Fusion
I created a shoe w/ t-splines then thickened it to make it a solid and added a ridge around the shoe opening. I cannot create a fille on the ridge as shown below. The f3d file is also attached. Does anyone know what I need to do to make the fillet?
What usually helps find a root cause for such problems is if a model has a timeline that records how it was designed.
Unfortunately, you've decided to model with a timeline, so that is impossible.
I am not sure what geometry used to trim the upper edge, but there should not be this many edges in the red circled areas.
yeah, you definitely have some funky geometry/topology in this model. In addition to what @TrippyLighting says, another good thing is to try to turn on curvature comb analysis on the edges in question. You can see here that you have some wild swings in curvature, around that same edge:
particularly in the area indicated by the arrow. I suspect that is the source of the fillet issues
Jeff Strater
Engineering Director
ah, you are filleting the inside edges. I missed that in the image. I do, though, see similar curvature concerns. The edge that is highlighted by the Fillet command does have a lot of curvature, which can cause Fillet failures:
And, zooming, in, I do see a similar reversal of curvature in that area:
Jeff Strater
Engineering Director
It's strange that when I highlight part of the edge I get wonky curves, but if I highlight more of the edge, like the section pointed to by the orange arrow, then the curve is tamed.
In any event, without history turned on is there any way to tame the curve now?
Accepted solution
The way that the curvature comb works is a bit funky. The default "scale" is determined by the number of edges/curves selected. I think that is the only difference between your two images.
"without history turned on is there any way to tame the curve now?"
It is certainly a lot harder without history. With history, you could easily go back to the T-Spline body and modify it to calm down that area of the surface.
There are some tools in Direct Modeling that can help. Just to see what happened, I selected some of the faces (I think it was a different set, but basically these +/- a few:
And I just deleted them. In Solid mode, Delete of a face or set of faces is "delete and heal". I really had no hope that would work, but it did produce a slightly better set of geometry, with some very weird "extras" that worry me a bit:
The first time I did this, I was able to just select and delete most of this geometry, but the "most" part worries me, and when I tried again a second time, Fusion crashed... So, beware, and save before trying this.
But, I was then able to put a 0.7mm fillet on that inside edge:
This model is attached. But, as I said, I don't have a ton of confidence in this geometry, so be a bit cautious with it...
Jeff Strater
Engineering Director
Thank you @jeff_strater! I was able to eventually delete the stray geometry in your attached f3d file w/ a bunch of clicks and deletes. Then I deleted one more face, shown at the red arrow below, from your model:
Then I was able to create a 0.96 mm filet along the inner and outer edge to create a nice round lip w/ the filets meeting in the center:
So you solved the issue. Thank you! For those following -> It was just a matter of deleting enough faces in Solid mode which Fusion 360 healed on its own until I could create the filets I needed.
@mrabushka wrote:
So you solved the issue. Thank you! For those following -> It was just a matter of deleting enough faces in Solid mode which Fusion 360 healed on its own until I could create the filets I needed.
That might have worked in this case, but isn't a technique you should not be relying on!
The reason for the problem is less than ideal modeling techniques.
