5 Replies Latest reply on Aug 23, 2016 7:09 AM by Jacob Murray

    Mating errors between configurations - same parts but it says 'missing faces'

    Jacob Murray

      I have made a simple vat that I would like to make several configurations of so I can have a few different volume choices, however I am having trouble with the mating of it between configurations. The vat walls are just extruded square sheets that I have converted to sheetmetal, with the dimensions for the sketches used as the configuration dimensions.


      However now when I select another configuration and unsupress the same mates used on the first configuration, all of them have errors. When I edit the mate feature it says the faces are missing.






      I use configurations all the time with my other work and I don't know why this is happening. I figured the walls should all have the same reference faces between configurations and the mates should be relevant to them all, but that doesn't seem to be the case.


      I have attached a pack and go file with all the assembly I am working on. Would someone mind having a look at this for me and let me know where I have gone wrong please? (It's Solidworks 2016)



        • Re: Mating errors between configurations - same parts but it says 'missing faces'
          Vladimir Urazhdin

          Different configurations may create different features ID (in your case wall). Mate refers to feature ID and this is the reason for error message.

          Just create a new mate for a new configuration and configure it: keep an old mate for a new configuration suppressed and suppress a new mate for old configuration.

          • Re: Mating errors between configurations - same parts but it says 'missing faces'
            Bill Toft


            A few guidelines when doing multiple configurations:

            1. This should be considered MANDATORY: Fully define all sketches. That way, when a dimension changes you control what happens to the sketch shape! For the rectangular shapes, just drag a corner to be coincident with the Origin. For the Hook, you need more dimensions/relations. Make sure all sketch entities are black (instead of blue).

            2. Do your mates in a logical order and use the absolute minimum number needed to fully define the part (no "-" in the feature tree). I think you have extra mates that cause conflicts. This will generate mate errors. 3 coincident mates is all you need for a single part.

            3. Add the parts in a logical order of assembly.

            4. If possible, mate a new part to only one existing part. Bottom is your fixed part and so should be your first choice for ALL other mates.. Make Side<1> the second part. It can be fully defined with 3 mates to the Bottom. Then add Front<1>. 2 mates to the Bottom and 1 mate to Side<1>. Same for Front<2>. Then add Side<2>. Make all 3 mates with Bottom. Make all 3 mates of Hook<1> and Hook<2> ONLY to Front<1>.

            5. Hook is the part giving you mate issues. As Vladimir said, when you have a part with 2 configurations that are created by 2 different features, you have 2 unique parts (from an assembly mating perspective), so need 3 unique mates for each configuration. My suggestion is to use ONE base flange feature and just change the dimensions in each configuration. As per #1, the Hook sketch is not fully defined, so add relations & dimensions to fully define it for the first configuration. Then change the dimensions to get the other configuration.Now you only need 3 mates to handle both configurations.


            Getting off-topic, I see 2 parts (Bottom & Side) were done in student edition, so your assembly is now flagged as educational. To fix that, create brand new Bottom & Side parts then create (from scratch) a brand new assembly (using the above guidelines).

            • Re: Mating errors between configurations - same parts but it says 'missing faces'
              Jacob Murray

              Thanks guys. I tried all the suggestions but ended up having to re-do it all from scratch. We have over 50 different configurations so to re-do every mate would have taken a long time, not to mention re-doing all the dimensions in the drawings. Making new walls off the one common feature is what we did in the end, like you pointed out Bill. We had no mating problems, but are now dealing with Solidworks errors in the drawings for some reason. I have posted another topic on that point.

              • Re: Mating errors between configurations - same parts but it says 'missing faces'
                Tateos Tvapanyan


                On a part level, you got a suppressed feature "Convert-Solid1" for all configuration except 85 wide.



                Unsuppress it and everything will be fine then.




                Do that for all parts!!!!