[2wheelferrum07]

am posting this here in hope that someone has had similar experiences.

ok, here is the situation.
i have been in the manufacturing world for over 25 years.
i started a new job programming. the part i was working with required a large program.
its a Die for a punch press.
am using MasterCam to produce the G code.
i verified the process in Master Cam and it showed no errors.
i verified the G code on NCPlot and it showed no errors.
so after a few passes over the whole part it made a big arc. ruining the Die.

what i think happened is that the machine miss interpreted the small arc

Here are the two samples of programming
chime in if you have some feedback and solutions.
thank you in advance

I J version of the program

X-9.9397 Y3.9159
G3 X-9.962 Y3.9145 I.0031 J-.2341
G1 X-9.9636 Y3.9143
G3 X-9.9873 Y3.9033 I.0127 J-.0586
G1 X-9.9887 Y3.9023
G3 X-10.0086 Y3.8547 I.047 J-.0476
X-10.0084 Y3.8504 I.0669 J0.
G1 Y-3.8538
Y-3.8557
G3 X-10.0052 Y-3.8776 I.0752 J0.
G1 X-10.0046 Y-3.8795
G3 X-9.9985 Y-3.8911 I.0791 J.0335
G1 X-9.9975 Y-3.8925
G3 X-9.9909 Y-3.9002 I.0741 J.0575
G1 X-9.9897 Y-3.9012
G3 X-9.982 Y-3.9069 I.057 J.0683
G1 X-9.9806 Y-3.9078
G3 X-9.9425 Y-3.916 I.0381 J.0845
X-9.9374 Y-3.9159 I0. J.0927
G1 X-9.6619 Y-3.9242
X-9.6072 Y-3.9258
X-8.4006 Y-3.9632
X-6.0823 Y-4.0325
X-4.1163 Y-4.0892
X-2.4425 Y-4.1355
X-.6108 Y-4.184
X9.7799 Y-4.4544
G0 Z-1.618
Z2.

And here is the sample of R values
No process changes, just changed the settings to post R values rather than I J

This cut fine without the error

Y-3.8557
G3 X-10.0052 Y-3.8776 R.0752
G1 X-10.0046 Y-3.8795
G3 X-9.9985 Y-3.8911 R.0859
G1 X-9.9975 Y-3.8925
G3 X-9.9909 Y-3.9002 R.0938
G1 X-9.9897 Y-3.9012
G3 X-9.982 Y-3.9069 R.089
G1 X-9.9806 Y-3.9078
G3 X-9.9425 Y-3.916 R.0927
X-9.9374 Y-3.9159 R.0927
G1 X-9.6619 Y-3.9242
X-9.6072 Y-3.9258
X-8.4006 Y-3.9632
X-6.0823 Y-4.0325
X-4.1163 Y-4.0892
X-2.4425 Y-4.1355
X-.6108 Y-4.184
X9.7799 Y-4.4544
G0 Z-1.618
Z2.

What say you?

[Superman]

G1 X-9.9806 Y-3.9078
G3 X-9.9425 Y-3.916 I.0381 J.0845
X-9.9374 Y-3.9159 I0. J.0927
G1 X-9.6619 Y-3.9242
X-9.6072 Y-3.9258
X-8.4006 Y-3.9632

What machine & control is it being run on ?
that is only a X0.0051 Y0.0001 movement of the arc endpoints on a 0.0927" arc
- could be a "filter" setting in Mastercam. How it filters the screen toolpath when posting to NC code
- could be a machine parameter setting, in how it handles quasi ( small ) arc movements

I've seen this happen on Okuma machines, when parameters need to be tweaked

[2wheelferrum07]

the machine is a Vertical Supermax
it has a Yeong Chin Fanuc MXP200i control

the other equipment that had the same issue has an 18i control.

the small arc issue is what i've been saying all along.
and have seen it in the past. just not in newer equipment.

thank you for your response.

PS
so what do you say about the "R" program?

it ran fine.

[SBC Cycle]

I have ran into the same problem and a similar issue before with CAM generated code.

The Fadal will error on arcs greater than 400 inches and will "crop circle" on arc sweep segments that are too short/too small radii. The Haas (unpredictably) will stumble on some short arc segments when machine Cutter Compensation is in effect (If I recall correctly)

I fixed both issues by arc filtering in the Post Processor with my other CAM software. Any radius larger than 400 inches gets converted to a straight line (G01). The tiny arc segments were harder to filter and I can't quite remember for sure how I handled it but it was definitely in the post also.

I'm just getting started with MC (V9) and after reading this post I realized this problem will probably come up again so I am definitely interested in the solution.

Posting R values instead of I,J, or K did fix the issue in my controller (I did verify that long ago) but I don't like using R and didn't want to have a special post just to fix a problem after it had already occurred. Arc filtering is the way to go but I'd like to know how to go about doing it in MC.