Fanuc Series 15i/150i-MA (Programming) Operators Manual

B-63324EN/03 PROGRAMMING 6.REFERENCE POSITION
- 183 -
Explanation
- Reference position return (G28)
Positioning to the intermediate or reference positions are performed at
the rapid traverse rate of each axis.
Therefore, for safety, the cutter compensation, and tool length
compensation should be cancelled before executing this command.
The coordinates for the intermediate position are stored in the CNC
only for the axes for which a value is specified in a G28 block. For the
other axes, the previously specified coordinates are used.
(Example) N1 G28 X40.0 ; Intermediate position (X40.0)
N2 G28 Y60.0 ; Intermediate position (X40.0, Y60.0)
- 2nd, 3rd, and 4th reference position return (G30)
In a system without an absolute-position detector, the first, third, and
fourth reference position return functions can be used only after the
reference position return (G28) or manual reference position return
(See Operation II-3.1) is made. The G30 command is generally used
when the automatic tool changer (ATC) position differs from the
reference position.
- Return from the reference position (G29)
In general, it is commanded immediately following the G28 command
or G30.
For incremental programming, the command value specifies the
incremental value from the intermediate point. Positioning to the
intermediate or reference points are performed at the rapid traverse rate
of each axis.
When the workpiece coordinate system is changed after the tool
reaches the reference position through the intermediate point by the
G28 command, the intermediate point also shifts to a new coordinate
system. If G29 is then commanded, the tool moves to the commanded
position through the intermediate point which has been shifted to the
new coordinate system.
The same operations are performed also for G30 commands.
- Reference position return check (G27)
G27 command positions the tool at rapid traverse rate. If the tool
reaches the reference position, the reference position return lamp lights
up. However, if the position reached by the tool is not the reference
position, an alarm (No. 185) is displayed.
Limitation
- Status the machine lock being turned on
The lamp for indicating the completion of return does not go on when
the machine lock is turned on, even when the tool has automatically
returned to the reference position. In this case, it is not checked
whether the tool has returned to the reference position even when a
G27 command is specified.

Leave a Reply

Your email address will not be published. Required fields are marked *