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

B-63324EN/03 PROGRAMMING 14.COMPENSATION FUNCTION
- 449 -
14.4.9 Corner Circular Interpolation (G39)
By specifying G39 in offset mode during cutter compensation C, corner
circular interpolation can be performed. The radius of the corner
circular interpolation equals the compensation value.
Format
(In offset mode)
G39 ;
Or,
G39 ;
Explanation
- Corner circular interpolation
When the command indicated above is specified, corner circular
interpolation in which the radius equals compensation value can be
performed. G41 or G42 preceding the command determines whether
the arc is clockwise or counterclockwise. G39 is a one-shot G code.
- G39 without I, J, or K
When G39; is programmed, the arc at the corner is formed so that the
vector at the end point of the arc is perpendicular to the start point of
the next block.
- G39 with I, J, and K
When G39 is specified with I, J, and K, the arc at the corner is formed
so that the vector at the end point of the arc is perpendicular to the
vector defined by the I, J, and K values.
Limitation
- Move command
In a block containing G39, no move command can be specified. If a
move command is specified in a G39 block, a PS0273 alarm is issued.
- Inner corner
G39 must not be used for blocks that form an inner corner. Otherwise,
overcutting results.
- Feedrate for corner circular interpolation
Even if corner circular interpolation is specified using G39 in G00
mode, the feedrate specified by the previously specified F command is
used in the block that specifies corner circular interpolation. When
G39 is specified in the case where the F command is not specified even
once in the program, the feedrate specified in parameter No. 1493 is
used as the feedrate for the block specifying corner circular
interpolation.
I_ J_
I_ K_
J_ K_

Leave a Reply

Your email address will not be published.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