I am trying to extrude an exported DXF from illustrator. When extruding, i get the "unable to create extrusion.... due t geometric conditions" error. The full image was quite complicated, so i removed all the details and just did the text portion and i am still getting the same error. I tried using the sketch tool to 'check sketch for feature' and there were no errors.
How do i solve this?
PS: I would just like a simple 10mm extrusion of the entire image.
I have attached the complicated dxf of the logo, just the simplified text portion and the imported solidworks file of just the text portion
Hi John,
There are some extremely small segments in these sketches. I've only worked on the text only one and there are 89 sketch segments less than 1mm long and one as small as 0.00179349mm. These will certainly cause problems when trying to extrude and even if it could extrude, you are likely going to end up with downstream issues depending on what you are trying to do with the extrusion.
Just to troubleshoot it, what I did was selected the sketch and made a Planar Surface out of it (available on the Surfaces tab of the CommandManager). Once I have the surface, then I used the Geometry Analysis tool on the Evaluate tab and set the short edges value to 1 mm, left all the other things as default, and then hit Calculate. The result is 89 edges less than 1 mm, 2 knife vertices, and 8 discontinuous edges. I would concentrate on the small edges first. In the analysis results, you can expand the small edge listing and see they are sorted from smallest to largest. If you start zooming in on these, you will see how small they really are; these are not suitable for solid modeling since you would never want to manufacture those small edges (now could you in reality by any manufacturing process. You may want to also clean up the knife edges as those often will cause problems in solid modelers, and again aren't really manufacturer. If you zoom in on the knife edges it highlights, you see what a knife edge is; 2 entities coming together at a very small angle.
Unfortunately, I am not aware of any automated tools in SOLIDWORKS to clean this up so you may have to do it manually if you need to work with what you have. As you can tell since I had to make a surface out of it even to analyze the geometry, SOLIDWORKS does not have the tools to analyze and repair sketches that are not relatively clean; it has some tools, but not ones for finding an eliminating small edges; at least not that I am aware of. Someone else may know better.
If you can, I would go back to Illustrator and use the tools there to generated a much cleaner vector outline of the logo without all the small edges.
I hope it helps,
Jim