Why CNC Sometimes Cuts a Line Instead of an Arc

A variety of input flaws can cause equipment to take a shortcut between the end points of what should be an arc. March 1, 2006

Question
I have a problem when I nest a part with an arc. The CNC will cut a line from end point to end point of the arc instead of following the arc. I am running a Multicam 5000 series powered by Mastercam version 9.1. I am not sure if this is an issue with my software or the machine. When I check the parts in Job Previewer and check the G code I see no problems. Has anyone ever seen this before?

Forum Responses
(CNC Forum)
From contributor A:
The first thing that comes to mind is if you are importing a CAD file (dwg., dxf., etc.) and the drawing is not clean (entities not connected and adjacent) - G codes being modal on most controls - if no chaining of entities then the control will recognize the last known code and proceed to the next coordinate. If it is a newer CAM module this may suggest the post needs tuning. Finally, check the code at the machine, as opposed to looking at it in your CAM software - you could be losing data in the transfer? If it looks correct, hand write a basic code in the machine of simple coordinate values and radius, execute and insure the machine is cutting properly, then work your way back. What type of machine and control?


From contributor B:
When I have had this problem in the past it was the resolution of the CAD software, Auto Cad Lite. At lower resolution the CAD software would draw lines instead of a circle. Try adjusting the resolution in your CAD. I don't remember how, but I'm sure one of the ACAD guys could answer.

From contributor C:
If you’re importing a CAD file make sure all the lines are exploded i.e. not a continuous polyline. If we don’t do this with ours, it just ignores the arcs as you describe.

From the original questioner:
I had the same problem a month ago. I run MasterCam 9.1 on a CR Onsrud CNC. The problem was our AMC controller. It does not recognize an arc larger than a 2300 inch radius. I could run a 2200 inch radius, but not a 2300 inch radius. The guys at Onsrud knew all about it. There is a linearation program that will make an arc of a large radius out of very small straight lines. However, I have not gotten it yet from Onsrud.

From contributor D:
I have also seen this problem occur when importing .DXF files with arcs into a CAM package. Low quality .DXFs seem to be the problem.

The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).

Comment from contributor E:
I've ran into this too, but with too small of an arc trying to be cut. I find the length and if it is as short as I specify I router the arc move as a line. If the square root of the cords is less than .1 then I output G01 rather than G02 or G03.

Ex:

$IF SQR(IX * IX + IY * IY) < .1
$LET MY_COUNTER = MY_COUNTER + 1
G01 X[GAX] Y[GAY] Z[AZ] F[F]
''
$ELSE
$LET MY_COUNTER = MY_COUNTER + 1
G02 X[GAX] Y[GAY] R[R] F[F]
''
$ENDIF

Related Articles