30 intermediate point values and vice-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. For example:
G30 X5.6 The controlmoves the Xaxistosecond home aftermoving to
5.6 on the X axis. The Zand Yaxesarenotmoved.
G30 P3 X1.0 Z4.0 The controlmoves the Xand Zaxes to thirdhomeaftermoving
to 1.0 on the X axis and4.0on the Z axis. TheY axis isnot
moved.
A t ypical application for the G30 command would be if the automatic tool
changer were located at a position other than machine home.
14.3.5
Return to Alternate Home
(G30)