6 Replies Latest reply on Dec 14, 2017 8:12 AM by Francois Boisguerin

    link BOM from an assembly drawing to another drawing

    Francois Boisguerin

      Hi solidworks community.

       

      In our office we create assembly and drawing of them.

      For each assembly, we create other drawing with detail part, usully we use A3 document size with 6 parts in it.

      here are pictures to show what I mean

       

      ENDV01F001.jpg

      ENDV01F010.jpg

      I would like to link the balloon number (and why not the quantity) of the assembly drawing to the detail drawing so that it is easier to find part and where they go for my workers.

      I don't really know how to do that. In the detail drawing, I have put a view of the assembly and add a BOM. Then in each view of the part I select properties and link the ballon to the assembly BOM. It works but the bom is not linked to the main drawing and if the pieces in each BOM are not ordered the same way, I get different number.

       

      Also I am able to add a table in the assembly model. But how to connect it to the drawing?

       

      I don't know if we can use macro to do that. I'm not an expert in macro but I'm not a beginner too.

       

      Thanks for your help !

        • Re: link BOM from an assembly drawing to another drawing
          Elmar Klammer

          Hi Francois,

           

          You can do it (even though I would not recommend it). If you setup the drawing a certain way (there are more variations possible).

          Put your assembly view and the BOM on the first page as you have shown. On the second and following page you can put your component drawing views. Now here is the trick. First RMC each component view and link it to the BOM on page one. Than you add a balloon as usual. You can use a split balloon and set it to display item number & Quantity or you can add the quantity to the balloon on the outside (fig 0).

          The balloon info is a life link. Any changes to the assembly should populate on rebuild or opening the drawing. In SW 2016 5.0 there is a bug and the link to the custom property won't show but you can get around using a note with a hidden leader as shown below (fig 2).

          Another way is to draw a table with sketch lines then add notes into the cells. The note leader is attached to one of the corners of the cell and then hidden (that makes sure the note moves with the cell size). Then use $PRPMODEL:"CustomProperty" to link it to the MODEL PROPERTY. Now select all sketch lines and the notes and make it a block. The notes will auto-populate, when you attach the leader of the block to your model (fig 3 - I left the first leader visible to show the principle, the black leader is the block leader). Be sure to avoid duplicate Attribute names for the notes or SW will throw you a wrench the next time you edit the block, complaining about duplicate names....

          There is limitations to each version...too many to list. You will have to experiment a little.

          As I said at the beginning I would not do it the way you want to simply because it's a nightmare to manage your drawing files (revisions etc.) but I can see it working in some cases. For mass production it is not suitable i would say.

           

          Good luck

           

          Elmar

           

          fig 0

          fig1

          fig 2

          fig 3