[Delw]

I am getting error 367 cutter compensation interference on a bore I need to cut. I dont use cutter comp that often so I am sure I am doing something wrong. my endmill dia is 3/8 thats what I put also in the offset page under dia. nothing is in wear.
the bore size is .9065 and the lead in and lead out rads are .4522

M6 T2 (0.375 DIA. END MILL)
G0 G90 G55 X0.2742 Y-0.1411
M3 S1500
G43 Z1.0 H2 M08
G1 Z0.1 F5.0
G41 D2 X1.7239 Y-0.0386
G3 X1.7648 Y0.0 I0.0023 J0.0386 Z-0.300
I-0.2648
X1.7239 Y0.0386 I-0.0386 Z0.05
G1 G40 D2 X0.2742 Y0.1411
G0 Z1.0
M09
G91 G28 Z0.0 M05
M30

My rad. lead in I have helical down so I have enough room to apply cutter comp command and rad lead out has a helical up as well.

Thanks
Delw

[djr76]

why dont you use G13?

G13 X1.7648 Y0.0 D2 I.4532 F5.

other then that, your I value should be I-.4532 since you are already comping the cutter with G41, you dont need to calculate the radius of the cutter.

[Delw]

I never used g13 before, I will look it up and try it
Thanks

[Delw]

other then that, your I value should be I-.4532 since you are already comping the cutter with G41, you dont need to calculate the radius of the cutter.

DJ
I kinda ignored this line, until I was driving down to the store, then it hit me , I screwed up in my cad software, I had offset enabled, thats why the numbers didnt make much sence late last night.

Thanks again,
once this jobs finished I am going to play with that g13, I have a good size part that I can try it on.

again thanks
Delw

[djr76]

DJ
I kinda ignored this line, until I was driving down to the store, then it hit me , I screwed up in my cad software, I had offset enabled, thats why the numbers didnt make much sence late last night.

Thanks again,
once this jobs finished I am going to play with that g13, I have a good size part that I can try it on.

again thanks
Delw

That code I gave you is 1 circle, put your X, and Y position before that line and add your Z value in the place of X, and Y where I had it instead. (G13 Zx.xxx D2 I.4532 F5.). You can also spiral out with I, K and Q value. K = finish radius, I = Start radius, Q = step over amount. You can also spiral up or down in Z with L value L = # of steps. Experiment with it in graphics.

[Delw]

Dj
I ran the g13 right after I made the last reply,Cause you know how it goes a jobs running pretty good and why not just try something new LOL WOW thats pretty badass.,
I dont run too many canned cycles, I do most of everything in cad. but the g13 is great cause you can just take your drilling cycle(center points) modify it and use it for the g13.
Thanks again for all the help.

Delw

[Machineit]

Dj
I ran the g13 right after I made the last reply,Cause you know how it goes a jobs running pretty good and why not just try something new LOL WOW thats pretty badass.,
I dont run too many canned cycles, I do most of everything in cad. but the g13 is great cause you can just take your drilling cycle(center points) modify it and use it for the g13.
Thanks again for all the help.

Delw

The G12 and G13 codes are very powerful and so easy to use. I use them so often that I keep a program on the control that is titled G13.

Easy to program, can use steps in size and down is Z axis.

Example: G13 G91 Z-.5 I.400 K2.0 Q.400 D01 L4 F20.

With a 1/2 inch endmill that would bore a 2.5 inch hole 2 inches deep with a step of .2 each pass and an initial hole size of 1.400. So easy!

If you do use the "L" for multiple passes in "Z" depth, make sure to switch back to G90 and clear the tool from the hole! This is one of the few canned code that does not retract from the hole when it is finished like all the drill cycles and such do. You always must retract the tool from the hole before moving to a different location.

Mike