When merge result is checked error message pops-up. When it is unchecked correct result is coming. What is the reason for that?
Round math is more difficult than rectangular math. The interesting thing about this particular problem is that if you make the extrude sketches the same length, the problem goes away. You can vary the dimensions between them slightly and things will be okay but at some point it fails. I'm also disturbed by the weird concave nature of the extruded surface that gets worse depending on how far around the circle the geometry goes:
You can see what's happening when you look at it end on in hidden lines mode:
That doesn't look right at all. If I construct the model using no split lines but just projected curves, it is better but still there:
You can avoid all this nonsense by using the right tool for the job: Wrap
And the feature tree is greatly simplified:
It shows that you will have a "Zero Thickness Geometry" issue likely out on the end of the radius. A work around to try with the merge checked is to add a 1mm depth in the 2nd direction.
Problem is with this type of shape there is no this problem. What is the reason for that?
It is kinda hard to explain what is causing the error but it has to do with where the 2 arcs are meeting.
Another option would be to just do an extrude from the midplane and make it offset from the surface
Thank you for your explanation.
2017 SOLIDWORKS Help - Error Message - Zero Thickness Geometry shows some examples of where this can happen, but Dave Dinius' solution will work. When I run into this, I always make the solids overlap, if that makes sense.
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