6 Replies Latest reply on Mar 14, 2015 10:32 PM by Bernie Daraz

    Link drawing note to different part file

    Rebecca Fetter

      When I have parts that need to be cut to mate each other (say, two pinion racks need to be joined for overall length), we put a note on our drawings saying "Mate with XX" where XX is the name of the file the mating part is in.

       

      Is there a way to get that to change dynamically in case part file names get changed? I know I can link the properties of the part to its own drawing, but can I link to properties of another part not in the drawing?

       

      Thank you

        • Re: Link drawing note to different part file
          Jamil Snead

          There might be a simpler way, but you could add a drawing view of that other part to the drawing, and move it off the sheet. Then you can make a note with the leader pointing to the part and link part of the note to a property of the "Component to which the annotation is attached". Then hide the leader and move the note wherever you want.

          • Re: Link drawing note to different part file
            Timothy Taby


            Create a view of the part you want the note to refer to and then add the note to that part using the "Link to Property" and select model in view to which the annotation is attached, then select the propertity you want the note tinclude.  Then, you can add other "Link to Property" that is Model in view specificied in sheet properties and select which property you want to show there.  THis will only work with 2 parts though, one that is attached to the sheet and the other attached to the view.

             

            C1.png

            In my drawing above the TL021534C1 is the part number for the assembly which is attached as the view to the sheet, the note is attached to part TL021534C2, hence the way the note is made.

            • Re: Link drawing note to different part file
              Bernie Daraz

              At the place I was before they wanted all of the 'connecting' parts as well as the next assemblies related in the drawing files. I used 'Configuration Specific Properties' and had a Property named "NextAssy" (and "TopLevel") where I listed the part number, etc. From there it was easy to back up a step and show those on the drawing using those properties. In my current environment I would build your assembly as a Weldment. Parts are then different 'bodies' of that weldment. The 'other' part number you show isn't necessary as it is just item 1, 2, 3 and so on of the 'master' part number. You're basically showing that now as ....C1 and .....C2. Of course your company may have standards in place and require you to do it that way. The highest number of unique parts I have had in a weldment is probably around 20. Others on here can speak to much higher numbers as well as lower. The weldment BOM or cultist will track the item counts for you based on the number of the same bodies.

               

              Sorry I was referring to the drawing above my reply.

              • Re: Link drawing note to different part file
                Timothy Taby

                You can use Configuration specific properties like Bernie said, but they won't change dynamically.  You could do it programmaticly using API calls, but that is some pretty high level stuff.

                • Re: Link drawing note to different part file
                  Bernie Daraz

                  This is about how I would make this part, it is a weldment. It's not proper drawing format to have all those notes all over the place. You can attach a part number to a weldment body like I did and it will automatically fill in the BOM. OK, so the scale of the views is off, I didn't show dimensions and Description should be Material. It's my day off! LOL!

                  weldment forum.JPG

                  • Re: Link drawing note to different part file
                    Bernie Daraz

                    I just remembered I had my old notes that were linked to the part properties from an earlier position, the BOLD notes refer to the custom properties I set up there. I deleted some unrelated and proprietary notes so the order is off. As I inserted a part or an assembly these would update automatically and they would update for any changes. Personally, I don't like to edit the drawing sheet and potentially remove important data.

                     

                    2) MATERIAL: $PRPSHEET:{MATERIAL}, SUITABLE FOR POWDER-COAT OR LIQUID-PAINT FINISHES.

                     

                    (7) FIT: THIS $PRPSHEET:{PART TYPE LIST} SHALL FIT FREELY WITH MATING $PRPSHEET:{MATE TO PART LIST} ( P/N:

                    $PRPSHEET:{MATING PART} ) WITHOUT BINDING OR CAUSING DEFORMATION OF ANY OF THE FABRICATIONS.