Chamfering a curve

[Anonymous]

Hi, my first post here.

I'm hoping it's a simple one. Can anyone tell me why Fusion360 won't let me chamfer this curved edge to any more than 0.5mm without throwing an error?

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Are there any unresolved issues highlighted in your Timeline?

[Anonymous]

Here's the file. There's only one issue in the timeline. Ironically, the sketch to make the curved plane. I'm not sure how to respolve that either.

[TheCADWhisperer]

Looking at your Timeline - I would start over from scratch.

I would fully define each and every sketch.  (I would include things like Tangent constraints to arcs.)

I would have one long continuous line rather than multiple short colinear lines.
But that's just my technique - your technique might differ.

[jeff_strater]

While I would always recommend following @TheCADWhisperer 's advice, on any CAD topic, I suspect the answer to your specific question on this model can be seen here (I had to make a guess about where in the timeline of the model you shared you were trying to apply the chamfer).  The problem is this edge/face that is adjacent to the edge you are chamfering:

If I measure the distance between those two edges, it shows as 0.5:

Which exactly correlates to the limit on the chamfer.  And, it makes sense, too.  At .5, that chamfer starts to interfere with that other face.

Also, this edge has "near tangencies" - meaning that the edges are almost, but not quite tangent (you can tell they are not tangent because they are not auto-selected when Chaining is turned on).  This causes problems with the modeling kernel.   You can see that if you turn on curvature comb analysis on these edges:

the tangent discontinuities show up as these steps in the curvature comb display.  So, that is where @TheCADWhisperer 's recommendations to make sure to have tangent constraints on your sketch lines will be helpful.