17 Replies Latest reply on Oct 2, 2017 8:40 AM by David Matula

    mates breaking

    John Chesna

      Hey yall,

       

      I've tried searching the forums with no luck, kept getting redirected to some jiveon forum site.  So I didn't come up with any search results, it keeps wanting me to post.  Not sure where to post or look, but whatever, onto the question.

       

      How do you build large assemblies without the mates breaking?  I see those pictures when SolidWorks is loading, and I'm thinking, "No fricking way is that possible!".  I can't even build an assembly with 100 machined pieces without parts jumping to a mated connection or flying off the screen.  And we're talking simple geometries.  Square edges and circles.

       

      I've downloaded the hotfix and patch that was supposed to clear this up.  When it first started happening I started investigating and noticed that this is an actual problem in SW 2017 and patches were created to help fix it.  Well, instead of parts flying off the screen into the void of the SW workspace, they now slide into position, breaking previous mates. 

       

      What am I doing wrong?  What are the tips?  How can I make this stop?

       

      Here's another scenario.  I mate everything up, it all fits good.  I use measure, verify dimensions, everything is spot on.  MMM, gravy.  I save it, close it.  I open it not even 5 minutes later with red text over all the mates!  WHAT!  Click rebuild.  Changes from red to Yellow exclamation warning.  Well, that wasn't there before, what the heck happened?  OK, close it all, save nothing.  Open it again, same problem.  Ok.  Ok.  Start from scratch.  Rebuild it all.  Everything fits.  Click save.  Gravy.  Close it.  Go home.  Come back the next day.  Red mates again!  Ok, go throug mates list, delete the most recent red mates.  Red text disappears.  Save. Close.  Open............ RED TEXT!1!1!!!!1111!

       

      I can create stable assemblies when there are few mates.  Anything for large assemblies, red with problems all day long.  This is a problem as we're building a machine.  I cannot create a stable assembly.

       

      I run SolidWorks Rx tool, it suggests updating graphics driver.  Ok cool.  I update driver from the link provided by the SolidWorks toolbox.  Reload the Rx tool, "Check your driver, the current one is not supported." Seriously?  I just downloaded it from your own dialog box!  This is the one you suggested I download!

        • Re: mates breaking
          David Matula

          use a bunch of sub assemblies....

          patterns  (hole wizard sketches...feature driven ect...)

          mirror parts...if you can use this helps prevent mating things again and again...

          good mating practices....

           

          I prefer mating surface to surface...make sure that surface is not going to change.....and all parts have to more or less be finalized....

          if I am adding a part or fixture that is not finished I will  blow away all the mates I used to hold it in place and then re mate it in the assembly.

           

          changes....will always happen as long as surfaces and planes that u use to mate to do not change names ref # or what ever solidworks uses to remember how things went together so when you open up the assembly on Monday it looks the same as on Friday when you last saved it.

          I don't worry about fully defining every nut and bolt....they spin....but other parts I always check to make sure they do not move.

           

          creating mate folders....another great idea....for large assemblies....put mates for some stuff in a folder so if you want to change something down the line you can find it quickly later....

            • Re: mates breaking
              Matt Peneguy

              David Matula wrote:

               

              use a bunch of sub assemblies....

               

              If you have more than something like 20 or 30 mates (maybe less) break it into a sub assembly.  And some mates work better than others.  I don't use angle mates, and try to keep the advanced mates to a minimum.  I created an assembly with about 10,000 parts somewhat following those rules and it works "okay".  But changes to that assembly are very difficult.

              I am now using the Skeleton Sketch Part method (also called Master Sketch among other things), with help from somebody who has already provided you an answer, John Stoltzfus.  I even created a thread at Skeleton Sketch Part Method for Large Assemblies.

                • Re: mates breaking
                  John Chesna

                  Hi Matt,

                   

                  Hmm that might be it.  I am using quite a bit of advanced mates.  A lot of slots and a lot of widths.  I've chosen those over coincident or concentric to simulate the adjustment and movement of the machine. 

                   

                  Maybe I'm doing it wrong from this approach - Is the assembly the best place to simulate movement?

                • Re: mates breaking
                  John Chesna

                  Hi David,

                   

                  Thank you for the reply.  Yes I am doing most of those things.  I've tried making smaller assemblies, then adding them to the large assembly.  I try to mate the simplest surfaces.  I strip fasteners of their threads or just use shafts of the max thread diameter to simulate a fastener or anything threaded.  I turn off simulated threads in tapped holes.  For o-rings I create flats on them so that I can have a concentric or coincident mating surface.  I put fasteners in a folder, then hide the folder.  I keep fasteners spinning (only 2 mates).  I try to base my mates off of centralized parts.  If a fastener is holding something, I do not mate it that way, I mate the actual parts concentric to their holes and use the fastener mate mainly as decoration in the hole.  I've built it without fasteners. 

                   

                  From this point I was thinking, hmm, probably the fasteners causing the issues.  Nope.  Even with the smaller assemblies inserted, flexible turned off, when I mate something to an already fully defined item, the fully defined item will "jump" and break its fully defined mates so that it can mate to the random piece.  Click rebuild.  Try again.  Fully defined item still jumps.  I see the yellow warning in the mate dialog box, click cancel and do not proceed with the mate.

                   

                  Since it's a moving machine, I make some assemblies flexible.  Movement becomes limited.  Pieces stop before their full stroke can be achieved.  I've found if I open the subassembly with the moving part, move it around in the subassembly, click rebuild, move it around again, click save, go back to large assembly, click rebuild, the full stroke can magically be achieved.

                   

                  I'm not editing the parts once they're in the assembly.  If I do have to edit something, I've found, although it is tedious, to rebuild the whole assembly anyway.  I scrap it all and start fresh. 

                    • Re: mates breaking
                      Jim Sculley

                      John Chesna wrote:

                       

                      ...

                      when I mate something to an already fully defined item, the fully defined item will "jump" and break its fully defined mates so that it can mate to the random piece. Click rebuild. Try again. Fully defined item still jumps. I see the yellow warning in the mate dialog box, click cancel and do not proceed with the mate.

                      This is highly suspicious.  Have you dismissed any dialog boxes with the 'Do not show this message again' checkbox?  You can check this in Tools...Options....Messages/Errors/Warnings.

                       

                      Flexible assemblies are great, except when they are not, which is pretty much all the time.  When they are nested many levels deep and involve multiple configurations, they become much more unstable and flaky.

                  • Re: mates breaking
                    John Stoltzfus

                    Has nothing to do with your Driver, all has to do how your assembly rebuilds and how you are relating components to other components or to other sketches within the assembly...  What you're experiencing can be eliminated completely, been there done that..

                     

                    I would love to see your entire assembly and to evaulate it, but time isn't on my side, however you could upload snap shots of your feature tree (expanded)  -  might be a glaring clue right there...

                    • Re: mates breaking
                      Paul Risley

                      John,

                      This is in reference to closing and opening the model to see red then yellow.

                       

                      Are any of the parts you are mating to imported files?

                      (Step,parasolid, etc...)

                       

                      These do not have to be where the mates are blowing up, just are there imported parts that have been converted to Solidworks files in your assembly?

                       

                      If so that may be causing an issue, we had that happen all of last year and into part of this year. Imported assemblies with internal parts were losing their "part id's". We never got a solid fix on what happened. After Solidworks 2017 SP02 it stopped happening, but I know it started in mid 2016 SP02 or so for us.

                       

                      As far as large assemblies go breaking into subs , using reference geometry planes axis etc goes a long way into building big assemblies.

                        • Re: mates breaking
                          John Chesna

                          Hi Paul,

                           

                          Thank you for the reply.  No, no imported parts.  All parts are being designed fresh for us to machine which is why I wanted to load this machine up in SolidWorks to simulate the "fit and finish" sort to speak.  Typically I stick with AutoCAD and create multiple views to simulate movement.  But seeing the advanced mates added into SolidWorks made this very tempting to try.

                        • Re: mates breaking
                          John Chesna

                          Just wanted to add, thank you everyone for your comments.  I've been reading them all and appreciate the info and the different thought processes / logic to these setups.

                          • Re: mates breaking
                            Paul Risley

                            John I just re-read your original post. If you have parts a,b, and c in your assembly mated. Then add part d and mate that to any of the prior parts the inclination is that part d will move to the part already mated into your model. If your part a,b, or c is moving to d then there is something wonky in the mating condition.

                             

                            I haven't seen that behavior in a couple of years so I am not going to be able to offer much in the way of a solution.

                             

                            In regards to the update of 2017 what they fixed was the dialog box of "do you want to overdefine the assembly with this mate." Now if you hit esc at this point it does not put that mate into effect. Prior to 2017 if you hit esc on the dialog it placed that mate and you had to undo it.

                              • Re: mates breaking
                                John Chesna

                                Hi Paul,

                                 

                                Yes, that exactly.  If I have A, B, and C mated and fully defined.  I add part D to the assembly, and instead of D moving to the fully defined parts, the fully defined A, B, or C will move to D, breaking their existing mates.  After reading yours and others comments, I'm checking my settings to make sure nothing is over riding how things are "supposed" to work.  But I'm also thinking this happens because of the multiple advanced mates being used.

                                 

                                I keep everything at default, but I'm also aware that patches can sometimes change settings.

                                 

                                Thanks

                              • Re: mates breaking
                                J. Mather

                                The best way to get at the root of the issue is to attach an assembly here that exhibits this behavior.

                                I will make wager someone will figure it out within 30 minutes of posting.

                                • Re: mates breaking
                                  David Matula

                                  Flexible, assemblies.....in the old days we would use configurations for this and suppress one mate and add another, and show max and min distances and nothing in between....kind of fun to make sure you hit nothing along the way if the movement was a long distance....but then again that was at the top level where I would do that.  Sounds like you have many levels of movement... locking them down may help out.