[SeymourDumore]

While it might move towards the part, it would not cause overcutting as this point is in fact exactly the same point from where the cycle started from, therefore there cannot possibly be any material left to overcut.

[sinha_nsit]

Still I feel that it is a good practice to move the tool away from the job during the ramp-off move. Maybe we should use X1.2 (say) instead of X1.125 in the ramp-off move, even though it is not required in this case.

[lowehardware]

I have tried both of your methods and here are the results:

Seymour's causes Alarm 41, "Interference in NRC-Overcutting will occur in tool nose radius compensation. Modify the program"

Cogsman's method simply overcuts the back of the sphere (towards the chuck) during roughing (nothing left to finish for G70). Please help guys. I'll post the new application I'm trying to use this for in both of your methods.

Seymour's:

G0X1.1Z0.
G1X-0.05F.004
G0G42X1.Z0.05
G71U.06R.02
G71P101Q201U.01W0F.006
N101G0X0.Z0.05
G1Z0.F.003
G03 X0.5785 Z-0.7658 R0.4375
G02 X0.7286 Z-1.0185 R0.1453
G03 X0.78 Z-1.0482 R0.03
G01 Z-1.22
N201X1.
G70P101Q201
G0G40X1.1Z.05
G80M09

Cogsman's:

G0X1.1Z0.
G1X-0.05F.004
G0X1.Z0.1
G71U.06R.02
G71P101Q201U.01W0F.006
N101G0X0.Z0.1
Z0.05
G1G42Z0.F.003
G03 X0.5785 Z-0.7658 R0.4375
G02 X0.7286 Z-1.0185 R0.1453
G03 X0.78 Z-1.0482 R0.03
G01 Z-1.22
X1.
N201G0G40Z0.05
G70P101Q201

I also tried both of these with tool nose 3 or 8. Didn't make any difference.

Check out my website so you know I'm not an idiot!

www.lowe-hardware.com

[SeymourDumore]

Lowe

I jut re-read your original post and realized that you're using a .0312R tool.
My bad!!! The start points in Z must be moved away appropriately to allow the tool to fit in. With .0312 that distance is .062, which is apparently larger than the Z.05 I've posted.

Sorry!!!
Try this one:


G0X1.1Z0.
G1X-0.05F.004
G0G42X1.Z0.1
G71U.06R.02
G71P101Q201U.01W0F.006
N101G0X0.Z0.1
G1Z0.F.003
G03 X0.5785 Z-0.7658 R0.4375
G02 X0.7286 Z-1.0185 R0.1453
G03 X0.78 Z-1.0482 R0.03
G01 Z-1.22
N201X1.
G70P101Q201
G00G40X1.3 Z.2
G80M09

[lowehardware]

I just tried that with both tool nose radius 3 and 8. 3 overcut again on the back of the sphere in roughing and 8 overcut at the front. I'm a little frustrated! ha

[cogsman1]

Did you set your "Z" from the CENTER of the radius where it contacts the material? When using # 8 vector that is where the code is working from.
With that vector and the tool touched off correctly you WILL get what you are looking for. Been there, done that. This works the same on Fanuc, Mitsubishi, (Okuma, Mazak, Mori, Citizen, Tornos, Tsugami, Star....) When you go from Swiss to non-Swiss the G41/G42 and G2/G3 are opposite but this cut would be #8 vector on all of them.

[SeymourDumore]

Yup, as Cogsman said.
Touch off Z at part face, then deduct 1/2 toolR from the offset in the offset register.
It's gotta work!!!