8 Replies Latest reply on Jan 28, 2010 2:21 PM by Mauricio Martinez-Saez

    Flatten a Part using sheet Metal

    Piyush Sharma
      Is there any way one can flatten the attached part using sheet metal. I am pretty new to sheet metal and would really appreciate your suggestion.
        • Re: Flatten a Part using sheet Metal
          SW will not convert this kind of geometry into a sheet metal part. The problem is that the bends are not flat, they are curved around the centerline of the part while they bend. SW cannot unfold this kind of sheet metal forming. SW will only handle flat formed flanges, like what you would be able to do on a press brake with standard tooling.
            • Re: Flatten a Part using sheet Metal
              Mauricio Martinez-Saez

              37503 wrote:

               

              SW will not convert this kind of geometry into a sheet metal part. The problem is that the bends are not flat, they are curved around the centerline of the part while they bend. SW cannot unfold this kind of sheet metal forming. SW will only handle flat formed flanges, like what you would be able to do on a press brake with standard tooling.

               

              SW Sheet Metal can produce (and unbend) flanges formed with a curved folding line.  See attached picture and part file (which unfold to a perfect flat pattern).

               

              Picture-01.JPG

                • Re: Flatten a Part using sheet Metal
                  While I was surprised to see this, (I forgot that I did get SW to do this before a long time ago) SW will not handle the second bend because the initial face is non-planar. Apparently you can go from flat to curved but not curved to curved. The Convert to Sheet Metal feature does not appear to recognize the flat to curved bend for the same reason ... it gave me the attached error dialog.
                    • Re: Flatten a Part using sheet Metal
                      Mauricio Martinez-Saez

                      Shawn,

                       

                      The part I posted is not "converted" is is a 100% done with Sheet Metal features and fold / unfold correctly and without any errors.  I do not understant from where are getting the error.

                       

                      Attached is another "exotic" thing you can do with sheet metal... (or SW), the attached is an example of a "bended" honeycomb pannel (which is a 3 layer composite). Open the assembly and change the configuration from "default" to "flat" (this will take sometime depending on your machine, since it will need to regenerate the "honeycomb", but it works).

                        • Re: Flatten a Part using sheet Metal
                          I think that the first question shouldn't be can this be flattened,  but should be "How are you planning on manufacturing this?".  For example, if you are planning on forming the flanges then you should redesign the part to match how it is going to be manufactured.  If this part is going to be punched out then you should design it to match that process.  Most likely it will be punched out.  If that is the case, then SolidWorks does not really handle punched out parts very well.  Good luck!
                          • Re: Flatten a Part using sheet Metal
                            I was referring to the original posted file, not your example, but it applies to your example as well, if you try to make a second flange on the ends of your sample, SW will not create them because the initial face being formed is not planar.
                              • Re: Flatten a Part using sheet Metal
                                Mauricio Martinez-Saez

                                The problem my friend, is that curved-to-curved forming is not a Sheet Metal bending forming process it is a Sheet Metal Stamping process (in fact a flat-to-curved is also a stamping process) and as you already mentioned on a previous post, SW Sheet Metal module is (as it is on all other CAD systems I know such as Pro-E, Catia, Alibre, etc.) a module to use for "bending" processes.  In fact, even when SW allow to do a flat-to-curved flage, the flat pattern produced by SW cometimes is not good at all since SW can not calculate the deformations of the material on this type of forming.

                                 

                                You are correct, SW Sheet Metal module is for press-brake (or any other straingth line bending) formed parts, not to model parts to be produced by stamping or deep-draw forming.  SW allow the use of "tools" to do this, but it can not produce the "blank" required to produce the formed part.

                                 

                                For example, one of th products we manufacture is Hermetic Refrigeration Compressors, on which as you know  the casing is build with two dep-draw shells, for that we have a special software which produces the blank requred for the formed part (modeled in SW and exported as IGES), SW can not do that type of work.

                      • Re: Flatten a Part using sheet Metal
                        Pankaj Bir

                        Dear Piyush,

                        A work around solution for your problem is possible with Solidworks.

                        The solution to your problem lies in modelling two separate sheetmetal bodies and then flattening them individually.

                        The combined flat pattern is the solution to your problem.

                        If you are using Solidworks 2010 you can do everything in a single part file. However if your are using any other

                        version you will have to model two separate parts to accomplish your requirement. The lock washer can be modelled

                        and flattened though.

                         

                        Find the solution attached.

                         

                        Pankaj Bir