Error: mitred vertex too complex to process

[luis.lange]

Hello !

I'm trying to fillet a body but I got this error. The sketch i'm using is scaled up from another drawing that fillet normally.

Here is the place I'm trying to fillet.

Any advice or tip?

Thank you in advance!

Luis

[Johnc911 · Accepted solution]

The problem is the sketches that you're using for the inside parts of that heart are derived from offsets. In CAD, offsets usually create curves that are slightly different from the parent curve and thus can often create "bad" curvature. If you use curvature combs to analyze those inner curves compared to the parent (original) curve you will see that the offset curves curvature appears to be an order of magnitude more aggressive curvature.

Since curves are the basis of surfaces, and surfaces are the basis of solids. This error is going to cascade to surfaces and to the solid edges. Then the fillet will be a problem because of the solid edges are not clean.

To fix this, simply redraw your hearts or use scale or copy/paste to make the curves. 

Avoid offset in sketches unless you take the time to analyze the resulting curvature.

This is not just a problem in Fusion. It is a problem in all CAD programs.

[TrippyLighting]

This is particularly bad it the curves were imported from external applications, which often don't adhere to CAD standards for precision.

[Johnc911]

Example

[luis.lange]

I understand your point, sometimes when fillet some corners in a offset curve I get some strange shapes, misalignment, but it is hard to believe that an "simple" offset get so much trouble. 

In my newer drawings I create only splines, no more importing sketches, this gives me more control, but I still have this issue sometimes.

That sketches are for cookie cutters and this offset curve is for the cutting wall. If it is better to scale up my sketch instead offsetting, how can I assure that it is aligned with "original" sketch to have a constant spacing between them (like an offset)? I cannot find a center point for the sketch.

Once ago I tried to sweep a profile over a sketch but with complex sketches (like a silhouette) this does not work.

[Johnc911]

Offset the extruded surface. Does that make sense? 

[TrippyLighting]

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@luis.lange wrote:

I understand your point, sometimes when fillet some corners in a offset curve I get some strange shapes, misalignment, but it is hard to believe that an "simple" offset get so much trouble. 

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Offsetting a "analytic geometry" is simple. Offsetting arbitrary curves in CAD is off setting NURBS and that is not trivial at all. 

Instead of working with offset splines, extrude the original spline into a surface and then offset the surface. Working with surfaces instead of with offset or projected sketch geometry generally yields out improved results and less problems.

[Johnc911]

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@luis.lange wrote:

... but it is hard to believe that an "simple" offset get so much trouble. ...

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If you're interested in more "behind the scenes" of how offsets are calculated, here is some info. Note I am not sure of the exact algorithm that Fusion uses, but any way they do it is going to have some mathematical approximation:

http://web.mit.edu/hyperbook/Patrikalakis-Maekawa-Cho/node210.html

Excerpt:

@jeff_strater  are you able to give us some insights on this topic?

[luis.lange]

I tried to create using offset faces and so on, this is the result.

They are equal in shape, but I really need to insert a fillet to guarantee some mechanical resistance. The process itself is not more complicated than using offsets, maybe I can use it in newer designs. But this design is "simple", there is no drawings inside the drawing, like this one in the pictures. So I cannot simply extrude the silhouette and forget the inside...