More G40 G41 G42 Cutter Radius Compensation

RS274/NGC G-code Reference

Cutter Radius Compensation — G40, G41, and G42

To turn cutter radius compensation off, program G40. It is OK to turn compensation off when it is already off. Cutter radius compensation may be performed only if the XY-plane is active.
To turn cutter radius compensation on left (i.e., the cutter stays to the left of the programmed path when the tool radius is positive), program

G41 D…

To turn cutter radius compensation on right (i.e., the cutter stays to the right of the programmed path when the tool radius is positive), program

G42 D…

The D word is optional; if there is no D word, the radius of the tool currently in the spindle will be used. If used, the D number should normally be the slot number of the tool in the spindle, although this is not required. It is OK for the D number to be zero; a radius value of zero will be used.
It is an error if:
• the D number is not an integer, is negative or is larger than the number of carousel slots,
• the XY-plane is not active,
• cutter radius compensation is commanded to turn on when it is already on.
The behavior of the machining center when cutter radius compensation is on is described in Appendix B.


G40 G41 G42 Cutter Radius Compensation