17 Replies Latest reply on Mar 5, 2017 6:49 PM by Robert Kirkwood

    solidworks continually losing mate references

    Matt Furches

      We use a simple widows server and windows explorer to manage files. No pdm system. The problem is that regularly when I open an assembly it has lost many of its mate references such as faces or sketch points and they have to be reselected. It seems to be worse on imported files than on natively created ones. Is this happening to anyone else? I have noticed that any assemblies I store on my local machine are not as likely to have this happen.

        • Re: solidworks continually losing mate references
          John Stoltzfus

          Did you just upgrade to 2016 ??

          • Re: solidworks continually losing mate references
            Eric Blankinship



            I've had this type of issue happen before when people didn't save/move models correctly and the internal part ID's got screwed up.  But that doesn't sound like what is happening here.  Another possibility is that the geometry used to define the mates has been changed or removed.  Not sure if any of these things will help but just throwing out some common things that can cause mates to have issues.



            • Re: solidworks continually losing mate references
              Sarah Dwight

              Do you work with sub-assemblies?

              I had my main assembly blow up with red and yellow warnings in the feature tree, and when I tried to track it down, nothing appeared wrong in the sub-assemblies. Turned out I had a mate reference in one sub-assembly that was countering a mate in the main assembly which in turn ruined all my other mates. Suppressing the mate in the sub-assembly fixed everything in the main assembly.

              • Re: solidworks continually losing mate references
                Matt Furches

                I do work with sub assemblies but the problem isn't coming from mates fighting each other. the issue is missing mate entities. Thanks though!

                • Re: solidworks continually losing mate references
                  Paul Risley

                  To clarify what you are seeing:


                  #1) Parts in assemblies are losing mates. Said mates can be re-established using same faces/ sketches, Etc.


                  #2) Your assemblies are having trouble recognizing faces, sketches and such of parts.


                  The reason I am clarifying is I read this whole string of conversation, and it sounds like your parts are not physically moving in folder structure. (That would obviously be a different issue).


                  So your parts are geometrically unaltered from the last saved assembly and your mates are unable to resolve because of lost features.

                  I have seen this happen both to imported(primarily) and native(very rarely) created files, if I remember correctly a lot of it revolves around the imported surfaces not being properly stored in memory. (Nothing you have done by the way.)

                  We re-installed solid works and had to create a template just for surface models. So that when we imported it did not create just surface 1,2,3 and so on. But that we had to create unique names for all surfaces and bodies. Otherwise you could have a part open and then open the next part and both have body 1 the graphics would glitch out, and I swear to God I could picture the little gremlin of Solidworks having a seizure.

                  Ok I wrote way more than this and got off topic, so my original point to this response is check numbering of faces and sketch entities, the other thing I would make sure of is there is no other part named as the one that is giving you troubles in your assembly open @ the time you have it open.


                  And 1 last thing, I had a guy who worked for me as a detailer and he thought he knew everything there was to know. Anyhoot he thought that he had to change the configuration name on a non-configured part to represent what that part was.Since the name of all of our base configurations is Default, this apparently collided with his OCD. Of course by changing all of these to new names after establishing the hierchy of the assembly caused many a pissy moments for myself and all others on these projects.

                  These are just some of the things I have encountered that might create the problems you are seeing.


                  I hope it helps, and if not well at least I got to stay at work for an extra 15 minutes.

                    • Re: solidworks continually losing mate references
                      Matt Furches

                      Paul ,you are correct about the problem. Can you clarify what you mean about creating a template just for surfaces?

                        • Re: solidworks continually losing mate references
                          Paul Risley



                          This box is checked because we have a separate template for importing files.

                          Primarily it is used for single part multi body parts, but we do have one Template for importing assemblies as well.

                          As far as auto populating names for bodies and surfaces, we do not have that. We manually re-name them based on prints we get from a customer. So if we have 4 surfaces that are datums A,B,C, & D we name them in the model accordingly. All other surfaces and features we would name descriptively what they are.(We also add a 4 number prior to feature name). So it would look like this:


                          This way there is no way it could overlap an internal ID of another part.

                          We keep an Excel spreadsheet in our job # work book that tracks all newly created internal ID #'s.

                          I know this sounds like a lot of work, but it saves us the headaches that we were experiencing. Which were very similar to what you are seeing.

                          I hope this sheds some light on what I was talking about earlier.

                          Good luck on your end of it.

                      • Re: solidworks continually losing mate references
                        Matt Furches

                        Paul thanks for clarifying it. Unfortunately our imported assemblies have hundreds of parts and thousands of faces so that wouldn't be a solution for us. If this is a solidworks problem and not a local server problem I'm surprised more people aren't experiencing it as I would think lots of users import large assemblies.

                          • Re: solidworks continually losing mate references
                            Paul Risley



                            I would still set up a separate template for importing assemblies and parts. I believe this was one of the solutions our VAR had when we had this problem. On our bigger imported assemblies we convert them into parts(Save assembly as part), this had worked really well in the respect that we no longer have the face and surface issues.

                            The method I clarified above was for parts that were problematic or you knew you were going to have to use the geometry in your tooling. We do a lot of surface cutting so we had to find a way to stabilize models in a fashion that we never lost surface data. That is what we use the log for. In our parts we reference the feature number in all of the profile cuts so we have traceability if there is ever a surfacing issue.


                            SO in your case we would bring in an assembly saving it out as a part right away.This took away the lost references. In our case it was pretty consistent, we would save an assembly using the tick box for saving all parts in the same folder. Then we would place the assembly in our models, as soon as you closed and opened it back up there would be missing references. This is when our VAR said we should try using a separate template for creation of assemblies from existing files. While we set this up we tried the saving as a part for assemblies option as well. These 2 things completely cleared the issue up, it has been 3 years and we have not seen it again.

                            I should really have led off with this description in my reply, sorry to have confused the issue. Like I said it has been 3 years ago since we really had to deal with it. I blame old age and not enough coffee for my brain fart on this one.

                            Now as far as repairing mates you already have if you go in and re-establish the mates. Then save the assemblly close it out, close sw then re-open sw and the assembly, if those mates still show as losing their references the above options will fix it. However if you repair mates and close out and re-open and the mates are still there, that is a different issue altogether.

                            A lot to read I know, hopefully something in this novel will be of help to you.

                            Good luck.

                          • Re: solidworks continually losing mate references
                            Paul Risley

                            We just had a step file that created this problem again, after thinking it was resolved. So we packed up our templates and the step file and sent them over to our VAR. Found the problem. Internally one of the parts had an issue when imported, if you opened that part of the imported assembly and did an import diagnostic found gap issues, none of which could be repaired. If that par is suppressed in the assembly all is fine. Mates stick the way they are supposed to after closing and re-opening assemblies. If that part is active all mates blow up. On a side note we do not mate to the bad part in question at all(it is weld bead detail on customers weldment). But we have to leave it on so they can see in tooling fixtures access points for welding.


                            So I am going to call this a bug within Solidworks itself. If there is an issue in a part and the rest of the assembly is fine the lost surface mating issues SHOULD NOT EXIST. Yes I am shouting as this defies any reasonably sound logic to be an issue at all. This should not happen as it has no impact on the resulting mates.


                            My VAR(Symmetry solutions) vetted this out to be the case in which we were seeing this issue. Their option was to either repair or replace faulty parts, Since some of our weldments range in the thousands of parts imported going through them all and doing import diagnostic would be a needless chore as  I will claim the software is not living up to it's end of the deal.


                            My rant is over but my frustration remains, while the software performs well in many categories it is the glaring simple things that do not work that frustrate me on a daily basis.

                            • Re: solidworks continually losing mate references
                              Robert Kirkwood

                              I am developer working on an add-in for repairing broken associativity.


                              I can suggest 3 solutions:

                              1 - Assure that all the referenced faces/edges have names before you create the mate (as others have recommended).  There is a system-option setting to assure names automatically.  If those names somehow get lost, please post the file and I will see if my toolset can repair the names and mates.  I believe it can.

                              2 - If your mates were created referencing unnamed faces/edges, assigning names to those faces/edges after the mate is created doesn't help.  My toolset was able to repair the one case I encountered but it may have been specific to those particular mate types, so I'm looking for more such cases.  If you can post the files I would welcome the chance to fix them.

                              3 - If you are using imported files, I can definitely fix any mates that reference them and would welcome a chance to show off.  Please post the files or contact me.