21 Replies Latest reply on Jun 22, 2015 6:29 PM by Eric Porter

    Part configurations within drawings issue

    Chris Stanley

      Hi,

       

      I'm having issues with parts with configurations within drawings.  My part file is driven by a design table in which I use both numerical and text custom properties to control the model.  My issue is that model does not update within the drawing views when specifying configurations within the drawing.  The configurations do update the custom property information such as the $PRPSHEET info I've enbedded into my template, but the onscreen model does not update.  It's stays in the last saved configuration of the part.  I know there is option in the properties of the drawing view for "Configuration Information" that says "Use model's "in-use" or last saved configuration" or "Use named configuration".  I'm using the latter.  I've had this issue with SolidWorks 2012 and 2013.  These are the only versions I've used so I'm not sure if this happens in all versions.  The part also has all the configurations rebuilt before saving.  Also, since the model doesn't update, the dimensions do not change.

       

      I'm trying to create individual drawings for every configuration without having multiple part files.  Thanks for any help you can give me!

        • Re: Part configurations within drawings issue
          Glenn Schroeder

          Chris,

           

          Welcome to the forum.  I have a couple of questions.  When you RMB on the drawing view and choose "Properties", does the dialog box show the correct configuration?  If it does, then changes to the model should be reflected in the drawing view.  Have you tried a Ctrl+Q rebuild after editing the model?

            • Re: Part configurations within drawings issue
              Chris Stanley

              Thanks Glenn,

               

              The dialog shows the configuration I have selected and when I change the config to another and click ok, the model does not update but the text property information that fills my drawing does update.

               

              Regarding the Ctrl-Q command, I never have used that before but I did just try it out.  Within the part file, it does rebuild the model to the specified configuration.  If I have the drawing file open at the same time, the model updates to whatever configuration I rebuilt in the part file.

               

              From what I'm seeing, no matter what is specified within the drawing, the model displayed is the current or last saved configuration of the part.

            • Re: Part configurations within drawings issue
              M. B.

              I have this problem often in SW 2011.  Very scary when a design is complete and all you want to do is print drawings for manufacture but are not confident the view configuration and associated dimensions display the way you want.

               

              Here's what I do. With only the part file open, manually create a new configuration with a unique name that has never been used.  I always use gibberish for a name.  Delete every other configuration, file the part, and for good measure completely exit SW.

               

              Reopen SW and open the part file. Open the design table and update external links if necessary.  Exit the design table to recreate all new configurations.  Delete the gibberish configuration.  Use a macro (I got one here) to open, rebuild, and update every configuration then save the part file.

               

              Now open the drawing.  Every view with different configurations should display the correct configuration and correct dimensions.

               

              This has always worked for me with the caveat that SW adds multiple display states that I don't want and have to delete.  These new additional display states can degrade performance and add size if you don't constantly delete them.

               

              p.s. I would like a better macro to open and update configurations if anyone has a suggestion

                • Re: Part configurations within drawings issue
                  Chris Stanley

                  Thanks M. B, I'll try this.  I believe SW has the rebuild configurations built-in now in SW2013.

                   

                  Just a quick question regarding deleting configs.  I have nearly 70 configs in this file, is there a quick way to select them and delete.

                    • Re: Part configurations within drawings issue
                      M. B.

                      Shift LMB will highlight as many names as you want.  A pop-up will tell you that it can't delete the active config. and I just clik OK.  Be sure that every config. you want to recreate is defined in the design table otherwise you will have to recreate it manually which could be a lot of work.  I have dozens of part files with over 200 configurations and have had to recreate those configs multiple times.  This is how I learned the hard way that additional display states are created every time you recreate a config.  With 200+ configs. constantly changing and being recreated, display states cause me endless grief.

                        • Re: Part configurations within drawings issue
                          Chris Stanley

                          Could you point me to the macro that you used?

                           

                          On a side note, I used one of my recent part files that I haven't attempted making drawings of yet and the configurations loaded in the drawing perfectly.  I was for the longest time thinking that this wasn't possible at all.

                            • Re: Part configurations within drawings issue
                              M. B.

                              Here is the macro I use the most.  I downloaded it from this forum but have no idea who to give credit to.  Can't remember but I might have renamed it from its' original name.  With your 70 configurations you might want to plan on doing something else while it runs or take a long lunch break depending on how complex your model is.

                              • Re: Part configurations within drawings issue
                                M. B.

                                Chris, I have also had to work around this problem in SW2011 by creating a new drawing with new views to get the configuration and dimensions to display correctly when the older previous drawing wouldn't.  If SW could find a way to fix these types of problems without screwing up something else I would purchase upgrades more often. I'd be very interested in finding out if the SW2013 config. updater/rebuilder actually works like we users think it should.

                                  • Re: Part configurations within drawings issue
                                    Chris Stanley

                                    We'll see how this turns out.  I've went through the process of remaking the configs for an excel file and I rebuilt a few of them manually.  I tried a new drawing and the model was still not updating.  I'm in the process of running the macro now.

                                     

                                    I need to do a little research on display states I believe.  For some reason the model had link the display state to the configuration enabled.  I disabled that so I'll see if that helps.

                                    • Re: Part configurations within drawings issue
                                      Chris Stanley

                                      The marco froze up in the middle of running...possibly just one of the models taking a while to solve and I just ended it.

                                       

                                      Regardless, I used the Ctrl-Q command on a few configs and created a new drawing.  The models still wouldn't update within the drawing.  Something within this file is wrong.

                            • Re: Part configurations within drawings issue
                              Jerry Steiger

                              Chris and M.,

                               

                              Have you sent these files to your VAR? If not, I strongly suggest that you do so. This is core functionality that needs to work. SolidWorks needs to see a bug to fix it. Rub their noses in it!

                               

                              Jerry S.

                              • Re: Part configurations within drawings issue
                                Mohammad Darabseh

                                you may need to rebuild the model (in sheet metal you need alsos to flatten/unflatten the part)  all configuration, try use a macro that will rebuild and flat/unflat part at all configuration before going to drawing.

                                also make sure that new created configurations in your design table will not chave new names.

                                 

                                as an alternative:

                                sometimes after finishing design table and before sending to manufacturing, we use macro that will save all configurations as separate files and then we use another macro to make the drawings for these parts, I know it is a longer solution but garanteed.

                                • Re: Part configurations within drawings issue
                                  Chris Stanley

                                  I have an update.  I sent the file to my VAR which got together with SW.  They confirmed it was a bug and they were able to recreate it.  I await the fix so I'll post agian when I know what comes of it.

                                    • Re: Part configurations within drawings issue
                                      Eric Porter

                                      So I just figured this out in an assembly I have. 

                                       

                                      -The assembly has two base sketches with dimensions linked to different configurations. One sketch for height, one for width.

                                      -There are two parts. One part changes with the two sketch dimensions, ex: 12x18, 16x20.

                                       

                                      I created a drawing where each page is the assembly in a different size configuration, ex: 12x18, 16x20.  I also had the problem where all the pages would be the last "in-use" model, instead of updating to the proper configuration sizes. 

                                       

                                      The solution came from SW 2013 help.  I needed to create multiple configurations for the part that changed size, and then have the part be in different configs for each assembly config.  Ex: In the 12x18 Assy config, the part is in the 12x18 Part config.

                                       

                                      Now all the pages update fine.

                                       

                                      Ahhh...SolidWorks...

                                       

                                      2013 SOLIDWORKS Help - Best Practice for Configurations with External References

                                       

                                      "

                                      If a part contains external references from a multi-configuration assembly, best practice is to have a corresponding part configuration for each assembly configuration.

                                      A warning appears when you save an assembly if external references from multiple configurations in the assembly influence the definition of a single configuration of a part. Having such a multiple-to-one (n:1) relationship is not recommended. Only the most recently updated assembly configuration will be up to date. The other assembly configurations will be out of date, and therefore will take time to rebuild when you activate them. Also, the different versions of the part's single configuration do not have unique identifiers, which could result in the wrong version being manufactured or purchased.

                                      Best practice is to have a one-to-one (1:1) relationship between configurations of the assembly and the configurations of the part."