11 Replies Latest reply on Feb 4, 2011 11:45 AM by Shawn Casebolt

    Multibody BOM

    Shawn Casebolt

      Is it possible to create a drawing of a multibody part and have a BOM with item #'s for each different body?.....furthermore, have columns linked to there dimensions?

       

      Think of simply like a wooden drawer, 5 bodies (front, back, left, right and a bottom).  This is modeled as a part.  Now I want to create a drawing that has a "cutlist" for the boards I need to make the drawer.

       

      Is this possible?  Right now I believe I need each piece to be a seperate part in an assembly.

       

      Thanks.

        • Re: Multibody BOM
          Scott McFadden

          Shawn,

          You would be correct.  Considering BOM's are marametrically driven from assemblies and

          not parts the only way to do it would be to manually contruct it and it would not be parametric.

          • Re: Multibody BOM
            Kelvin Lamport

            Change the drawer to a Weldment (Insert > Weldment > Weldment) and then use a Cut List instead of a BOM

            • Re: Multibody BOM
              Alin Vargatu

              Listen to Kelvin. Insert a Weldment feature inside your part and it will work.

              • Re: Multibody BOM
                Andrew Hall

                Try using the a Cut list table, this is intended for weldment parts but can be used to list bodies in a multi body solid.

                 

                To get the insert cut list option to become available you will have to create a weldment feature, im not sure if you can do this without creating a structural member but if you create it then delete it you still have the option of making a bom, you will also have to right click on the cut list in your part feature tree and select update to get the bodies to appear on the parts list, you can then add descriptions and custom properties to the "cutlist"/bom by right clicking on the item in the cut list in the part feature tree and selecting options.

                 

                it is a little bit cumbersome but will be parametric and will produce a list of bodies.

                 

                Alternatively you are able to push your bodies into an assembly as individual parts from the save as part dialog however i am not too sure what happens if you add a new body to your original part.

                 

                If some one from solidworks reads this perhaps we could sneak some bom functionality into the multibody solid part feature set, and maybe even an exploded view feature?

                • Re: Multibody BOM
                  Shawn Casebolt

                  That worked perfectly!!!  I never thought to do that.  I have all properties I need.  However, this has brought another question.

                   

                  On sheet 2 of my dwg, I created a view of two of the "bodies", by using, insert-> view-> relative to model

                   

                  On the first view, I inserted a balloon, which gave me the item number, perfect!  I inserted another balloon, and changed its properties to description......works perfect, and a third for the finish.  All work great.

                   

                  My problem is, I want to copy and paste these 3 "balloons" to the other view and have it read the correct properties.  However, I get a ? mark in the balloon.  Is there a way to "attach" it to the other view?  The reason for this request is that they are customized.......no border, larger and bold font, etc..  So it will be cumbersome to do this to all pieces.

                   

                  Thanks Guys

                  • Re: Multibody BOM
                    Shawn Casebolt

                    Nevermind, copy and paste will work.......just have to do all 3 individual