Need Help!- Crop circles - tiny arc turns into full circle

[Fadal Error]

What does line 26 in the Fadal post processor do?

26. Set debug.
debug_off

Should I switch debug to on?

[Fadal Error]

Originally Posted by fizzissist Assuming you've config'd Bob's post processor to split circles into halves?

I'm trying to figure out how to do this.

Can you post the code where the Bob-circles happen?

N15899 G01 X6.8714 Y-4.8318
N15900 G03 X6.8714 Y-4.8318 I-.0431 J.0117


N16657 G01 X8.1181 Y-4.8318
N16658 G03 X8.1181 Y-4.8318 I-.0432 J.0118

[Fadal Error]

Found it.

223. Break arcs into two pieces if greater than 180 degrees? y

[Dyad1]

Hi Guys,
In looking at your two examples of code it seems to me that both items start and finish at the same point. This being the case it is like not putting the x and y coordinates in at all and calling for a complete circle at a radius of .04468".
Trying to be too precise can sometimes backfire. It has happened to me a few times with arcfit routines. Try loosening it up a bit. A lot less code and I'll bet you won't be able to see a difference.
Good luck,
Gary

[Neal]

Looking at the original post, Normally these type of "circles" are caused by geometry breaks that cause cutter comp to have a problem following the proper tool path. This usually happens in the CAD/
CAM geometry due to the tolerences set too wide open.

Neal

[Fadal Error]

So I thought I had it all figured out and then a big crop circle showed up in one plate yesterday. NC Plot did not catch it, but I tracked down the errant line and found this:

N5112 X3.1868 Y-4.0839
N5113 X3.1867 Y-4.0889
N5114 G02 X3.1866 Y-4.0902 I-1.8002 J-.0971
N5115 X3.1867 Y-4.0889 I3.1393 J-.1244
N5116 G01 X3.1868 Y-4.0839


I do believe that line 5114 is the culprit, especially because the crop circle went away when I changed it to a G01.
Bobcad outputs a .0013 long arc, which seems like a legitimate move to a super precise CAD/CAM program. The Fadal sees an end point that is almost exactly the same as the beginning point and figures I must have meant that I wanted a 3.6" circle right there.
Am I right? How do I eliminate this. It could be that the video on Bobcad's youtube channel could fix this, but I haven't tested it yet.

The good news is that I finished all six plaques and they are on their way to a trade show in Germany. I delivered them at 9:30 last night, making that my earliest quitting time since Wednesday of last week. And with all of the crop circle chasing, I made $18/hour!

[Andre' B]

I have had this same problem with MasterCAM and a Fanuc control.
Since CNC contols for the most part only go to 4 decimal places CAM programs limit the precision of the calculations they do, speeds things up. This can lead to problems with arc centerpoints when the length of the arc is very small, even more when the arc radius is relativly large.

I bet if you put (I-1.7947 J0.1374) in line 5114 it would work fine.

At the time I was having my problems I did not know much about MasterCAM and it's posts so I gave up and set it up so it did not output any G2 or G3 lines but divided all arcs up into G1 moves. The program size exploded but it stopped crashing, I was doing arcs in the YZ plane so I was breaking end mills and melting tool holders when it decided to go full circle.
I think I now know enough that I could get the post adjusted properly but since it works with just G1 moves why bother.