10 Replies Latest reply on Sep 28, 2015 7:59 PM by john teng

    Unfold a metal strip for ease of fabrication drawing

    Amruthkiran Hegde

      I have a solid model of a metal strip rolled to a certain radius with holes punched at a fixed distance in a circular pattern across its circumference. For ease of fabrication, I would like to unfold this to the original straight metal part while creating the 2D fabrication drawing. It would be great if someone can advise me on this. Thank you.

        • Re: Unfold a metal strip for ease of fabrication drawing
          Mike Helsinger

          There are two approaches I take when I handle something like this.

          1. Use the Convert to Sheet Metal tool

            You will need to select a flat face or straight edge to use this tool.  Pick SELECT ALL BENDS to collect the entire part.  Confirm your part's characteristics (thickness, K factor or bend allowance).  After using this tool take a look to confirm that your features are as they should be.  Example, if there are countersinks, this tool would remove them, or if the perimeter on one side is different than the perimeter on the other side you may not get the exact representation you need.
            If you cannot complete with this method - some geometries don't agree with this tool, go to method 2.

          2. Recreate the model in sheet metal.

                         Start a new part with the basic shape of the part you need to make.  Save this new file.

                         Create an assembly file mating your new working file to your target file.
                         Modify your new sheet metal part to match the target part, this can be done in the assembly file.  Change the transparency of the parts to help                compare your parts.

            • Re: Unfold a metal strip for ease of fabrication drawing
              Amruthkiran Hegde

              Thank you Mike for the response. The first approach worked and I was able to convert my solid model to sheet metal but how do I visualize it back as a straight strip? (I tried using the unfold option but since the sheet metal is rolled and has no bent edges that option did not work)

                • Re: Unfold a metal strip for ease of fabrication drawing
                  Mike Helsinger

                  If the entire part is rolled it gets a little more complicated.  Could you attach your file so I know exactly what you are trying to tackle?  In you are unfamiliar with attaching on this forum, you can do that by picking USE ADVANCED EDITOR in the upper right corner of your reply window of this webpage.

                    • Re: Unfold a metal strip for ease of fabrication drawing
                      Amruthkiran Hegde

                      Hello Mike,

                       

                      I have attached the file to this reply. I basically have a circular strip with a pattern of holes that need to be punched. But in reality, the circular ring will be made of two sections, i.e., at the beginning of fabrication, a bar of metal is cut into the required length, the holes are then punched and the bar is rolled to the required radius. The same procedure is adopted for the other section. Hence, I am kind of reverse engineering the whole thing, i.e, from the circular ring with the punched holes, I am trying to arrive at the right length of bar that is needed, by using the sheet metal option.

                        • Re: Unfold a metal strip for ease of fabrication drawing
                          Mike Helsinger

                          Good, I think I understand, and it's a bit easier than I thought it might be.  You have a 5" thick bar that is rolled the hard way into a R84" half circle?  There are multiple ways to get there, here is how I would do that.  Sketch your half circle, just a single arc, and make that sketch your Base Flange of your sheet metal part.  Make sure you check your K Factor / Bend allowance, your flat length depends on this.  Get everything looking right and then observe your feature tree.  Instead of unfolding your part to get your stock length, I find that is more proper to work with the Flat Pattern feature.

                           

                          A little more about sheet metal:

                          If you were to create a drawing file from your sheet metal part, you should notice that in your configuration tree you have a derived configuration that is named SM-Flat-Pattern.  This configuration is automatically created by unsuppressing the Flat Pattern feature.

                          This would allow you to have a drawing that can display your flat and your formed part simultaneously without having to bounce between folding and unfolding your part.  This has great value in the sheet metal world.  For you, if you don't need the drawing you can view the flat part this same way, unsuppress the Flat-Pattern1 feature.

                            • Re: Unfold a metal strip for ease of fabrication drawing
                              Amruthkiran Hegde

                              Hello Mike,

                               

                              I was wondering why the holes that need to be punched disappear on switching to Flat-pattern view

                                • Re: Unfold a metal strip for ease of fabrication drawing
                                  Mike Helsinger

                                  Check the face under your Convert to Sheet Metal feature.  If that face has holes they will translate over to your sheet metal part.  Or depending on what surface you used to convert, if they aren't present on that surface you will loose them & need to replace them after you convert.  If you can't select a face with holes you can mark the hole locations on an independent sketch, then convert, then use your marker sketch to locate the holes later.

                                   

                                  The convert feature works by replacing the previous model geometry with a sheet metal representation based on the sketch within that feature (the face you selected to start the feature).  Whatever face you choose becomes the new part definition, and this can change your part due to chamfers, fillets, countersinks, etc.  Keep this in mind as you model, use the convert to sheet metal feature as soon as you reasonably can.  Once you get comfortable with sheet metal modeling I recommend you use the tools under the sheet metal toolbar to build your parts, and convert only when necessary.

                        • Re: Unfold a metal strip for ease of fabrication drawing
                          john teng

                          Hi,

                           

                          Solid3dtech.com has a plugin to unfold such surface. The plugin can unfold single or multi-face surface into a single contour.

                        • Re: Unfold a metal strip for ease of fabrication drawing
                          Tateos Tvapanyan

                          Hi,

                           

                          Make "Extruded Boss" in one of the ends. After that use "Convert to sheet metal" tool and at the end "Cut" the added before "Extruded Boss".