Hello,

I'm using SolidWorks 2013. Please take a look at the part I'm uploading. Here's a screenshot of it:

What I need to do is to chamfer all 4 long edges on this part so that there are 8 sides instead of 4. However, this chamfer should be of variable width, as it must follow this kind of sketch throughout the whole length of this part:

Meaning that chamfer would be smallest at the top, largest at the maximum thickness of this part, and varying in width according to the curvature.

I tried using Chamfer feature, but it results in errors and doesn't give any kind of result. I could re-Loft the part with this sketch, but it's almost impossible to make Loft follow the exact curvature of this part without creating complicated guide curves.

Can anybody please advise? How should I chamfer these edges proportionally to this sketch?

Thanks in advance!

J.R.

My initial thought was that you should just extrude an acute isosceles triangle with the vertex angle equal to 360/number of sides you want. Then cut the base of your extrude to the lengthwise profile and circular pattern it for the complete shape.

But, then I looked at your model and realised you are working with imported geometry and perhaps don't know exactly what the profile should be. I think a simpler approach to your problem, since you want the profile from the imported part, would be to make a circular pattern of the "square" body and use the "Combine" feature to get the final shape.

Either roll back to before your Body-Delete feature so you can use the temporary axis of the round body, or create an axis with the front and right planes.

Then, Circular Pattern the square body around the axis (e.g. 2 times at 45° for octagon, or 4 times at 22.5° for hexadecagon).

Finally, use the Combine feature, select all the "square" bodies and check "common" for the Operation type.