8 Replies Latest reply on Mar 1, 2017 7:56 AM by Mattew Stafford

    Lofted Bend Issue

    Mattew Stafford

      Perhaps I am going about this the wrong way.  I am really new to sheet metal.  The image below represents what I am trying to accomplish, but I am getting an error message: "The bend may be fused with other bend.  To remove this problem try to 1) reduce radius for this feature or 2) Change Facet Value.

      I have (2) open sketch's. The top sketch is a 3d sketch and the bottom is a regular sketch.

      The top sheet metal feature looks correct, but when I want to create the transition, I get errors.  Even if it did work, does this transition piece connect to the top part?  It would be ideal if it did.

        • Re: Lofted Bend Issue
          Mattew Stafford

          After conversation with my VAR, it was determined that what I was trying to accomplish is not possible, because: "...the sheet metal piece could not be created because it was a multi-radius bend. Unfortunately at this time SOLIDWORKS is not able to handle those types of

          bends."

          • Re: Lofted Bend Issue
            Casey Bergman

            That is a pretty tricky part.  One thing that I have discovered over the years of making transitions like this is that Solidworks still can't make this with the material toward the inside of the profile.  I used the inside of the material to create the sketch and then used a smaller bend radius and it will work.

             

            I have turned this into my VAR and requested this enhancement years ago but it still has not been addressed.  It doesn't make any sense to me, it is the same part.

              • Re: Lofted Bend Issue
                Mattew Stafford

                Thank you Casey Bergman & Dennis Bacon.  Both are viable solutions to what I was trying to accomplish and both touched on the biggest problem.  I was using the outside profile to create my sketch, when I should have used the inside.  Offsetting certain geometry "inward" is a common problem with other software as well & like you said, it is the same part.  I should have remembered that from my years of experience in surfacing.

                 

                Dennis Bacon, I am not sure why there is a beveled cut on Boss-Extrude1, I am not seeing it on my end.  I actually was trying to have 3/8" material & it appeared as it was 3/8" per the dialog box, however, by changing it to decimal units it does show up as .394".  Most of our drawings have architectural units & are burn-out plates, so by keeping the units as architectural in the base model, the properties show up properly in the BOM.  It looks like one downfall to doing that is what I just experienced...the .394" is rounded to 3/8".  Either way, I am good to go now!

              • Re: Lofted Bend Issue
                Dennis Bacon

                Here is a slightly different method. I added a line onto sketch137 and made a parallel relation with the corresponding line on your 3DSketch2. Reordered the sketches to do that.Then filleted it. Then between an unfold and fold I sliced off the additional material. It does take some horsepower to flatten this probably do to the computations necessary as it slices across the bends in the lower right. The result is good looking bends without the gap developing. I'm assuming you wanted the material thickness and radii to match your Base-Flange2 (.394") I changed the units in this file since the fractions were driving me crazy. I also added a dimension to control the bottom length. You have a beveled cut in your Boss-Extrude1. Not sure what that is for or if you intended it to be beveled.

                I'm also assuming that a "Formed" option will not work for you.