G40, G41, G41.1, G42, G42.1 (Cutter Radius Compensation)

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 the 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 the 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 or for turning the zx 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 a with g41 1 d is the same as g41 d except now the d number is not a tool number but a tool diameter with g42 1 d is the same as g42 d except now the d number is not a tool number but a tool diameter example code for milling this example mills out a rectangular object from the outside and inside on the outside, we use g42, tool radius compensation right and for the inside g41, tool radius compensation left is used for both contours, a tool radius compensation entry move is programmed consisting of a line that must be longer than the tool radius used and a circle, of which also the radius is bigger than the tool as a side note, all arc radii should be bigger than the tool radius if you have inside corners, there should always be an arc, so that the tool fits the g42, g41, and g40 codes are programmed with a / (block delete sign) in front this makes it easy to debug tool comp programs the program is loaded with the block delete, this is the blue curve then the program is run with block delete off resulting in the yellow curve it is clear to see what the entry move does g0 z3 g0 x 15 y15 f500 /g42 1 d6 g1 x 5 (cutter comp entry move 1) g2 x0 y10 r5 (cutter comp entry move 2) g1 z 3 (plunge down) g3 x10 y0 r10 g1 x70 g3 x80 y10 r10 g1 y90 g3 x70 y100 r10 g1 x10 g3 x0 y90 r10 g1 x0 y10 /g40 g0 z3 g0 x30 y30 /g41 1 d6 g1 x20 g3 x10 y20 r10 g1 z 3 g3 x20 y10 r10 g1 x60 g3 x70 y20 r10 g1 y80 g3 x60 y90 r10 g1 x20 g3 x10 y80 r10 g1 y20 /g40 g0 z3 m30 example code for turning the movement starts at the right upper corner the blue line is the programmed contour the yellow is the contour with tool radius compensation g41 the first g1 line is the tool comp entry move you can get this figure by putting a / character in front of the g41/g40 codes the load the program with block delete on and execute it with block delete off with block delete on the tool comp is skipped the g42, g41, and g40 codes are programmed with a / (block delete sign) in front this makes it easy to debug tool comp programs the program is loaded with the block delete, this is the blue curve then the program is run with block delete off resulting in the yellow curve it is clear to see what the entry move does (radius programming) (use i,k programming for arc’s) g0 x 10 z20 /g41 1 d5 g1 x 10 z10 g3 x0 z0 i10 k0 g1 x10 g2 x20 z 10 i0 k 10 g1 z 20 g3 x30 z 30 i10 k0 /g40 m30 (diameter programming) (use i,k programming for arc’s) g0 x 20 z20 /g41 1 d5 g1 x 20 z10 g3 x0 z0 i10 k0 g1 x20 g2 x40 z 10 i0 k 10 g1 z 20 g3 x60 z 30 i10 k0 /g40 m30 (radius programming) (use r word for arc’s) g0 x 10 z20 /g41 1 d5 g1 x 10 z10 g3 x0 z0 r10 g1 x10 g2 x20 z 10 r10 g1 z 20 g3 x30 z 30 r10 /g40 m30 (radius programming) (use i,k programming for arc’s) g0 x 10 z20 /g41 1 d5 g1 x 10 z10 g3 x0 z0 i10 k0 g1 x10 g2 x20 z 10 i0 k 10 g1 z 20 g3 x30 z 30 i10 k0 /g40 m30