23 Replies Latest reply on Sep 13, 2017 8:54 AM by David Matula

    Drawing Views-Problem with updating

    Liam Connelly


      I am experiecing a problem when updating drawing views on Solidworks 2011.

      Occasionally, a drawing view will not update properly after a model has been changed. The drawing view will behave in a strange way, showing a combination of the old model (prior to changes), and the new model (after changes). The old model is visible in black lines, while the new model appears as a kind of trace, which can be clicked on and dimensioned, but is invisible.


      The image below shows an example of a drawing view that is having this problem. Note:
      - The new model is shown by the highlight-blue lines and dimensions. It is interactive but invisible.

      - The old model is shown by the black lines. It is visible, but not interactive.


      I think this problem may be related to "updating views". I want to find a solution that will force all the drawing views to update, and override this problem. So that all the drawing views show only the new model, both visible and interactive, like normal.


      Any help would be greatly appreciated!




      1. This problem only happens occasionally, and it appears to be qutie random. i.e I can't find any connection to specific files/features/actions. So far none of my collegues have had the same problem, which has lead me to wonder whether it is a glitch?

      2. I have found several solutions which will force the drawing view to update itself back to normal. The problem is that all these solutions require me recognising the problem myself, looking at the drawing sheet and spotting the error. This can be time consuming and difficult to check with small changes. I want to find a solution that will force all drawing views to update accurately.


      The solutions I have found are:


      - making further changes to the model (making more changes will usually make the drawing view update like normal)

      - changing the view orientation

      - hiding the part, and then showing it again


      3. I have tried the following actions which had no effect:


      - Pressing Ctrl+B / Ctrl+Q, / pressing the rebuild icon or menu tab.

      - turning off automatic updates and rebuilding

      - opening the part, then returning to the drawing

      - closing the drawing and model, then opening it again

      - closing solidworks and opening it again (also computer)


      4. The part shown in the drawing (and the one that I am currently experiencing the problem with), has one configuration and is a basic extrude.

        • Re: Drawing Views-Problem with updating
          Glenn Schroeder



          Welcome to the forum.  I haven't seen this behavior, and I don't remember seeing anyone else mention it here.  You mentioned several things that don't work.   I have one more suggestion when it happens.  Have you tried switching to a different display style, such as Shaded with Lines, or Hidden Lines Removed, and then switching back?


          Also, have you reported this to your VAR?  They might be able to help, or they can report the behavior to SW if they can't.

          • Re: Drawing Views-Problem with updating
            Mark Kaiser

            Have you tried the same part/drawing file on another co-workers pc?  Would isolate whether its the cad file itself or something with your pc.

            • Re: Drawing Views-Problem with updating
              Tom Simmonds



              We had the same problem.  We had this issue going back as far as 4-5 years.  It was always random.  The drawing could be fixed by switching to shaded view and then back.  Once this switch was made, the drawing stayed fixed forever.  My VAR could not figure it out.


              When the drawing was not showing up correctly, if a DXF was made, it had the wrong geometry.  I can't begin to add up all of the bad parts we had made.


              It would come and go at random.  It would happen a lot, then we would go months without seeing it.  Then it would start again.  It happened over many different releases of Solidworks and service packs.  At first I don't think my VAR believed me.  Then I sent them a file that they could repeat the problem on.


              The best they could do was give us a macro that woud open and switch views to shaded and back then close.  You had to tell it what folder to do this on. 


              The frustrating part was the randomness of it.  And the months between incidents.  It wouldn't happen, and people would get lax about running the macro.  Then it would rear up again and we would get parts that were cut wrong from our laser cutting vendor.


              VAR said the macro could be set to run on our complete part inventory, but it never worked that way.  We have a very large database of drawings and we are an engineer to order company.  Everthing is custom, usually one of a kind.  We have a system to identify similar parts, and we frequently copy and rename assemblies.


              It has now been well over a year since we have seen the issue.  Hopefully it is gone.

                • Re: Drawing Views-Problem with updating
                  Alex Lachance



                  I've been experiencing the same problems ever since I started using SolidWorks at work. We've been on SolidWorks since 2012 and as mentioned, it seems to come and go at random times.


                  I've had 2012 from SP2.0 to SP5.0, 2014 from SP2.0 to SP5.0 and currently running SolidWorks 2016 SP4.0.


                  I still have the problem, sure it isn't often but it is still quite irritating to have a part that is 76'' x 96'' have to be thrown to scrap because the program decided to do a bug every month.


                  From what we've gathered so far, the bug seems to happen on a very specific action. Once the bug is caused. it is active and will cause every drawing opened and saved to be bugged afterwards. There is no specific pattern that I can recognize that would give me a lead to find what causes it.


                  I have contacted my VAR about this before. I was basically told ''Yeah, it's a known bug, so?''. That was a while ago and I haven't contacted them again since. The reason I haven't is because I know the answer I'll get. I need to be able to locate the problem and the cause of it before contacting them or else it's pretty useless.


                  Off subject, while I'm at it, has anyone ever had a bug fixed within the version they are working on or is everyone getting the same answer as me? Whenever I get a confirmation that a bug will be fixed, the answer is usually along the line of ''Will be fixed in the next version of SolidWorks''. It is quite irritating to be told every year to buy the next year's version to fix the current year's bug when you already know the new version will have bugs caused by all the new flashy stuff they put in the program.

                • Re: Drawing Views-Problem with updating
                  Doug Kuhn



                  I have experience the same issue.  There are a few fixes you can make.  this is just a bug in 2011 and because you cannot repeat it, good luck getting it fixed.  The main thing is that you can fix the issue.  If you go into the part, roll the part back one step in your feature tree, then roll it back to the end.  it will fix that issue forever on that drawing.

                  the other fix is to upgrade to 2012...i have not seen it in 2012.

                  change the view layout (not the best option as it tends to get rid of your dimensions).



                  good luck

                  • Re: Drawing Views-Problem with updating
                    Liam Connelly

                    Thanks a lot for your help everyone.


                    It is a good start to at least confirm it is a bug and not a feature that I wasn't understanding properly.


                    The problem does seem to be random, and I don't have any files to test soultions on right now unfortunately (I had to save over the example one), but it sounds like it should be ok as long as I play with the model a bit before exporting my drawings. Changing to shaded view and back again, and rolling back the parts as well.

                    Long term, it sounds like changing to 2012 would be the only solid fix.



                    Glenn, I haven't reported it to our VAR yet, as I thought it might have been a feature. I will speak to them if it comes up again.


                    Fredrik, I also haven't looked into the video card, but I may do if it keeps happening.


                    Mark, I haven't tried opening the same part/drawings on co-workers PCs yet, but that would be interesting to know, as they could be having the same problem without realising it. It could go unoticed for quite a while, unless the part was getting cut.


                    Tom, that is very helpful to know, as I am also converting the drawings to DXF files for cutting, and have also cut parts incorrectly, which is why I want to get the issue fixed.


                    Doug, I will try rolling back the part along with changing to shaded views. I agree that changing the view layout is definitely not desirable for how we are using it.


                    Thanks again for all your help. Hopefully that will deal with the problem and I wont have to write again!

                      • Re: Drawing Views-Problem with updating
                        Aaron Forbes

                        I wonder if this problem happens in 2012 even?  I feel comfortable with 2011 mostly and you won't catch me using 2012 until 2013 sp2 is out. I absolutely disliked 2010 and since then I have been leary on upgrading. The only year I haven't had problems was 2007 and 2008, but back then I wasn't intensely as involved as I am now.


                        I have this problem too, and I swear one day SolidWorks is gonna get me fired, because we will burn $5000 of material and all the flat patterns were wrong over some random bug like this. Its hard for management to understand when SolidWorks users are outnumbered by AutoCAD users.

                      • Re: Drawing Views-Problem with updating
                        Tom Simmonds

                        We just had the issue appear again.  We are using Solidworks 2012 SP4.

                        • Re: Drawing Views-Problem with updating
                          Bjorn Gunderson

                          I see this is an old topic, but I thought I should report that I've experienced this issue recently with SW 2013 SP4.  The shaded display trick worked, so thank you for that.  But it doesn't seem to be just a bug with the 2011 version.

                          • Re: Drawing Views-Problem with updating
                            Dennis Beeren

                            Setting the 'Verification on rebuild' did not solve the problem. It appears to be an issue originating from old templates. Issue is solved from Solidworks 2016. We tested this and indeed in SW the drawings open with the right geometry. Since we are still on SW2014 we received a macro from our VAR which updates all drawing views. We execute this macro on every drawing that is passing our image server. After I figured out how I will post this macro here.

                            • Re: Drawing Views-Problem with updating
                              Dennis Beeren

                              I can't find a way to upload the macro