24 Replies Latest reply on Sep 20, 2013 3:54 PM by Ahmet Turan

    Splitting a Sheet Metal Part into Multiple bodies

    Clayton Schroeder

      Hi,

       

      I am trying to split a base flange part into multiple bodies using the split command, however, it does not save them as sheet metal parts, therefore I cannot flatten the new split bodies. I have already used solidworks help, and followed the steps, but I'm not getting the same result. Does anyone know the solution to this, or what I may be doing wrong?

        • Re: Splitting a Sheet Metal Part into Multiple bodies
          John Stoltzfus

          Good morning Clayton,

           

          Welcome to the forum,

           

          I don't use split sheet metal here, there may be someone else that could help you.  The way I do an assembly like that is I would have (4) four different parts, as we have one drawing per part, so I would need to dimension each individual part anyhow.  I would put what you have in an assembly and then make four new parts and mirror those parts for the other side.

           

          Later,

           

          John

          • Re: Splitting a Sheet Metal Part into Multiple bodies
            Clayton Schroeder

            And here is my split part. I can only flatten the middle section of the split parent base flange. Very odd..

            • Re: Splitting a Sheet Metal Part into Multiple bodies
              John Stoltzfus

              Good morning Clayton,

               

              Are you using a D size drawing and need to show all the flat pattern and the part dimensions or will you be doing individual drawings for each segment?

               

              If you do individual detailed 8 1/2 x 11 drawings per split part then I would suggest make individual pcs right from the start.

               

              If you split the part, you should be able to suppress the other bodies and add the sheet metal features per each split part?

               

              Hopefully someone else that does this steps up.

               

              Later,

               

              John

              • Re: Splitting a Sheet Metal Part into Multiple bodies
                Thomas Morness

                Clayton

                 

                I did not open yor file.

                 

                I don't think SW will not allow disconnected surfaces of a sheet metal part by making one sheet metal part work as two different parts.

                • Re: Splitting a Sheet Metal Part into Multiple bodies
                  Alin Vargatu

                  Clayton, I believe there is a limitation at this time for saving multibody sheet metal parts.

                   

                  First of all, in order to get sheetmetal features in the new part, you can use only this workflow:

                   

                  1, Open a new part

                  2. Insert the unibody sheet metal part using Insert Part

                  3. Break the Link to the original part

                   

                  Break links.jpg

                   

                  Unfortunately, when the original part is a multibody part, you get this error:

                   

                  error multibody.jpg

                   

                  Let's hope that this functionality will be added soon.

                  • Re: Splitting a Sheet Metal Part into Multiple bodies
                    Filipe Venceslau

                    Hi Clayton, as previously mentioned, Solidworks has limited functionality with regards to splitting sheet metal parts.

                     

                    Attached is one way of doing what you're after with one part, one drawing and multiple configurations.

                     

                    The first problem you will run into, is the limitations of where and how you make your cuts. I find it more reliable to make the cut line cross the body completely - on both ends of the cut (rather than just making the line end-points coincident with the edges).

                     

                    The second problem will be delimited by how you actually model your parts. With the part you originally submitted, I could not find a way of getting multiple flat-patterns, while I do this nearly everyday with no problems. Being that said though, the cuts I usually perform are fairly simple and while they cross bend features, they do not cross them at angles or at possibly overlapping radii (like this channel has on the step-down corners).

                     

                    I noticed your part was built in context (I do not recognize the method you used) and somehow, there's something happening within all those features that isn't allowing solidworks to recognize it as a multiple body sheet metal part, hence it not giving you the multiple sheet metal flat-patterns.

                     

                    My approach would be to try and re-model the part in a simpler manner and see if you can get your desired results.

                     

                    I must warn you though, I take no responsibility for any broken screens or injuries you may inflict on yourself from trying to get this functionality to work for you. (Don't know whether to laugh or cry when I talk about this..lol).

                    From my experience, I just stay away from all these fancy features that seem to only work when they feel like it.

                    You will have to find the right sequence of steps and stick to them, otherwise sw will be crashing quite often and no one likes that.

                     

                    Hope this helps,

                     

                    Filipe

                     

                    2.png

                     

                    1.png

                    • Re: Splitting a Sheet Metal Part into Multiple bodies
                      Brooks Peschke

                      if you split the part using planes at the breaks you want you can then just use convert to sheet metal on the new bodies and you will get usable flat patterns for each individual part.  when inserting them into drawings you will need to use the "select bodies" tab in the property manager.  you can select the them from the cut list or the graphics area.

                      • Re: Splitting a Sheet Metal Part into Multiple bodies
                        Clayton Schroeder

                        Thanks everyone for your replies. I tried many different ways to do this but nothing worked quite the way i wanted it to. Hopefully future versions of SWX will improve this functionality.

                         

                        I ended up just creating 6 different parts, and it worked fine. Not as efficient in my opinion, but there are many ways to skin a cat.

                        • Re: Splitting a Sheet Metal Part into Multiple bodies
                          Nathaniel Taylor

                          broken screens and torn shirts are the norm through solidworks 13. the ONLY way to have success is to make individual parts as clayton suggests unless you would like to just run to get dxfs only or solidbodies.

                           

                          forget bend patterns in drawings and what not. If there is a way I cant find one. It causes endless headaches.

                           

                          I have tried very hard to enable reasonable drawing to be made.

                           

                          Create separate parts. SWX does not improve in swx13 0.0

                           

                          perhaps sideskirts example above will work but i cant tell you how he did it. Properties manager? what?!?

                           

                          my part is too complicated. What I did to solve it though is save coppies of my part in every possible confuration I wanted then inserted those into my drawings and did my own annotations. what a pain.

                          • Re: Splitting a Sheet Metal Part into Multiple bodies
                            Bernie Daraz

                            Nathaniel,

                             

                            I noticed that no one asked, did you end up with multiple "Flat PatternX" features in your part after splitting?

                              • Re: Splitting a Sheet Metal Part into Multiple bodies
                                Nathaniel Taylor

                                Bernie

                                 

                                AHH correction: I did not split parts. I made new ones as if in an assembly. referencing faces of parts ofsetting planes and creating new sketchs and features from those planes.

                                 

                                yes. multiples. about ten. folded in a few directions. which is nice. yet then to make drawings is where everything begins to breakdown.

                                 

                                Its actually a very simple "sign" for a catering bisuness. And I thought to venture into unknown territory. Start simple. And try to make a multibodiy sheet metal part within one part. Its probably a better technique to just make multiple parts. from the first sheet metal part in an assembly. and I have had much sucess doing it that way yet keeping track of references becomes complicated. and then I have to open each part to export dxfs for laser cutting.

                                 

                                What happens is that SWX seems to get confused as to what flatpattern to insert after you hide the features. And if it does get it it has the orientation wrong in reference to the pattern itself. so often you end up with a flat pattern that looks like a piece of flat sheet metal viewed as its thickness. (a long line) as well none of the bend annotations carry over.

                                 

                                features pop up that were once hidden and new ones hide. very confusing and buggy. and probably linked to configurations references and what not somewhere deep within the code.

                                 

                                could be I have yet to hit the correct radiobox. What would be nice is to beable to export the solidbodies as dxfs and new parts retaining the folded features but none of the original references to the master part. keeping a nice master part that can generate multiple sheet parts rather than just dxfs and featureless solidbodies. Which is why I essentially ended up just saving new part files for each configuration I wanted in a drawing. One file for the Standard 3 view. and one file for the flat pattern.

                                 

                                For the top level flat pattern and sheet part original that exports to a drawing fine. and shows the annotations correctly.

                                 

                                I find myself more artist than engineer and tend to work myself into creative corners, discovering solidworks limitations.

                              • Re: Splitting a Sheet Metal Part into Multiple bodies
                                Bernie Daraz

                                Nathaniel,

                                 

                                I apologize, my question was directed to Clayton as the original poster. My error. But if I may, 'a very simple "sign" for a catering business' shouldn't yield this kind of difficulty. Many of us make very complex assemblies designed bottom up and top down in sheet metal and machined components.

                                 

                                When you quote that features hide and others pop up that tells me that it's possible due to the references you mention in your first sentence, there is actually a reason for that. I'm sure you're aware that 'supressing' a feature also supresses the related/constrained/equation features as well. Hiding a feature does not usually have that effect.

                                 

                                I prefer to work bottom up but have worked top down when working with supplied model or components. In this case I think I would have worked bottom up.

                                • Re: Splitting a Sheet Metal Part into Multiple bodies
                                  Laurits Peter Solvtoft

                                  I do this all the time

                                  first unfold "if necessary" your sheet metal part, then use the split tool, then use fold tool on all three or four bodies..

                                   

                                   

                                  search youtube for: Splitting a Sheet Metal Part into Multiple bodies

                                  • Re: Splitting a Sheet Metal Part into Multiple bodies
                                    Ahmet Turan

                                    I solved it this way:

                                    after splitting the part,   I am using the surfaces to re-create a sheet-metal part from the split-body-part.

                                    I then unfold it.   This way I have all the flat patterns linked to the original part and can resize etc at will..