6 Replies Latest reply on Feb 14, 2016 6:58 PM by Mark Biasotti

    Combine zero thickness error

    John Smith

      Hello,

       

      In my - now famous on the forum - model, I am trying to combine two solid bodies, but I get the "Unable to create feature because ... zero thickness geometry". From another post, I understand that this is due to merging two solid bodies that have surfaces lying against each other. I think the problem does come from the surfaces where the bodies should join, and this is probably induced by the way I built the second body. I believed I was using the right worklow for surface modeling but apparently not.. :

       

      1. cut back part of the main body to have some room to work with and make a nice transition with the "front-support"

      2. make 3D sketches to shape the new solid

      3. use filled surfaces to form the new solid

      Note: I tried using boundary surfaces, but didn't succeed.. it always selects an entire sketch and won't let me pick just a single edge, even if I used the "plit entities" tool. So I always end up having billions of sketches where 99% of them contain converted entities from other sketches...

      4. knit them together with "try to form solid body" checked

      5. combine the main solid body with the newly created one

       

      The error happen on step 5. When zooming in, I can definitely see that both bodies don't match perfectly (see "here-is-the-problem.jpg"), though they were created with the exact same lines ! I think this is a tolerance problem as discussed in another thread I created a few days back.

       

      As I read on the thread mentioned above, I could directly merge the surfaces with the main body and form a solid body all at once, without the need of step 5. Is that really possible ?

       

      Thanks for your help !

       

      All the best,

      J.

        • Re: Combine zero thickness error
          John Smith

          Well, I found a workaround I changed the way I built the support, but the important change really is that instead of putting a filled surface at its top, I knit all surfaces with the surface of the main body created by the cut, with "try to form solid body" checked. Then I combine both solids and everything goes together quite nicely. I added a .5mm fillet on the joining edge, which makes a smooth transition, but then had to delete with "patch and delete" a face it created, nothing really complicated here

           

          Still, can anyone tell me what is wrong in my workflow ? How do you usually go about "adding" new shapes to an existing solid body using surfaces ?

           

          Thanks if anyone can enlighten me on this

           

          All the best,

          J.

            • Re: Combine zero thickness error
              Mark Biasotti

              hi John,

               

              I had a brief glance at your model. The first thing; with shapes like these you cannot model tangent surfaces against closed solid edges because solidWorks cannot understand the connection (because the solid edge has two adjacent faces to choose from. and knit tolerance gets confused as to what you are trying to merge to.)

              What would be better and more successful for you is to model the entire model as a a network of surfaces that are connected to each other and then finally solidified. Otherwise, start solid, but then delete face to make what exists a surface model with an open boundary and model your fill feature surface to that, then make solid again thru knit and/or mutual trim then thicken (as closed collection of surfaces knitted all to one another.  I also notice that you are not applying tangency for your surface features where it looks obvious that the design intent would require them.

               

              Mark