5 Replies Latest reply on Nov 20, 2011 1:01 PM by Kevin Quigley

    Cannot Thicken Part..... Any advice?

    Thomas Le

      I imported this part in as a step file. I' am trying to flatten this part but since this sheet metal part is a surface body instead of a solid body. I used a SW add-on Software called LOGOPRESS 3F and used the face merging features. Now I' am trying to thicken this part but it is giving me an error saying Unable to thicken surface/Failed to offset or face could not be deleted. Can anyone help me out?

        • Re: Cannot Thicken Part..... Any advice?
          Charles Culp

          What is the required thickness?

          • Re: Cannot Thicken Part..... Any advice?
            Piotr Regula

            Try using the offset surface feature. You won't be able to offset the entire surface at once however you will be able to do so piece by piece. One you have offsetted the entire model in both directions you just have to knit the pieces together. Once you have two offsetted surfaces you should be able to use the Boundry Surface feature to create the edge of the part and than knit everything into a solid.

            • Re: Cannot Thicken Part..... Any advice?
              Denny Metcalf

              I'm not quite understanding what you're asking for as the file you uploaded is already 0.080" thick. You just want to bring it into SolidWorks and flatten it as a sheet metal part?


              I have the part up on my screen and am working on it but I went back to read this thread and Piotr mentioned that offsetting in both directions so now I am confused. Did you want the surface that you worked on after the body delete to be offsetted 0.040" in both directions?


              Are the ribs critical because if not this is really easy to do.


              Here's where I'm at now, but I'm going to stop and wait for you to post some more information as to what you're looking for as this is a bit labor intensive.


              • Re: Cannot Thicken Part..... Any advice?
                Kevin Quigley

                Not opened the part but looking at Denny's screenshot I'd suggest a few things:


                1. Delete all the ribs

                2. Surface Offset one side of the part with zero value offset

                3. Create sketches on the faces with holes, reference the hole edges on the sketches

                4. Delete the holes on the offset faces

                5. Knit the offset faces and thicken into a solid

                6. Cut the holes on again (using the sketches you created)

                7. Convert part to sheet metal


                I'd suggest trying to flatten that part as it is with all the ribs/gussets etc might be a problem, and they don't affect the flat form shape in any case (assuming that is all you need).