Error: Bad starting point given for edge-edge blend geometry

[rarsenianNT7BC]

Hello Fusion360 Users,

Sorry i'm new to fusion, but i'm trying to round some edges on a simple part.
Basically I converted a letter which was a PNG to an SVG file, then imported it into Fusion.

I then extruded the letter which looks great and now I want to slightly round the edges, but I get the error: " Error: Bad starting point given for edge-edge blend geometry" and I can't figure it out..

Here is the file, I'm hoping someone can tell me what I'm doing wrong

[Anonymous]

Your extruded sketch curve appears simple enough, but it's likely that somewhere in the bitmap to vector conversion some odd geometry was created that is confusing Fusion.

What software did you use to perform the vectorization? A quick google search shows there are a number of free alternative options you may like to try. My guess is one of these will produce a favorable result.

[rarsenianNT7BC]

hello 

Thanks for the reply.. I used inkscape.

Basically i did a bitmap trace. then saved to SVG

[TrippyLighting]

There are several problems:

1. These imported curves are not curvature continuous in several places, and the curvature is pretty bad in some of the tights corners. You can check this with Inspect->Curvature Comb.

2. Some of the "tight corners" are collapsing when you make the fillet to big. I can get this filleted t a maximum of .035mm. You can check that by creating a sketch on the top surface of the object and projecting the outline into it. Then do an offset. At 0.2mm you can already see pretty strong degradation in the corners

[rarsenianNT7BC]

Thankyou.

So in your experience, what would be the best way to fix this?

Cheers

Rich

[TrippyLighting · Accepted solution]

You cannot fix this using the existing sketch.

What I did as a workaround is:

1. I created a new sketch and placed 1mm circles in these sharp corners that present the problem when filleting. These circles were not locked in place, just in dimension.
2. Then I created another sketch and simply projected these circles into a new sketch.
3. In that new sketch I then sketched splines and applied tangent constraints between the beginning and end handles and the circles. I tried to hand position the splines on the circles as close to tangent as possible.
4. Then it was a bit of tedious hand work to adjust the spline points and tangent handles to best reflect the shape of the original sketch section I wanted to trace.
5. When done with a given spline I applied a fix constraint to that spline in order to improve sketch performance (the sketch solver in Fusion 360 needed a little help)
6. When done I extruded the new sketch and filleting to 0.45mm  was no problem.

[rarsenianNT7BC]

Thanks so much Peter. You're a genius.