8 Replies Latest reply on Oct 11, 2015 7:19 PM by Patrick Sheehan

    creating hole template from dome surface

    Patrick Sheehan

      hey all,

       

      Our client has provided us with a 3d model of a dome that they are building and asked to cut out the holes as required. What I want to do is create a 1mm sheet metal template with 5 elliptical holes in it that I can position on top dead centre and fold over on the dome so that we can scribe the holes and cut through precisely where they have to go. Where I am coming unstuck is that I can't work out a way to produce a sketch based on these holes, that I will be able to flatten out and export to the laser cutter.

       

      Does anyone have any ideas or pointers? I've done a fair bit of googling but haven't come up with much. Attached is the solidworks part file.

        • Re: creating hole template from dome surface
          Thomas Morgan-Witts

          Do you mean kinda like this?

          Obviously the holes aren't quite right with the imperfections on the diameter.

            • Re: creating hole template from dome surface
              Patrick Sheehan

              That's something like it. Is it possible to flatten the swept part so that a flat pattern template can be generated for the laser cutter?

               

              Can you also give me a bit of a run down on how you did it, as I can see we are going to get a few of these jobs come through the workshop in the near future.

                • Re: creating hole template from dome surface
                  Thomas Morgan-Witts

                  As far as I know, the solidworks sheet metal functionality doesn't like creating more complex curves like that, instead limiting to straight bends, though I'm sure one of the more experienced sheet metal people will correct me on that.

                   

                  As to how I did it, I rolled back the feature tree to before all the holes were added and then created a sketch on the front and right planes, using the intersect curve command to capture the curve of the dome. Then in the right plane (or whichever one you want to be thinner) I offest the curve by the 1mm thickness you decided and then trimmed to size. Then you simply use a sweep feature to sweep the sketch on the right plane along the one on the front plane.

                   

                  I'm kinda hoping that Deepak Gupta or someone else of that caliber will come in and save the day on the unfolding though.

                   

                  That being said, one somewhat unsavory option is to actually do the math of what the side lengths would end up being and then creating the sketch by hand.

              • Re: creating hole template from dome surface
                Dennis Bacon

                This is an interesting issue. I made a sheet metal part that wraps over the dome in one direction (lofted bend). I used 3d sketch to put (3) points on the edges of the holes and then created planes using the points to define them. Then converted the hole edges in your part to those planes. I actually did more work than I needed to in retrospect (added more planes than I needed). I could have made a snug fitting Swept Flange (compound curve) but with 2015 the holes do not transfer to the flat pattern. I also have 2016 and in that version the holes do transfer. It looks like you are using 2015.

                You might be able to clamp the sheet metal part to the dome and hammer it around to make it work. Or use 2016. I have been playing with it today and it is a bit flakey but does work.

                 

                Perhaps the attached file will give you some ideas.

                 

                You can use the sheet metal flatten tool to flatten the sheet metal.

                 

                Edit: Looks like Thomas is using 2015

                • Re: creating hole template from dome surface
                  Kevin Pymm

                  Patrick,

                   

                  Not sure if this helps you in any way but in SW 2016 you are able to do a surface offset of 0 & then do a flatten surface. In SW 2016 holes are now included in flatten surface, previous versions didn't include any holes.

                  • Re: creating hole template from dome surface
                    Patrick Sheehan

                    Thanks for all your responses guys.

                     

                    Dennis, I've adapted your ideas a bit so that I could make two parts and overlay them 90 degrees to each other so that I could get the sheet metal to fold in two directions. Exporting both of these to dxf files meant I could then remove the overlaps and create a pattern that is going to be accurate once folded down.

                     

                    After all the issues with this template, we're now upgrading to 2016 premium, so that the future jobs can be done a lot easier.