This assembly is NOT over defined, but SolidWorks continues to error the third mate.
It looks like one part is fixed and you have added a mate to the fixed part. Can't be positive on what the 2 mates are.
One mate is coincident. the other is a distance.
I need to add another distance dimension to have the parts in the correct location.
I am a 22 year veteran of Solid Edge.
I have stumbled through SolidWorks and find that it is not as good as Solid Edge.
I frequently have this over defined error in assembly and the parts and not even close to being located properly.
This is very frustrating.
My guess would be that you're trying to mate another face and if the component is an imported file from another extension there is a chance that the surfaces aren't exactly parallel/perpendicular. Delete the mates you have and find three points and mate those coincident and if they take then your surfaces have an issue...
That did not work, either.
You picked "Face" - In my post I mentioned "Points" - there is definitely something misaligned ...
Try doing 1 face and one edge (of the other face) and use the distance mate. Also, use the measure tool between the two faces. If it doesn't say that they're parallel, they're not. Even if the angle says 0.00000000000
The two faces are not quite parallel. If you look at the angle right under the distance in the picture you will see that it is not 180 but rather 179.999 blah blah blah. you might want to try using a plane instead of faces.
Michael what John said above and one other note. On most custom extrusion profiles there are variances of minor angle changes out to 4 or 5 decimal places that solidworks will burp out you cannot make them parallel.
We deal in window and door seals and see this frequently on extruded profiles especially scaled ones for pull die work where there are 2 surfaces on a profile that look parallel but are actually out by minor fractions of a degree.
The shapes were all created in SolidWorks, not imported.
I have gone to great lengths to make sure the lines in the part drawings are defined.
It seems that you have to work really hard for this program.
The program should be doing the work for us.
When I first started using SolidWorks I got those errors all the time, and you're right. They can be frustrating. I still get them occasionally. I've found that when I get them there's almost always a problem with what I'm trying to do. Is it possible that two edges that should be perpendicular aren't, or something similar? Can you Pack and Go the Assembly to a zip folder and post it here?
Can you post the assembly and parts?
Michael this is what I was talking about. The faces will not maintain a distance mate because they are not parallel.
Thanks for everyone's suggestions.
I will try to go through the profiles and make sure they are not out in angularity.
Something that has helped me a lot for mating is researching GD&T reference frame, and the minimum needed to define a point, a line, and a face.
You know you can 'lock' a part's movement with only 6 points? 3 points to define a bottom plane, 2 points to define a face perpendicular to the first face, then just one point to lock in a plane perpendicular to the other two planes. Keeping that and other things I learned from GD&T in mind as I mate parts together really helps me, and I've had to work on assemblies that are made to change on the fly as it runs through programs like DriveWorks.
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