Chamfer error in model. No idea why.

[sies5DRVJ]

I'm trying to add a chamfer to this guitar body. Strangely enough, it won't do it. It does work if I apply the chamfer before creating the cutout for the neck, but then the chamfer size is limited, because there is one smaller radius in the contour.

I want to be able to add a chamfer to a contour with two ends like this. I don't see why it shouldn't work.

Can anyone tell me what's going on here and how to fix it?

[TheCADWhisperer]

File >Export and then Attach your *.f3d file here.

[mavigogun]

I'd swear this exact same context was addressed in another thread- by "exact same" I mean the termination of a Chamfer/Fillet on a guitar body at a void designed to receive the neck.   Can anyone point to that thread?

[TheCADWhisperer]

This same problem comes up here every Fall. 

I assume it is students working their way through a Tutorial.

Might be nice if instructor joined the discussion.

[sies5DRVJ]

That's a coincidence. I'm a professional guitar builder who just switched to Fusion360. I've worked with Siemens NX as a mechanical engineer for 10 years and never had this kind of error with chamfering with that software. 

Would be very helpful if someone could point me in the right direction.

I'd rather not share my exact body shapes pubicly, so if we could do it without having to upload my file, that would be great...

[TrippyLighting]

My question would be: How is the curve constructed that creates the outline of the guitar ?

Is that imported or sketched with the native tools in Fusion 360 ?

If so, is it one continuous spline or several sketch objects ?

If it is comprised of several sketch objects, are these constrained to each other with tangent (G1) or continuity (G2) constraints ?

If it is imported then start from scratch with the native tools in Fusion 360. Imported geometry very often creates near-tangent conditions that prevent Fusion 360 to complete chamfers, or fillets.

If it is sketched in Fusion 360 then my questions imply what should be the case.

[mavigogun]

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@sies5DRVJ wrote:

I'd rather not share my exact body shapes pubicly, so if we could do it without having to upload my file, that would be great...

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You might just drag around those curves that are farther away form the neck for the purpose of obscuring your work, leaving the critical smaller radius curve for consideration, and share that version here-File>Export>Attach

While a search for "guitar" on this forum may produce lots of topical returns, this one has some bearing:

https://forums.autodesk.com/t5/fusion-360-design-validate/bass-guitar-modeling-confort-shapings/m-p/...

[mavigogun · Accepted solution]

...short of sharing, there are some basic troubleshooting things to be done.    Chop the guitar body into sections, isolating those curved Edge ends, to narrow where the error is occurring.    Is it on this end, or that?    You want to know which is the problem end- if either -and can make a determination easy enough with a little investigation.    Mayhaps the problem has no relation to the termination, but instead is caused by the radius or adjacent split face- this is a step toward knowing.

[TheCADWhisperer]

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@sies5DRVJ wrote:

...switched to Fusion360. I've worked with Siemens NX ...

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Why?

Can you post an image of Sketch1 showing the constraint glyphs?

[sies5DRVJ · Accepted solution]

The body has been created from one native sketch. All arcs are tangential, the sketch is black. As mentioned, the chamfer works fine before I made the cutout for the neck (for which I used a second sketch, because it's under an angle). 

Update: solved
I've cut the body in two to see which side the problem was on. Turns out it was the one on the right (with the body held upright). There, the cutout made for the neck aligns with a coincident point of two arcs in the contour. I guess because I've extruded the neck pocket under an angle, that area became a bit strange. I've moved the concident point of the two curves a few tenths of a mm away from the intersection with the neck pocket and now it works fine.

Thanks for helping out.

[TrippyLighting]

It sounds to me @mavigogun's suggestion lead to the solution. Can you mark his reply as the solution please ?

[sies5DRVJ]

I've marked his reply as a solution (because of its approach) and mine as well, since this is the more detailed and concrete fix in this specific situation. I guess both are helpful if someone starts a search with a similar problem.

[mavigogun]

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@sies5DRVJ wrote:

Turns out it was the one on the right (with the body held upright). There, the cutout made for the neck aligns with a coincident point of two arcs in the contour. I guess because I've extruded the neck pocket under an angle, that area became a bit strange. I've moved the concident point of the two curves a few tenths of a mm away from the intersection with the neck pocket and now it works fine.

That's good to know- I'll put it in my pocket for future consideration.    A point of clarification, when you wrote of "arcs in the contour", were you referring to Coincident Splines End Points, or segments made with the Arc tool?   It might not matter, either way- just more information.

[mavigogun]

I tried to reproduce this error and got inconsistent results- seemingly without regard for the location of the Spline intersect and Constraint!   There is an entire range of Fillets that work- in my example up to a value of 18 -then failure; the weird part is that while dragging the Fillet control back and forth, a very narrow range will flash resolvable around 25-26!!    This suggests to me the possibility that moving the Spline End Points may shift where that range of possibilities falls.    Another point of interest: selecting G2 curvature causes these larger values to fail.    I don't think we'll ever really know without the file- if you're inclined, you might share it privately with @jeff_strater, referring to this thread;  if extra-ordinary, it may illuminate some dark corner of code.

[sies5DRVJ]

I must applaud you for your determination and your work in developing this software.

The sketch for making the body consisted only of tangential arcs, no splines. 
I'll send you the file in a private message.