Sweeping stops at sharp corner

[Anonymous]

I encountered this problem while attempting to sweep a sketch along the edge of an object. The sweep stops at the first sharp corner.

The problem is a bit difficult to explain, so I appended a video demonstrating the process that leads to the problem.

Edit: In case the screencast doesn't show up, here's the link!

Thanks a lot for helping out!

All the best-

[jeff_strater]

@Anonymous - your video failed to attach - try again?  But, better, attach the model here.

Even without seeing either the model or the video, my guess is that the problem here is that the sweep will "self-intersect" at that sharp corner.  Solid sweep does not allow a self-intersecting result.

But, share the model for a more accurate answer.

[Anonymous]

Hey Jeff,

thanks for the reply! I tried again and I think the video is showing up now.

Anyway, here's the file: https://a360.co/3eBDYPn

In the screenshot below, the object I was talking about is the one on the right. Originally, I was planning to achieve the effect though a simple fillet operation, which failed (compare three objects on the left). I think the problem is that the chamfer operation always leaves behind two seperate points that then mess with the fillet or the sweep. 

The object was supposed to look something like this:

[chrisplyler]

Look in your Sweep setting options...you have it set to Perpendicular. Try it set to Parallel and see what happens.

[jeff_strater · Accepted solution]

This was an interesting one.  Thanks for providing an interesting Friday puzzle.  The problem, as you guessed, was that Chamfer.  That is not really a good use of chamfer, because it ends up leaving a tiny sliver edge in the model.  You can see it if you use Select Other or Measure.  There are two vertices here:

and you can see if you measure them, how close they are:

This tiny edge throws off both Sweep and Fillet.  I think the Sweep would, in fact, be self-intersecting, but the problem is really that edge.

The solution is to not use Chamfer to get that angled face, but use Draft instead, then you can use Fillet on the result.  See the screencast below:

[chrisplyler]

Fusion usually allows sweeps to self-interset at hard corners...it just miters. Two hard corners that close together though...that would try to miter around both, possibly leaving a 'partial profile sliver' between them, screwing it up.