14 Replies Latest reply on Sep 10, 2015 3:27 PM by Andrew Kronquist

    Changing the name of drawing and parts

    Keith Rutter

      When I have to change the part name of a drawing and model, the views in the drawing turn into dotted line boxes. What can I do to get my drawing back?

        • Re: Changing the name of drawing and parts
          Mark Kaiser

          Open the drawing, and in the file open dialog box, I believe there is a 'references' button.  Click this and point your drawing file to the renamed part file.

           

          Or, change the names of the files using SW Explorer.

           

          Or, change the drawing file name, open the drawing, open the part file, do a save as on the part file to the new name.

           

          Or, search around here, plenty of answers here on this one.

            • Re: Changing the name of drawing and parts
              Keith Rutter

              The reference configuration drop down box is empty.

               

              The file name in SolidWorks Explorer is already changed to the current one. Is there something I am supposed to do here?

               

               

              What I did was open the part, save as, changed the name. Then opened the drawing, save as, changed the name. Then I deleted the old part and drawing. I believe I closed the part and drawing after I did each save as...

               

              Is it to late to fix my problem? And just start making a new drawing...?

                • Re: Changing the name of drawing and parts
                  Mark Kaiser

                  No need to redo anything, you need to fix your reference from the drawing to the part file.  The file name is the link of how the drawing finds the part.

                   

                  So, close everything in SW, do a file>open, you will get the dialog box below.  Click on your drawing, then click on the references button.  Choose your part file.  All should be good.

                   

                  • Re: Changing the name of drawing and parts
                    Glenn Schroeder

                    Keith Rutter:

                     

                    What I did was open the part, save as, changed the name. Then opened the drawing, save as, changed the name. Then I deleted the old part and drawing. I believe I closed the part and drawing after I did each save as...

                     

                    Next time I'd suggest opening your drawing and going to File > Pack and Go.  That's a process that will copy the open file and all it's children, either to a new folder or the same one, depending on which you choose from the dialog box.  You can double-click on the file names in the "Save to Name" column in the dialog box to assign a new name to the new files.  I believe this will work much better than the method you tried to use.

                • Re: Changing the name of drawing and parts
                  Deepak Gupta

                  You need to fix the references of the drawing OR keep your drawing open and then do a saves as on both part and drawing. You can also use SOLIDWORKS explorer to rename/fix references OR pack and go option to rename and create a copy.

                  • Re: Changing the name of drawing and parts
                    Richard Wehmeyer

                    If you rename to part or assembly file using Windows Explorer its a pain to fix, even using references.  Fastest method is to change the filename back using Windows Explorer then rename using SW explorer:

                    9-10-2015 11-28-13 AM.jpg

                      • Re: Changing the name of drawing and parts
                        Richard Wehmeyer

                        I didn't read your method til now.  Using "Save As" is just creating a copy, doesn't update the drawing (which contains the path to part file).  Both drawings were looking for the old name. 

                         

                        I think it does work to some degree if you open part and drawing at same time, then SaveAs the part, the drawing will update the path. I think I blew up an few assemblies doing this years ago but I dont know if it works for drawings.

                         

                         

                        Drawings, as far as I know, are not referenced by anything so they don't require the same care in changing their filename.

                      • Re: Changing the name of drawing and parts
                        Chris Saller

                        Whenever doing a save as, and their are assy's & drawings involved to be updated, open the dwgs and assy's first.

                        Otherwise, always rename within SW Explorer.

                        You can right-click in a view and do a replace of the part.

                        • Re: Changing the name of drawing and parts
                          Keith Rutter

                          Thank you for all the responses!

                           

                          For future reference, what is the fastest was to change the name of a part and drawing without causing any problems? I often have to change the name of  drawings, parts, and assemblies. I'm looking for the best/fastest way to get this done right the first time.

                            • Re: Changing the name of drawing and parts
                              Deepak Gupta

                              Why can't you them correct in the first place itself? If that is not the design intent then use SW explorer.

                              • Re: Changing the name of drawing and parts
                                Richard Wehmeyer

                                Depending on the circumstances involved either

                                the "SaveAs" method where everything is open and then delete the old

                                or

                                the RMB>Solidworks>Rename method if you dont need to open the files. Start at the parts, then assemblies, then drawings.

                                 

                                Caution:  I have never found a way to successfully rename parts where virtual parts are used.  You have to do something during the SaveAs to update the references but I have never figured it out fully.  Procede with caution and backups.

                                • Re: Changing the name of drawing and parts
                                  Glenn Schroeder

                                  Keith Rutter:

                                   

                                  For future reference, what is the fastest was to change the name of a part and drawing without causing any problems?

                                   

                                   

                                  You can re-name a drawing any time.  That shouldn't cause any problems.  For renaming parts or assemblies, the method I use is to right-click on the model in Windows Explorer and choose SolidWorks > Rename, as shown below.  (I believe you need to have SW Explorer installed to get this option.)  That will bring up a dialog box which will show all files referencing this model and a space for you to enter the new name.  Keep in mind that I almost always have all my files for each project in the same folder, so finding the relations isn't a problem.  If you have files scattered in multiple locations then SW might not find all the referencing files.

                                   

                                • Re: Changing the name of drawing and parts
                                  Keith Rutter

                                  Part of the problem is a lot of the parts/drawings I have are older files which were created by other people. A lot of these parts and assemblies are also configurations. Now there i'm using a new data logging software (non-SW) where the names of the parts, drawings, and assemblies may have too many characters to be entered into the data logging software. This is why I have to change the names.

                                   

                                  So I can just have the part, drawing, and assembly open while doing a save as and everything will be just fine?