42 Replies Latest reply on Dec 18, 2017 8:19 AM by Alex Lachance

    Drawing Views-Problem with updating

    Liam Connelly

      Overview

      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!

       

       

      Detail

      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

          Liam,

           

          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

              Liam,

               

              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

                  Hello,

                   

                  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

                  Liam,

                   

                  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

                              • Re: Drawing Views-Problem with updating
                                Alex Lachance

                                @Jim Wilkinson ,

                                 

                                Can you help us out here? I've had this problem since 2012 throughout 2016 SP4. The bug itself has cost us in the 5 digits over a 5 year span.

                                 

                                Here are 2 parts that I've put aside that have the bug present. Just so you know, both have been saved into the correct state. You can tell by opening them in preview or looking at the preview in windows. Upon opening them, the view bugs out and shows the part I started from.

                                 

                                 

                                  • Re: Drawing Views-Problem with updating
                                    Jim Wilkinson

                                    Alex Lachance wrote:

                                     

                                    @Jim Wilkinson ,

                                     

                                    Can you help us out here? I've had this problem since 2012 throughout 2016 SP4. The bug itself has cost us in the 5 digits over a 5 year span.

                                     

                                    Here are 2 parts that I've put aside that have the bug present. Just so you know, both have been saved into the correct state. You can tell by opening them in preview or looking at the preview in windows. Upon opening them, the view bugs out and shows the part I started from.

                                     

                                    Hi Alex,

                                     

                                    I'm doing some testing on them and I've found an interesting thing that I'd like you to double check.

                                    For the MURS-337.SLDDRW file, I find that if I open the file into SOLIDWORKS 2016 (or later), using File, Open or drag and drop it the SOLIDWORKS window, it exhibits the bad behavior. If I double click the file to open it from Windows Explorer, then it doesn't exhibit the behavior. Can you confirm?

                                     

                                    FYI, ACCE-403.SLDDRW doesn't exhibit this same behavior in SW2016; it seems to always open in the bad state no mater what method I use to open it.

                                     

                                    Please let me know if you find the same and I'll continue to investigate.

                                     

                                    Thanks,

                                    Jim

                                      • Re: Drawing Views-Problem with updating
                                        Alex Lachance

                                        Hey Jim,

                                         

                                        They seem to behave the same way, no matter how I open it, though I do remember some instances in the past where I wasn't able to get it to display the bug while showing it to my VAR(I think). The drawing hasn't changed since so it's really something specific. As stated before, once the bug occurs, it corrupts every part drawing opened until you restart SolidWorks.

                                         

                                         

                                        Edit: As the OP stated, the bug comes and goes. We can be 3 months without seeing and hearing from it and then 3 months straight of getting this bug on every project. I will try and isolate as many part files as possible to send them to you guys, my boss might not lynch me if we get this fixed

                                          • Re: Drawing Views-Problem with updating
                                            Jim Wilkinson

                                            Alex Lachance wrote:

                                             

                                            Hey Jim,

                                             

                                            They seem to behave the same way, no matter how I open it, though I do remember some instances in the past where I wasn't able to get it to display the bug while showing it to my VAR(I think). The drawing hasn't changed since so it's really something specific. As stated before, once the bug occurs, it corrupts every part drawing opened until you restart SolidWorks.

                                            Hi Alex,

                                             

                                            Sorry about that, but I had the files reversed. Please try opening ACCE-403.SLDDRW by double clicking it from File Explorer. For me, if I do that, no matter what has been opened previously in SOLIDWORKS, it opens fine. If I open it through other open methods it then exhibits the problem. Please confirm if that works OK for you.

                                             

                                            In SW2016, MURS-337.SLDDRW always opens in the bad state independent of what method I use to open it.

                                             

                                            Can you please test ACCE-403.SLDDRW by double click and confirm that is the same behavior for you?

                                             

                                            Thanks,

                                            Jim

                                              • Re: Drawing Views-Problem with updating
                                                Alex Lachance

                                                Double clicking it from my Windows Explorer window does the same thing as dragging it. Are you speaking of SolidWorks Explorer?

                                                 

                                                Just tried it with SolidWorks Explorer and still get the bug by double clicking in it too.

                                                  • Re: Drawing Views-Problem with updating
                                                    Jim Wilkinson

                                                    Alex Lachance wrote:

                                                     

                                                    Double clicking it from my Windows Explorer window does the same thing as dragging it. Are you speaking of SolidWorks Explorer?

                                                     

                                                    Just tried it with SolidWorks Explorer and still get the bug by double clicking in it too.

                                                    OK...Interesting. So what I have found so far on my machine is:

                                                    ACCE-403.SLDDRW is saved in SW2014 format. If I open it by any method in SW2014, it exhibits the problem. If I open it by double click from Windows Explorer in SW2015-2018, it does not exhibit the problem (but does exhibit the problem by opening it through File, Open or drag and drop).

                                                     

                                                    MURS-337.SLDDRW is saved in SW2016 format. If I open it by any method in SW2016, it exhibits the problem. If I open it by double click from Windows Explorer in SW2017-2018, it does not exhibit the problem (but does exhibit the problem by opening it through File, Open or drag and drop).

                                                     

                                                    So, for me, files with the problem consistently open in the bad state in the version in which they were last saved. But, opening them by double click DOES NOT exhibit the bad behavior if the file is converting to a newer version on open.

                                                     

                                                    It's strange that this is not the same behavior you are seeing for ACCE-403.SLDDRW.

                                                     

                                                    By the way, if I open the MURS-337.SLDDRW file and it is in a bad state and I then open ACCE-403.SLDDRW through double click, ACCE-403.SLDDRW is NOT in a bad state. So having a file in a bad state open in SOLIDWORKS does not make all other drawing files opened in the session also open in a bad state (at least not for me). Perhaps your previous statement to that effect relates more to if the problem initially occurs to a drawing in a session, then any drawing opened after that in the session will exhibit the problem. However, unfortunately, having the files in the bad state does not tell us how they got into this state. But hopefully the files in the bad state can give our developers some clue of what to look for or be able to detect they are a in a bad state and make it so rebuild or something else will fix them.

                                                     

                                                    I'll continue looking at this to see what might be going on.


                                                    Has anyone on this thread received an SPR from there reseller for any of these cases? If so, what is the SPR# you received? I haven't found any related SPRs through searching our SPR database, but as you can imagine, this problem could be described in many different ways so finding the right keywords to search by is difficult.

                                                     

                                                    Thanks,

                                                    Jim

                                                      • Re: Drawing Views-Problem with updating
                                                        Alex Lachance

                                                        Opening a drawing with the problem doesn't cause the problem.

                                                         

                                                        It's when the problem is caused that the drawings all turn that way. I don't know when it is caused and what causes it.

                                                         

                                                        To be more clear, before ACCE-403 was corrupted, I opened this drawing and there was no problem. I saved it, continued to work. Something  unnoticeable by eye causes the bug to happen during the time my session is active. After it has happened, any future drawing opened and saved will have this problem.


                                                        The reason I know this is I have 2 macros that run themselves when I save a file. The first does my PDF and the second does the DXF. When I click the X to exit the drawing, it prompts me to save before exiting. As I press Save and exit, the drawing proceeds to browse through every drawing page and that is when the bug happens. I can actually see the view changing in a blink of an eye as the PDF is being generated. If I'm lucky, I notice it at the first part and close the program and correct the part. If I'm less lucky, I notice it after a while and correct most of the drawings. But when I'm not lucky, I don't notice the problem, continue working and corrupt many files, proceed to send my project into production and then BAM it hits me in the face. Half the parts are not good and I need to throw them away and have them reproduced.

                                                          • Re: Drawing Views-Problem with updating
                                                            Jim Wilkinson

                                                            Alex Lachance wrote:

                                                             

                                                            Opening a drawing with the problem doesn't cause the problem.

                                                             

                                                            It's when the problem is caused that the drawings all turn that way. I don't know when it is caused and what causes it.

                                                             

                                                            To be more clear, before ACCE-403 was corrupted, I opened this drawing and there was no problem. I saved it, continued to work. Something unnoticeable by eye causes the bug to happen during the time my session is active. After it has happened, any future drawing opened and saved will have this problem.


                                                            The reason I know this is I have 2 macros that run themselves when I save a file. The first does my PDF and the second does the DXF. When I click the X to exit the drawing, it prompts me to save before exiting. As I press Save and exit, the drawing proceeds to browse through every drawing page and that is when the bug happens. I can actually see the view changing in a blink of an eye as the PDF is being generated. If I'm lucky, I notice it at the first part and close the program and correct the part. If I'm less lucky, I notice it after a while and correct most of the drawings. But when I'm not lucky, I don't notice the problem, continue working and corrupt many files, proceed to send my project into production and then BAM it hits me in the face. Half the parts are not good and I need to throw them away and have them reproduced.

                                                            Hi Alex,


                                                            A couple of questions.

                                                             

                                                            1. The ACCE-403.SLDDRW file that you are testing; has it been saved in SOLIDWORKS 2016 already? If so, this is why you wouldn't be seeing the behavior I am with double click. If you have already saved it, can you take the old SW2014 version of it that you posted on the forum and put it in a folder somewhere and then try opening that one with double click from Windows Explorer to see if it exhibits the behavior or not? By taking your files and saving them in a bad state with new versions, I have now confirmed my original finding that files will always open in a bad state in the current version, but will open OK in a future version if opened by double click.
                                                            2. Hearing you say that you are using a macro to do these drawing exports when you save, maybe it is the macro itself that is causing the problem. Perhaps it is not doing everything it needs to do when switching sheets to do the exports. I'm not saying this IS the problem, but since you mention you notice it happening when the macro is running, it perhaps could be a clue.

                                                             

                                                            Thanks,

                                                            Jim

                                                              • Re: Drawing Views-Problem with updating
                                                                Alex Lachance

                                                                Hi Alex,


                                                                A couple of questions.

                                                                 

                                                                1. The ACCE-403.SLDDRW file that you are testing; has it been saved in SOLIDWORKS 2016 already? If so, this is why you wouldn't be seeing the behavior I am with double click. If you have already saved it, can you take the old SW2014 version of it that you posted on the forum and put it in a folder somewhere and then try opening that one with double click from Windows Explorer to see if it exhibits the behavior or not? By taking your files and saving them in a bad state with new versions, I have now confirmed my original finding that files will always open in a bad state in the current version, but will open OK in a future version if opened by double click.
                                                                2. Hearing you say that you are using a macro to do these drawing exports when you save, maybe it is the macro itself that is causing the problem. Perhaps it is not doing everything it needs to do when switching sheets to do the exports. I'm not saying this IS the problem, but since you mention you notice it happening when the macro is running, it perhaps could be a clue.

                                                                 

                                                                Thanks,

                                                                Jim

                                                                Hey,

                                                                 

                                                                1. No, the file is still in 2014 I believe, as I uploaded it here. When I save it to test some stuff I save it on other names. If I do save it in 2016, the bug goes away as stated. Maybe we can do a teamviewer so you can have a look if you'd like?

                                                                 

                                                                2. It is not quite a macro but more of a third party program SolidWorks add-on that executes certain scripts. It's called CustomTools. I don't believe it is the cause as stated because the whole thing is extremely simple, so simple that someone with no programming background can understand it. The macros do not interfer with the view. The only thing they do is the first one reads to find sheets with the word ''Feuille'' in it while the other searches for sheets with the word DXF in it. If there is the word feuille on multiple sheets in the same drawing, it merges them together into a PDF, if there is only one then it'll be a lone page PDF. If there is no sheet with the word feuille, it makes a PDF for each sheet and names it as follow <Drawing Name>-<Sheet Name>. If the sheet has DXF in it, it ignores it in it's PDF process. The DXF works similar as it ignores every page that doesn't have DXF written in them. The ones that do get saved on a 1:1 scale to DXF.

                                                                 

                                                                Edit: By the way Jim, thank you so much for taking the time to have a look at this, it is really appreciated.

                                                                  • Re: Drawing Views-Problem with updating
                                                                    Jim Wilkinson

                                                                    Alex Lachance wrote:

                                                                     

                                                                     

                                                                    1. No, the file is still in 2014 I believe, as I uploaded it here. When I save it to test some stuff I save it on other names. If I do save it in 2016, the bug goes away as stated. Maybe we can do a teamviewer so you can have a look if you'd like?

                                                                     

                                                                     

                                                                    It sounds like you are unsure if it is in 2016 format. You should be able to tell because the save icon should show a yellow symbol on it indicating that saving will convert it forward. And for me, if I save the file in 2016, the problem does not go away unless I actually do something to correct the views. If the views are in the bad state and I hit save, it saves it in the new version still with the same problematic views. Are you not seeing the same?

                                                                     

                                                                    Since you seem to be seeing different things than I am, can you please do the exact steps here just to be sure?

                                                                    1. Copy the files for ACCE-403 that you posted to this thread into a new folder.
                                                                    2. Start a new session of SOLIDWORKS 2016.
                                                                    3. Open the ACCE-403.SLDDRW in SOLIDWORKS using the File, Open menu -> the drawing views should have the problem.
                                                                    4. Close the drawing without saving.
                                                                    5. Open the ACCE-403.SLDDRW in SOLIDWORKS using double click from File Explorer -> the drawing views should NOT have the problem.
                                                                    6. Close the drawing without saving.
                                                                    7. Open the ACCE-403.SLDDRW in SOLIDWORKS using drag and drop from File Explorer into SOLIDWORKS. -> the drawing views should have the problem.
                                                                    8. Save the drawing (this will convert it to SOLIDWORKS 2016).
                                                                    9. Open the ACCE-403.SLDDRW in SOLIDWORKS using the File, Open menu -> the drawing views should still have the problem.

                                                                     

                                                                    Let me know if you get different results on any of these steps. If I am understanding you correctly, you are saying you are getting different results on both steps 5 and 9.

                                                                     

                                                                    Sorry, I can't do a teamview or anything today. II'm not actually officially working today (it's a holiday here in the US) and I'm leaving shortly for an event.

                                                                     

                                                                    Thanks,
                                                                    Jim

                                                                      • Re: Drawing Views-Problem with updating
                                                                        Alex Lachance

                                                                        No problem Jim, thanks for your time again, happy Thanksgiving to you!

                                                                         

                                                                        I will get back to you on monday to answer this as I am also out of office right now.

                                                                        • Re: Drawing Views-Problem with updating
                                                                          Alex Lachance

                                                                          Hey Jim,

                                                                           

                                                                          I'm back in office today so I just had a look at this. This is what it gets.

                                                                           

                                                                          1. Copied files from this forum in a new repertory.
                                                                          2. Started new session of SolidWorks 2016
                                                                          3. Opened drawing going from file>Open
                                                                          4. Closed the drawing without saving.
                                                                          5. As I said, if what you call ''File Explorer'' is Windows Explorer, then I double clicked in Windows Explorer to open the file. The file still has the problem.
                                                                          6. Closed the drawing without saving.
                                                                          7. Dragged and dropped the file from Windows Explorer to SolidWorks window, still has the problem.
                                                                          8. Saved the drawing, converts to 2016.
                                                                          9. Reopened file, the bug is gone, views are fixed.

                                                                           

                                                                          So yes, I am getting different results on 5 and 9. Note that I have had files in 2016 have this problem so I don't think that it's something that is related to versions.

                                                                            • Re: Drawing Views-Problem with updating
                                                                              Alex Lachance

                                                                              Hey Jim Wilkinson,

                                                                               

                                                                              I just remembered I hadn't closed my SolidWorks add-on that generates PDF/DXF.

                                                                               

                                                                              If I save it in 2016, the file still has a problem when my add-on is turned off. so the only place that I differ from you is when I open it from Windows Explorer, if it is truely Windows Explorer that you were talking about.

                                                                                • Re: Drawing Views-Problem with updating
                                                                                  Jim Wilkinson

                                                                                  Alex Lachance wrote:

                                                                                   

                                                                                  Hey Jim Wilkinson,

                                                                                   

                                                                                  I just remembered I hadn't closed my SolidWorks add-on that generates PDF/DXF.

                                                                                   

                                                                                  If I save it in 2016, the file still has a problem when my add-on is turned off. so the only place that I differ from you is when I open it from Windows Explorer, if it is truely Windows Explorer that you were talking about.

                                                                                  Yes, I am talking about Windows Explorer. I am going to take this into a PM while we do some troubleshooting.

                                                                                   

                                                                                  Thanks,

                                                                                  Jim

                                                                                    • Re: Drawing Views-Problem with updating
                                                                                      Jim Wilkinson

                                                                                      For the information of others viewing this thread and seeing similar issues, SOLIDWORKS technical support is going to work with Alex and his VAR on this issue. If you have this issue, please report it through your VAR so that they can troubleshoot it as this is certainly an issue we want to get to the bottom of and figure out what might be causing it and fix it if it is indeed a problem in SOLIDWORKS. Your VAR can involve SOLIDWORKS Technical Support for additional help in troubleshooting it and you should ask them to do so if the results of your VAR troubleshooting alone are not sufficient.


                                                                                      Thanks,

                                                                                      Jim

                                                                                        • Re: Drawing Views-Problem with updating
                                                                                          Jim Wilkinson

                                                                                          I wanted to close the loop for anyone who is following this thread.  Alex was able to work with SOLIDWORKS Support and his VAR to review files which were exhibiting the problem and work out a resolution.

                                                                                           

                                                                                          Some background is needed regarding an old bug, which is very likely the reason for this thread.

                                                                                          For performance and stability reasons, SOLIDWORKS only updates drawing views when they need to be updated.  If the internal time stamp of a drawing view is newer than the body shown in the view, the drawing view will not update.

                                                                                          In SOLIDWORKS 2013 and 2014 there was a fault with AutoSave backup function. This fault saved internal time stamps for drawing views which were newer than the part file body time stamp. Because the time stamp was newer in the view, the views did not updated. This fault has been fixed in 2015 onward and so far no cases of newly created parts/drawings from current templates show this problem.

                                                                                           

                                                                                          Saving the part/drawing in a newer version does not address the bad behavior.  Editing a feature or a Ctrl+Q of the part and a save are required to update the body time stamp so the drawing view will update moving forward.

                                                                                           

                                                                                          Alex has worked with his VAR to automate the required rebuilding of part files to ensure their drawing views will always update moving forward.

                                                                                           

                                                                                          If anyone else still encounters this issue with newly created files OR if a Ctrl+Q/save of the part files does not address this issue – please contact your local VAR for additional troubleshooting.

                                                                                           

                                                                                          Thanks,

                                                                                          Jim