FANUC Series 16/18/160/180-Model C for Lathe Operator Manual

PROGRAMMING
4. INTERPOLATION FUNCTIONS
B–62754EN/01
42
The G00 command moves a tool to the position in the workpiece system
specified with an absolute or an incremental command at a rapid traverse
rate.
In the absolute command, coordinate value of the end point is
programmed.
In the incremental command the distance the tool moves is programmed.
_: For an absolute command, the coordinates of an end
position, and for an incremental command, the distance
the tool moves.
G00IP_;
Either of the following tool paths can be selected according to bit 1 (LRP)
of parameter No. 1401.
D Nonlinear interpolation positioning
The tool is positioned with the rapid traverse rate for each axis
separately. The tool path is normally straight.
D Linear interpolation positioning
The tool path is the same as in linear interpolation (G01). The tool is
positioned within the shortest possible time at a speed that is not more
than the rapid traverse rate for each axis.
End position
Non linear interpolation positioning
Start position
Linear interpolation positioning
The rapid traverse rate in the G00 command is set to the parameter
No.1420 for each axis independently by the machine tool builder. In the
positioning mode actuated by G00, the tool is accelerated to a
predetermined speed at the start of a block and is decelerated at the end
of a block. Execution proceeds to the next block after confirming the
in–position.
“In–position” means that the feed motor is within the specified range.
This range is determined by the machine tool builder by setting to
parameter No.1826.
4.1
POSITIONING
(G00)
Format
Explanations

Leave a Reply

Your email address will not be published.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