8 Replies Latest reply on Dec 28, 2015 6:04 AM by Frank Ruepp

    why do step files lose mates

    Rob Myre

      why does solidworks models and step files do not stay mated. I was told by my VAR that this was resolved SW2015 lied to again.

        • Re: why do step files lose mates
          Karl Wooster

          What exactly do you mean? A STEP file doesn't contain any mate information, and a SOLIDWORKS assembly will only have SOLIDWORKS parts in it. As such, I am really not sure what you are trying to accomplish.


          If you can clarify your intent, I might be able to assist you.



          • Re: why do step files lose mates
            Frank Ruepp

            Hi Rob,


            I am guessing that you have native Solidworks files (built in Solidworks with features) and imported Soidworks files (imported step files) mated together in an assembly.  Now you will get a new step file which is a later version of an existing file and you import it again with a new name (or the same name in a different folder).  When you replace the existing mated imported file with the new imported one, likely all mates will become dangling.

            Can you confirm that this is the issue?

            When you open a step file, Solidworks imports the geometry and creates a Solidworks file with the imported geometry.  Every geometric entity of a body has a specific ID and this ID is remembered i.e. in mates.  Those IDs get created on import.  Not sure what triggers the entity ID but usually those IDs do not match even though the imported geometry might be very similar.  When the new ID does not match the remembered ID in the mate, the mate will become dangling.

            When you know which faces will be used for mates, you can override the internal IDs with custom names (i.e. when you RMB on a face you can select "Face Properties" (you might have to expand the RMB menu since this option is not displayed by default) and then you can specify a name for this face).  This custom name is remembered in the mate and when the new part has an identical face name the faces will be replaced without making the mates dangling (at least when the geometry allows the replacement; you definitely cannot replace a i.e. a cylindrical face with a planar face even though the names might match).


            Hope this helps

            Kind regards


            Solidworks Product Definition Team