FANUC Series 16/18/160/180-Model C for Lathe Operator 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.
For details of how to use this function, refer to the manual supplied by the
machine tool builder.
G31 _ ;
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 #5068, as follows:
#5061 X axis coordinate value
#5062 Z axis coordinate value
#5063 3rd axis coordinate value
#5068 8th axis coordinate value
To increase the precision of the tool position when the skip
signal is input, feedrate override, dry run, and automatic
acceleration/deceleration is disabled for the skip function
when the feedrate is specified as a feed per minute value.
To enable these functions, set bit 7 (SKF) of parameter No.
6200 to 1. If the feedrate is specified as a feed per rotation
value, feedrate override, dry run, and automatic
acceleration/deceleration are enabled for the skip function,
regardless of the setting of the SKF bit.
1 If G31 command is issued while tool nose radius compensation 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.
2 For the high–speed skip option, executing G31 during feed–per–
rotation mode causes P/S alarm 211 to be generated.

Leave a Reply

Your email address will not be published.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