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

PROGRAMMING
B–62764EN/01
4. INTERPOLATION FUNCTIONS
39
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.
IP_: For an absolute command, the coordinates of an end
position, and for an incremental commnad, the distance
the tool moves.
G00IP_;
Either of the following tool paths can be selected according to bit 1 of
parameter LRP 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 G00 command is set to the parameter No. 1420
for each axis independently by the machine tool builder. In the
posiitoning 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).
In–position check for each block can be disabled by setting bit 5 (NCI)
of parameter No.1601 accordingly.
4.1
POSITIONING
(G00)
Format
Explanations

Leave a Reply

Your email address will not be published.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