35 Replies Latest reply on May 1, 2018 9:02 AM by Alex Lachance

    Empty view shells in drawing?

    Alex Lachance

      Hello,


      I've had this bug for the past 5 years and have been trying to figure out what causes it and how to fix it and I haven't found anything. I recently found out that this bug was the cause of many other major bugs we had in our company.

       

      I am currently running on Windows 7 (French version, it does matter from another bug I've had before).

      I use an AMD FirePro V7900 as a graphic card

      18GB of ram

      Intel i7 @ 3.60GhZ

      SolidWorks 2017 SP 4.0

      I also use a third party program to generate my properties called CustomTools. As far as I'm aware I've had the bug both with and without this add-on so I've ruled it out of the equation.

       

       

      Here is my situation, hold on tight as it may take a while to read the explanation.

       

      When I make a new drawing, there is almost always empty view shells floating around. I do not know where they come from because my templates are empty. Those view shells generally represent every view available in SolidWorks, including Annotation views. In order for them to ''show'', I have to use the ''View>Show/Hide>Show hidden views'' which, by the way, doesn't work correctly. It doesn't show the hidden views when I use it unless I change sheet or save. When that trick doesn't work, I end up clicking around in the drawing for about 15 minutes until I can locate them as a blind man would. When they hidden views do show up, like the screenshot below, there is no way to make them show a model, they will always remain a big red X.

       

      Here is where it gets tricky. Those view shells are not shown in the feature tree. Not only that, they are not linked to a sheet, they are linked to the drawing itself. What I mean by that is that the views show up on every sheet until you erase it from one sheet. When the views are all erased from the sheet, they never show up again on any sheet whatsoever.

       

      Those views seem to be linked to the drawing but I haven't found a way to get them to show a model...

       

      I usually have between 8 and 14 empty shell views floating around, I was hoping I could find either what causes it or a solution to it or even both.

       

      Here is a screenshot to show you what I mean, I have also uploaded a .sldprt along with a .slddrw for you guys to see it. There is 9 empty shells on that drawing

       

       

       

      Hopefully I'm not the first to get this bug and some of you can help me out with this.

        • Re: Empty view shells in drawing?
          Jim Sculley

          Interesting.  My first thought is that you are suffering from Crusty Old Template File Gotcha syndrome.

           

          Some observations:

           

          If you hover over one of the 'hidden' views you can right click and select 'Show' and it will appear, briefly.  As soon as you rebuild, pan, zoom, etc. it disappears.

           

          You can cut and paste the 'hidden' views to another drawing and the bad behavior remains.

           

          You can project views from the hidden view and they behave correctly.

           

          If 'Lock view focus' and add some notes, it will crash eventually.  At least it did for me.

           

          More observations:

           

          Initially, Hide/Show...Hidden Views would not show anything for me, not even the orange boxes with X's.  If I open the Tools....Options dialog and click OK, the boxes would appear.  Rebuild, they disappear.  Delete one, the others disappear, but aren't deleted.  When they disappear, they can be brought back by toggling Hide/Show Hidden Views and going to Tools....Options...OK again.

           

          Programmatically, the views don't exist.  Using a macro to list all views, they are not listed.

           

          I deleted everything from the drawing including the sheet format and saved it as a new template.  I created a model of a 1"x1"x1" cube using my part template.  I made a drawing using the 'bad' template and the 'ghost' views were created.

           

           

          There is one view for each view in the view palette:

           

          They appear in reverse order, from left to right, except that Current appears before Iso/Di/Tri Metric.

           

          If you turn off this option:

           

          in the 'Drawings' category of System Options and make a new drawing using 'Make Drawing from Part', the 'ghost' views are not created.  However, as soon as you load the model in the View Palette, the ghost views will be created.

            • Re: Empty view shells in drawing?
              Alex Lachance

              Hi Jim,

               

              First of all, thanks for the response. That is an extremely interesting read and the observations you have noted are also interesting. I did not quite understand what I had to do in order to update my existing assemblies and parts template. I'd like to point out my SolidWorks is SolidWorks 2016 SP4.0 and not 2017 as mentioned above, my mistake.

               

              As in the article, I have looked up one of my assembly, and it is in fact outdated.

               

              As far as my templates goes, I have went and saved them all one by one everytime I have upgraded my SolidWorks so they are supposed to be saved into the correct version, unless there is something I don't understand.

                • Re: Empty view shells in drawing?
                  Jim Sculley

                  I may have misspoken about the bad behavior persisting after cut and paste.  This morning I cut a view from the bad drawing and pasted it into a new drawing.  I was then able to right click and 'Show' the view and it appears to be working correctly. Nope.  Still broken.  A second attempt and the view disappears.

                   

                  Saving your old templates in the new version does not update them.  You actually have to recreate your templates from scratch, starting with the default SOLIDWORKS generated templates.  If you check in the folder C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20xx, the default generated templates may be there.  If they aren't there, remove all folders from File Locations...Document Templates in the system options and reset the Default Templates in system options to the default.  Now when you create a new part, the three default templates will be created by SOLIDWORKS and you can use those as your starting point.

                • Re: Empty view shells in drawing?
                  Alex Lachance

                  Thanks Jim for your extensive analysis of the problem. I am not a programmer my self, I can read codes and correct them if the errors are minor but I have no formation in order to do so, it is all self taught.

                   

                  I've had the problem since we switched to SolidWorks and our templates were made from scratch back when we did the switch, so I think the templates might not be the problem but then again I am not entirely sure.

                    • Re: Empty view shells in drawing?
                      John Stoltzfus

                      Alex Lachance  Re-doing your templates isn't that hard...  What I did was have two sessions of SW open.  First thing I did is to draw a 8.5" x 11" sketch and place the one corner 0,0 and fixed the sketch, then in the second screen and the other session I just copied the entire title block and pasted off of the new sheet, (don't let the pasted sketch overlap into the new template,  then I highlighted the just pasted sketch and ctrl and picked the 0,0 corner of the pasted sketch and dropped it onto the newly fixed sketch and done.  Close the original template and save over the old template with the new... Takes a few minutes per sheet...

                        • Re: Empty view shells in drawing?
                          Alex Lachance

                          It is not a matter of being hard or not, it is a matter that it shouldn't even have to be done in the first place. If we follow SolidWork's logic and update each year, this is a process we have to do over and over again. Could you imagine having to restart your whole computer everytime you have to open a new drawing? This is pretty much the same thing, to a different extent.

                           

                          Your solution does fix the templates, but what about all my existing drawings? How do I fix those? We have around 25 000 components, over 150 different models of large assemblies of trailers, there is no way I'm going through the hassle of redrawing everything every year.

                           

                          I've found that deleting the problematic views does fix the problem for existing drawings, but what tells me that it won't occur again, that this bug isn't caused by more than just one thing?

                           

                          There should be a solution for this problem and it shouldn't have to come from my side or any of ours. This is a SolidWorks problem, it needs to be adressed by SolidWorks. I can't believe there are support techs from SolidWorks on these forums and that they skip over such important problems...

                        • Re: Empty view shells in drawing?
                          Deepak Gupta

                          For a test, create new templates without any details in it and using them can help you find if this is setting issue, software issue or templates.

                      • Re: Empty view shells in drawing?
                        John Stoltzfus

                        Can't you right click and show??

                        • Re: Empty view shells in drawing?
                          Alex Lachance

                          Hello everyone,

                           

                          I have forwarded this to my VAR last friday and they have forwarded it to SolidWorks. When SolidWorks responds, I'll post what they mention, if I get a SPR opened I will also post the SPR number.

                           

                          Regards

                          • Re: Empty view shells in drawing?
                            Sarah Dwight

                            Once in a blue moon I get a drawing that does this. Generally they are old drawings I am updating.

                             

                            Until now I hadn't seen the extra views highlighted like that!!

                             

                            I would hit "F" to fit to screen and get a zoomed out focus on my viewport. Then I would wave my cursor over the empty space on the far left until my cursor changed to indicate there was something there, then I would click on and delete the view. "F" to fit screen and start over until I have a normal focus on the page. I couldn't box-select or ctrl-select them or do anything to get them to be visible.

                              • Re: Empty view shells in drawing?
                                Alex Lachance

                                Hey Sarah,

                                 

                                Quick tip I found while removing those views. After doing the ''Show hidden views'' thing, switch page. If you don't have 2 pages in your document, create one before doing the ''Show hidden views''.

                                 

                                When you'll switch page, you'll be able to see all the views with the orange x's on them. I was pretty much doing the same thing as you up to last week when I noticed that it would sometimes show when I saved a document with multiple pages. Figured there was something there and eventually got that little trick to easen up the hassle of finding them.

                              • Re: Empty view shells in drawing?
                                Alex Lachance

                                Hello all,

                                 

                                Still haven't gotten a real SPR opened, but I did get feedback from my VAR who got feedback from SolidWorks.

                                 

                                Apparently, it is the first time SolidWorks hears of this problem, they are still investigating.

                                • Re: Empty view shells in drawing?
                                  Alex Lachance

                                  Hello everybody,

                                   

                                  Finally got a SPR opened.

                                   

                                  SPR #469002

                                    Titre: Hidden empty views are appearing outside drawing sheet format after created drawing view

                                   

                                  Send this to your VAR to get this issue fixed ASAP

                                  • Re: Empty view shells in drawing?
                                    Alex Lachance

                                    Response from SolidWorks:

                                    The SPR 469002 became ‘Inactive’ because of no customer hits for long period. Since we have added the customer to the notification list, the SPR becomes ‘Open’.

                                    Longer time to export drawing as DWG

                                    I observed that these views are not exported in DWG file. Further, I did not observe much time difference when I exported drawing ‘ATTE-025.SLDDRW’ with/without those hidden views.

                                    Does customer have drawings showing this issue? Please provide sample file showing the problem.

                                     

                                    After receiving that response, I sent them a multiple bodies part along with the 20+ page drawing. That should make them notice the difference.

                                    • Re: Empty view shells in drawing?
                                      Alex Lachance

                                      Re-reading this thread got me wondering, why is it almost unthinkable in SolidWorks to keep working through different versions of the program with the same file while it has never been a problem for AutoCAD? The intention is not to stir this into a AutoCAD vs SolidWorks debate BTW.

                                      • Re: Empty view shells in drawing?
                                        Alex Lachance

                                        I just found out today that the ''View Palette' tab is the one that keeps on recreating these faulty view shells. Will forward this to my VAR when I get the time.

                                         

                                        I hope someone from SolidWorks reads this.

                                         

                                        Edit : Re-reading myself, I realize it might not have been clear what I meant. When you use the View palette tab and refresh it, SolidWorks regenerates the faulty views in the drawing.

                                        • Re: Empty view shells in drawing?
                                          Alex Lachance

                                          Hey everyone,

                                           

                                          I'm back home. Finally freed up some time so I sent this to my VAR. Will tell you guys what I hear back from them.

                                           

                                          Edit: They added the info to the current SPR.