FANUC Series 16/18/160/180-Model C Machining Center Operators Manual

Linear interpolation can be commanded by specifying axial move
following the G31 command, like G01. If an external skip signal is input
during the execution of this command, execution of the command is
interrupted and the next block is executed.
The skip function is used when the end of machining is not programmed
but specified with a signal from the machine, for example, in grinding. It
is used also for measuring the dimensions of a workpiece.
G31 IP_ ;
G31: One–shot G code (If is effective only in the block in which it
is specified)
The coordinate values when the skip signal is turned on can be used in a
custom macro because they are stored in the custom macro system
variable #5061 to #5064, as follows:
#5061 X axis coordinate value
#5062 Y axis coordinate value
#5063 Z axis coordinate value
#5064 4th axis coordinate value
#5065 5th axis coordinate value
#5066 6th axis coordinate value
#5067 7th axis coordinate value
#5068 8th axis coordinate value
Disable feedrate override, dry run, and automatic
acceleration/deceleration (however, these become
available by setting the parameter SKF No.6200#7 to 1.)
when the feedrate per minute is specified, allowing for an
error in the position of the tool when a skip signal is input.
These functions are enabled when the feedrate per rotation
is specified.
If G31 command is issued while cutter compensation C is
applied, an P/S alarm of No.035 is displayed. Cancel the
cutter compensation with the G40 command before the G31
command is specified.

Leave a Reply

Your email address will not be published.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