14 Replies Latest reply on Jan 22, 2018 4:44 PM by Sergio Castillo

    Multibody sheetmetal flat pattern drawings are taking forever

    Roark Summerford

      Just that. When I start a drawing packet for a multibody sheetmetal part, when I select body, then flatten part.... oh wow does it hate that. takes 2 minutes minimum of spinning blue ring for a part with 1 bend... upwards of 10 for something with a few more normal cuts and up to 4 bends.

       

      Most are convert from solid sheet metal parts, with features put in them afterwords. They unfold and fold easily, they flatten without error.... but making a print of them is the end of me. I seriously have an engine design text book I've gotten through a few chapters in the past 2 days.

       

      Any ideas?

       

      HP Z240 tower workstation

      i7-7700k 4.20GHz, 4 core

      Quadro M4000 1GB

      16gb ram

      SW18

      everything is saved locally.

        • Re: Multibody sheetmetal flat pattern drawings are taking forever
          Jim Steinmeyer

          Roark Summerford,

          The request will come up sooner or later so I will ask from the start, Can you upload your file? If not maybe a screen shot of your model tree, not as good but it may help. It looks like your machine should be fine So I am going to guess that, like some models here, there is something in the way it was modeled that is causing the issue. Just a guess but that would be where I would look first since I really don't have enough information. Of course SW '18 will limit who can help.

          • Re: Multibody sheetmetal flat pattern drawings are taking forever
            Sergio Castillo

            I have the same problem.

            also when i try to export flatten dxf files.

             

            following this post.****

              • Re: Multibody sheetmetal flat pattern drawings are taking forever
                Roark Summerford

                My work around here recently for getting dxf's is to use "flatten" button... the model visually flattens quickly then right mouse click, export to dxf, face... works fast.

                 

                The only hiccup to that I have found is when opening it on my waterjet software is that complex curves fail. I'm not sure if it's solidworks or Flow but I can fix it in solidworks... In that case waiting for the export tool to unfold helps... but the best is to use the unfold button, as it seems to generate a better flat pattern than flatten or the export tool.

                 

                But I have no answer for making prints yet. The reps will be here in an hour or so... I'll post an update if we discover anything.

                  • Re: Multibody sheetmetal flat pattern drawings are taking forever
                    Sergio Castillo

                    good luck with the rep.

                     

                    my process of exporting dxf files will still be slow, since i have a multi body part and can only flatten one part at the time.

                     

                    quick question.

                    what industry do you work on? 

                      • Re: Multibody sheetmetal flat pattern drawings are taking forever
                        Roark Summerford

                        I've got 131 bodies in my multibody part and making dxf's go pretty fast the way I described.

                         

                        The reps sat down and had a look at the file... 1.5gb to my surprise. Turns out when it tries to make a flat pattern for a drawing solidworks "has to" rebuild all of the configurations. In this case, every body, including identical, and mirrors are individually rebuilt. That said there are 1023 flat pattern configurations that "has to" be rebuilt every time it pulls a flat pattern.

                         

                        We talked about saving bodies, but the saved body of a flat pattern looses my sheetmetal bend/flat pattern information... which is worthless to say the least.

                         

                        So It's getting sent up the chain to SW to see if they can:

                        a: keep solidworks from having to rebuild every configuration every time a flat is made (freeze bar does nothing to effect this)

                        b:enable the sheetmetal information to be transferred out in "save body"

                        c:I told them while they are at it please figure out how to get prpwld$: to be an option on the drawing sheet formats for a selected body!

                         

                        As far as industry... I mostly make my money with defense, but this is commercial automotive and highly proprietary... not to mention impractically massive to upload.