Issues with 2d contours and NC file format

[patt.t.klein]

Hey all,

I'm having an issue with 2d contour paths exported from Fusion to .NC for a NK105 G3 contoller.

For some reason majority of the files I export from Fusion 360 that contain a 2d Contour path are coming up with NC running error (Line 16): Arc / Circle Radius error.

I don't get this error with any other pathways, it's only ever the 2D contour.

This morning whilst trying to solve the problem, I had the exact same settings (different end mill though, one was an 8mm, other was 10mm) on 2 different models, one of them cut fine, the other gets stuck and doesn't get past Line 16. It has also always been Line 16 that is the issue amongst various models when trying to get them to work. 

It has been driving me crazy trying to work out what error is causing it. Has anyone had a similar issue?

I've attached screenshots of the paths this morning that worked and didn't.  I have no idea how they are generated the way they are, as the fusion 360 settings are the same. 

I'm hoping it's something small and dumb that I am missing! 

Thanks

[engineguy]

@patt.t.klein 

The only difference that I can see is in the working file there is a G18 G3 with an R value and in the non working there is a G19 G2 with no R value which is probably the line (Line 17) that your control is not able to read, check your Leadin/out settings first.

As there is no arc in the Line 17 non working this may be a Post Processor issue, what PP are you using ?

Can you upload a Fusion f3d file that produces the error and a copy of the Post processor ?

[dammitcotezee]

I have the same sometimes error on the same controller (nk105 G3). Attached is a f3d and the post it generated that breaks on line 21 ( I think the error is in line 22)

using the post linked by will_1 here: https://forums.autodesk.com/t5/hsm-post-processor-forum/post-processor-for-weihong-nk105-solved/td-p...

[seth.madore · Accepted solution]

It seems to be occurring on G18/19 lines. What happens if you disable Vertical Lead-in/out moves? You can do that in the Linking Tab of the toolpath dialog:

 

[patt.t.klein]

This is the solution I stumbled across too shortly after posting this. 
Only difference was unticked the Lead in & out completely. I haven't had any issues similar since doing that and have cut about 50 sheets now with no errors. 

Always a simple solution in the end but getting there can be rather frustrating sometimes! 

Cheers

[dammitcotezee]

So setting the highlighted box in lead-in/out to zero disables the feature and solves the issue? 

I found a possible solution last night as well. Which is to use a different post linked earlier in that same thread https://forums.autodesk.com/t5/hsm-post-processor-forum/post-processor-for-weihong-nk105-solved/m-p/... and then disable helical moves in the post settings. 

This so far has been stable for me, but I will see as I continue. 

[seth.madore]

Yes, the one other option if you want to continue using the post processor you currently are, is to do a quick modification to the post that will turn G18/19 arcs into linear line segments.

allowedCircularPlanes = undefined; // allow any circular motion

Changed to:

allowedCircularPlanes = PLANE_XY; // allow circular motion on XY Plane only