6 Replies Latest reply on Aug 8, 2018 11:08 AM by Dan Pihlaja

    Creating identical parts/assemblies but with different lengths.

    Robbie De Smedt

      Hello,

       

      To complete our library, I would need to create a lot of these:

      This is an assembly, made out of these parts (I'll give them a nickname):

      - Flat fixings

      - base tube profile

      - clips

       

      The lengths I'd need go from 100mm to 5000 mm easily.

      It is the base tube profile that must have the diferent lengths. This must be populated by clips. And in a set distance be populated with flat fixings.

       

      What would be the best way to make these parts or assemblies? I think it would be ridiculous to make the part 'base tube profile' with 1000 configurations (with design table?) for all the different lengths and then using it in the assemblies, or not?

       

      I'd love to hear your feedback.

       

       

       

      Greetings

        • Re: Creating identical parts/assemblies but with different lengths.
          Josh Brady

          -As far as part vs assembly goes, if you ever need to create a BOM, parts list, count of clips and flats,etc. then you probably want an assembly rather than a part.

           

          -Your picture shows 5 "clips", but it looks like it's supposed to have 6 and it's just been cut.  The other "flat fixing" is cut short as well.  Do you want this?  Do you have single/double/triple clips, or are they all triples?

           

          -Are your lengths infinitely variable and you just cut them, or do you have discrete values like integer number of clips etc?

           

          I would recommend a design table for lengths, then set up component pattern features in the assembly that are driven by the length of the tube profile.

           

          When you create configs using a design table, there's actually very little overhead.  SW only builds the config when you activate it.  Once a config is built, SW saves the geometry and display info to the file, so it starts getting bigger.  If I recall correctly, doing a File->Save As... will purge a bunch of that data, making the file small again. You can create a design table with thousands of rows that's incredibly complex, but the part file will not be large until you actually activate lots of configs.

            • Re: Creating identical parts/assemblies but with different lengths.
              Robbie De Smedt

              Hello Josh,

               

              Thanks for the info. To give an answer to your questions:

               

              We have 'clips' existing of 3 and 5 clips in total.

              The 'flat fixings' can be 50mm or 70mm long, but 50mm most of the time.

              The lengths can be infinitely variable.

               

              The design table for the lengths should be made in the 'base tube profile'-part?

               

              The component pattern features driven by an equation made in the assembly?

               

              Greetings

                • Re: Creating identical parts/assemblies but with different lengths.
                  Josh Brady

                  Robbie De Smedt wrote:

                   

                  Hello Josh,

                   

                  Thanks for the info. To give an answer to your questions:

                   

                  We have 'clips' existing of 3 and 5 clips in total.

                  The 'flat fixings' can be 50mm or 70mm long, but 50mm most of the time.

                  The lengths can be infinitely variable.

                   

                  The design table for the lengths should be made in the 'base tube profile'-part?

                   

                  The component pattern features driven by an equation made in the assembly?

                   

                  Greetings

                  So I guess the real question is... What do you want out of the model?  Is it just visual, and some dude will grab parts out of a bin to assemble as needed, or do you really need to know how to make it, and what spacing to use?  How do you decide when to use a 50 and when to use a 70 flat fixing?  If length is infinitely variable, how is the thing made?  Do they assemble however many clips to make "extra" and then cut, like what your screenshot shows?  You mentioned clips come in 3 and 5... The screenshot you posted shows 5 clips, but it's made with one 3-clip unit and another cutoff one.  Why not a 5?  How do you decide when to use a 3 and when to use a 5?

                   

                  If you need to show an assembly, then yes.  I would make a design table in the base tube, then equations or something for the component patterns in the assembly.

                   

                  If you really don't care about the part list or whatever, you could do the whole thing in a part with patterns of extrudes or bodies etc.

                   

                  It all just depends on your design intent.

                    • Re: Creating identical parts/assemblies but with different lengths.
                      Robbie De Smedt

                      Perhaps this will be a better (and longer) example:

                      These are old models, but I want/need to remake and automate these assembled components so they represent a perfect BOM and are visually correct. Even with cost-calculation per part that is used.

                       

                      The length of the 'base tube profile' should be chosen from the available configurations.

                      This length should decide how many 'clips' will be used in the assembly. Driven by a component pattern equation.

                      The 'fixings' will also be driven by a component pattern equation.

                • Re: Creating identical parts/assemblies but with different lengths.
                  Sergio Monti

                  Hi Robbie,

                  I have the same problem when using partial lengths of some bought-out profiles in our machines.

                  What I usually do is to create only 1 part for the 'base tube profile' having the maximum length.

                  Then use cut-feature in assembly (this is what you do in reality to manufacture the parts) and change the quantity to be used in BOM at the assembly level:

                  You can also change the UnitOfMeasure in metres, or inches, or whatever you want.

                  There are may other better ways to do it, but this works fine for me so far.

                  Hope it helps.

                  • Re: Creating identical parts/assemblies but with different lengths.
                    Dan Pihlaja

                    Use Configuration publisher with a single line design table:

                    SolidWorks Configuration Publisher: Taking File Configuration to the Next Level

                     

                    Then your configurations will be created on the fly as you need them.