3 Replies Latest reply on Aug 21, 2014 6:37 PM by Paul Cullen

    Knitting Challenge(d)

    Bjorn Sorenson

      Can't get the attached part to form a solid and I'm hoping to keep my feature tree, so I don't want to do the export/import/import diagnostics dance.  I've tried a number of ways and am getting some curious error messages that I'll leave it to you to discover.  Any surfacing experts out there care to tell me what I'm doing wrong?  Thanks in advance!

        • Re: Knitting Challenge(d)
          Devin Weston

          I'm going to have to ask first why you are trying to do this with surfaces. From what I'm seeing, you could easily model this as a solid in SW.

          • Re: Knitting Challenge(d)
            Jamil Snead

            Here you go. The problem was that your sweep didn't follow the exiting edges very well, so there was some weird sliver faces happening. It's really hard to tell unless you zoom in super far.


            So then after you delete faces the remaining surface is weird along that edge. Notice how the edge is black and blue instead of just blue. It has that sliver in there too.


            To fix it I just unchecked merge result in your sweep to keep it a separate solid body. Then I went through and updated the feature scopes of the features that needed to cut the new body. I edited the delete face feature to include the bottom of the sweep and the top of the base the faces that are touching each other between the two bodies). Then I just updated the relevant edges in the boundary surface. With all that changed the surfaces were able to knit and form a solid.


            By the way, you don't need to make those composite curves. In the boundary surface you can use the selection filter to select a combination of edges. When you are making the selections for the boundary surface you can right click, then choose Selection Filter, then pick the option that shows 3 cursors, then select all of the edges that you want included in that single selection, then press ok.

            • Re: Knitting Challenge(d)
              Paul Cullen

              Hi Bjorn


              It is your sweep feature that is messing up your part if you look at your part after the sweep the inside edge is irregular and not made up of a continuous curve see highlighted edges in the picture below

              Failed Sweep.JPG


              As I am using SW 2014 and you are using an earlier version I cannot send you a repaired file so I will try and explain what I did below


              Firstly I edited your sweep feature but instead of selecting your sketches for the guide curve and path I selected the inner and outer edges of the body

              New Sweep.JPGNew Sweep 1.JPG

              This then gave me a continuous curve on the inside edge of the part. To quickly clean up the part where the sweep did not come flush with the end on the left hand side. I did a surface cut using the top plane and then mirrored the part and merged it together again. There is probably other ways to clean up that edge but this is what first came to my mind. I then rolled forward your cuts 5,6 and 7 and made any necessary changes for missing edges, vertices, etc.


              Surface Cut.JPGMirror.JPGCuts.JPG

              I then deleted the faces as you had done and created the boundary surface

              Delete Face.JPGBoundary Surface.JPG


              Then doing a knit surface I knitted the surfaces and created a solid

              Finished Part.JPGFeature Tree.JPG


              Hope this helps