13 Replies Latest reply on Mar 4, 2016 10:13 AM by Ryan McVay

    SW 2016 export than import back in...invalid solid!

    Ryan McVay

      Now this I just don't understand. It could be that I am doing something wrong here - at least I hope I am. I have a normal SW2016 sheet metal part. I export the part as a Parasolid. I then import the Parasolid back into SW and have the system run Import Diagnostic. The diagnostics reports many face errors. What? I just created the blasted part how can it have face errors? It won't heal the faces! C'mon this is ridiculous. Next it tells me to run feature recognition and (as expected) it says its an invalid solid.

      What the heck is going on here?

        • Re: SW 2016 export than import back in...invalid solid!
          Umberto Zanola

          I think the problem is the bend without corner relief that got exported as non manifold (ZTG)

          Look at it in wireframe and you will see a face "inside" the part.


          Btw i deleted the 4 faulty faces and I was able to sew it back to solid... indeed a strange export issue

          • Re: SW 2016 export than import back in...invalid solid!
            Dennis Bacon

            I agree with Umberto. The issue in undoubtedly with the edge flanges being fused with the base where there is no relief. There would be an issue with this no matter what version of SW you use. I suggest you create the gap prior to exporting. In my model I made it .0075 wide (approximate beam width for lasering) and it exported and imported fine. If this is going to be punched you would need a gap of approximately the material thickness for the tool. If you have a fancy tool to lance and form then theoretically there would be no gap. I doubt if this is the case but I was able to make that gap .0005 and it exported and imported (no face errors) and I was easily able to covert to sheet metal (insert bends). Probably could have gone smaller.

              • Re: SW 2016 export than import back in...invalid solid!
                Ryan McVay

                I totally agree with both of you. Now here comes the big question. If I can't create a hole tangent to planar face because of ZTG why is SW allowing the flange to be created with ZTG? When I explicitly told it to use a obround relief and SW was able to generate a flat body? Does this means that SW is not properly rebuilding or analyzing its geometry correctly? That's my big concern!


                The funny thing about this is that I was creating this dumb solid to see how smart the direct edit functions are within SW. I was able to test this part. Although I was able to pull the Parasolid into another CAD system, convert to sheet metal, it recognized the tab, flanges and hole. I was able to work on the other flanges and main tab but wasn't successful with the two flanges- I had to delete them.