11 Replies Latest reply on May 31, 2018 12:11 PM by Chase Nichole

    LINK DRAWING TO DIFFERENT MODEL

    David Guza

      Can anyone help on this?

      I have a model of a small enclosure box with NPT holes.  I have generated a detailed drawing of this part and saved both with a part number as the file name.  I need to modify the holes with a different threaded hole call-out and save this under a different part number as the file name.  In other words, I need two separate models and sets of drawings.  I did a "save-as copy" for the model and renamed it to the new part number - good so far.  Is there now a way to save the work already done on the first drawing and save with the second file and part number as a separate drawing file with references only associated only with the new part?  Would doing a "save-as copy" for the drawing using the same file name as the new part work and establish the correct references leaving me with two separate models and two separately and respectively referenced drawings?  The changes are minor so if this is possible, it would save a bit of time needed to regenerate a new drawing.

      Thanks!

        • Re: LINK DRAWING TO DIFFERENT MODEL
          Prasad Bhonsule

          Hi David, what you can do is:

           

          1. Open the original drawing and do a Save as copy

          2. Close the original drawing, and click File, Open in SolidWorks

          3. In the Open dialog, click on the copy yousaved in Step 1, but DO NOT open it yet

          4. Click the references button (see below0

           

           

          5. In the references window, double click the current file and browse for the new part.

           

          Now the copy of the drawing should reference the copy of the part with the new holes etc. You may have a bit of cleanup work to do, but should be OK.

           

          Hope this helps.

           

          Kind regards,

           

          Prasad Bhonsule

          • Re: LINK DRAWING TO DIFFERENT MODEL
            Matthew Menard

            You might also want to try the pack and go command. 

            You can make a copy and rename all of the files you want in one shot with this tool.  Like most things in Solidworks, there are a number of ways to get the job done.

            • Re: LINK DRAWING TO DIFFERENT MODEL
              Wojciech Paterski

              or you can open original drawing and right clik on the view (the first view u created - master view ) and right click then choose 'replace model' go to browse and point to the new file.

              • Re: LINK DRAWING TO DIFFERENT MODEL
                Jan Forkovic

                Hi,

                in Pack and Go check "include drawings" an rename the drawing too.

                • Re: LINK DRAWING TO DIFFERENT MODEL
                  Sarah Dwight

                  We do this everyday for our same-but-slightly-different parts by:

                  Opening the drawing

                  Opening the part from the drawing (RMB a view and open part)

                  Save As the part as a new part name and choose Save As to keep references in drawing

                  Save As the drawing as the new part name and then do any changes to part/drawing.

                  This will keep the original files untouched and references intact.

                    • Re: LINK DRAWING TO DIFFERENT MODEL
                      Matthew Menard

                      I do the same thing as well when I only need a single new drawing and part derived from an old one.  However, I will usually "save as" the drawing to a new file, then open the old part from the new file and then "save as" the part to a new name from there.  The only reason I say this is because I have done it the opposite way before and saved the new part into the old drawing when I gotten distracted mid way through.  It's not the end of the world, because you can go back and change the references back to the way they should be the way Prasad illustrated above.  Neither way is wrong, but I would argue that saving the part before the drawing leaves you a "save" instead of a "save as" away from a few extra mouse clicks to fix a reference.

                        • Re: LINK DRAWING TO DIFFERENT MODEL
                          Mark Dougall

                          I know this is an old thread but I have just done this procedure and all references are changing EXCEPT the $PRPSHHET:"Description" field. No matter what I do or Change the drawing still wants to reference the old description even though the drawing Shows the new part and when I open part from drawing it opens the new Named part and the new part has the new description etc. I can't find where the drawing would be referencing the the old description from.

                           

                          EDIT: I have now gone as far as to delete the original file and the old description is STILL being referenced. When I go into the drawing properties it Shows the old description and if I try to Change it, it reverts back to the old as if it were referencing the part which is deleted. Once again the new part has the new description changed in ist propeties menu.

                           

                          EDIT EDIT: Ignore this. Solved it. It was a Description property from EPDM I had to Change to have the description reference.

                      • Re: LINK DRAWING TO DIFFERENT MODEL
                        David Guza

                        It is wonderful that knowledgeable folks like you are kind enough to help!  I hope to return the favor sometime if able.  That should close this discussion. Thanks everyone!

                        • Re: LINK DRAWING TO DIFFERENT MODEL
                          Chase Nichole

                          To create a duplicate part with a new number and bring in the drawing with references intact for both files:

                          Option 1

                          1. Save as Copy the original drawing file with a new part number.
                          2. Close the original drawing file.
                          3. Open the part from either the new drawing, or open the original part and Save As with the new part number.  If you are working with a part or assembly that is referenced by higher level assemblies, it is good practice to open those assemblies before you "Save As" the new part with a new part number so that the higher level assembly references update automatically.  If your new duplicate part is one of many instances in a higher level assembly and you need both the new part and the old in those assemblies, use the "Make Independent" feature (see the note 1 below to create a duplicate drawing that references the new part).
                          4. Update any manually controlled custom properties in the new part/drawing that may reference the old part (e.g. description, configuration specific part numbers, etc.).
                          5. Make the desired changes to the new part and update the drawing as needed.

                           

                          Note 1: steps 1-5 assume you have had the foresight to create the duplicate part before making changes to the original.  If you find yourself in the position where you have modified an existing part and now require a new number along with an up to date drawing that shows those changes (as much as is possible):

                          1. With the drawing closed and the modified part open, save the modified part as a copy with a new number.
                          2. Open the original drawing.
                          3. RMC the first view you created (in an assembly with a BOM, RMC the view the BOM references) and choose Replace Model to update the drawing reference to the new modified part.
                          4. Update your drawing as needed.

                           

                          Note 2: if you are working with a duplicated assembly created from the steps above, use the "Replace Component" feature wherever possible to keep your drawing up to date as you modify the assembly moving forward.  This is especially important with large assemblies that use customized display states, configurations, advanced drawing views, etc.