Trouble import/exporting STP, IGES -3D

Hi Coremembers,

Any ideas how to export a 3D file that initially used AI exported print/patterns to create a texture like the photo below?

I’ve tried Creo & Solidworks, so far in Solidworks I managed to create a similar looking texture, but couldn’t export as STP. I could however export as IGES, but I try to import back into both programs and it ended up crashing every time.

Any help,


If you can export as one file format but not another, you probably have some type of geometry that’s either too complex, or corrupt.

Importing curves directly from Illustrator can sometimes lead to messy geometry that may look visually correct, but might actually have some areas where the curves double back on themselves, criss-cross, etc.

If you were building something like this my recommendation would be to double check all of your curves in the sketch and make sure they are cleanly laid out. Also, if your computer doesn’t have enough RAM and it’s a very complex piece of geometry, the large file size of the export could crash the program.

Without seeing your actual geometry those are only guesses.

Thanks for your reply Mike.

Unfortunately, I already checked multiple times to see if there were any overlaps, criss-cross. But had no luck in exporting. If lines/patterns did overlap, I usually am not able to extrude the pattern, which I could do fine in Solidworks. Currently, the MAC’s RAM is 32gb.
Sigh, hopefully this can be solved with some magic.

Hi Tangofan

This is likely due to geometry that is too complex to be described well in STEP / IGES definitions.
Check your illustrator file if there are curves with tight bends, a lot of vertex points or overlaps.
Use a remove duplicates script and use simplify path on complex paths.
In Solidworks, always make sure that surfaces are offset a bit from surfaces on the target.
Also small radii and complex fills often cause errors in exporting. I hope that helps.

If all else fails install an evaluation version of Rhinoceros, those exporters work better.

Ralphzoontjens - cheers for sharing your wisdom.
If you were given these pattern AI files from a third party, would you tend to redraw sections even if it’s like the above image’s organic shape?
I’ll look into the duplicate script.

Doing this workflow in Alias there is a fit curve tool which allows you to rebuild curves using the exact tolerance or curve parameters. For almost any type of Illustrator artwork I will normally do that because even very simple geometry (The Circle in our old logo) would sometimes come across with bugs/quirks.

Rebuilding the clean geometry gives you more precise control which will ultimately let you get exactly the end result you want. I’m not sure if Solidworks has any features for reducing curve complexity within a sketch, but that could be another good place to start.

It could also be worth checking your construction/geometry tolerances. If your construction settings are too loose or tight that could cause issues during export.

@tangofan: suggestion (and maybe this is how you did the model)

  • Make only enough geometry to make a piece of the pattern. (i.e. only 15* of the geometry)
  • Bring in only one single set of curves that makes the pattern.
  • Make that a “Block” so that SW handles it easier.
  • Offset the outer surface to the depth you want the cut to be.
  • Using the sketch block extrude cut “up to surface”.
  • Once the geometry is cut and looks good, pattern the body.

Will probably be much less taxing on your system and easier to export as STEP or IGES… but also try parasolid as that is the best format out of SW.