I'm trying to create a parrallel face mate, a pretty easy task in Solidworks that I use a lot as I'm creating assemblies. In SolidEdge I only seem to be able to select an edge, and then it doesn't make them parallel, it connects them. I don't see any menu for selecting a face instead of an edge or anything like that.
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I don't know if I understand your question correct, but I think you are looking for a floating mate, no?
Yes, Planar Align or Mate is what you are after. The Parallel relationship is for edge to edge contact. Planar Align and the Mate will do what you want, but be aware that these look like they do the same thing (make two faces parellel with either a floating or fixed offset) but they have one major difference. Mate orients the face normals (imaginary perpendicular vector on the face pointing away from the solid) in opposite directions and the Planar Align points them in the same direction.
As Ken mentioned if you think of it as a bookcase, the mate puts the books side by side and the planar align aligns their bindings.
Thanks, but I'm not sure I want either of those. I want the two faces to be aligned with each other, but not to constrain the distance or anything else. Imagine you're building a cad sandwich, you want the faces of the two slices of bread to be be parallel, but not define the distance or location in space.
When I do a Planar Align it puts them on the same plane, not what I want, I just want them parallel.
You need planar align, but click on the ruler (this is for fixed distance) and choos the blue arrows. Than the faces will be aligned without a fixed distance. (see screenshot in my first post)
Hi Joris, thanks, that wasn't working but then started working, maybe something to do with mates not updating until I move things around?? When I 'turn off' (uncheck in the tree) a part in an assembly, does that not stop the mates associated with that part from constraining another part?
I've noticed that Rigid and Adjustable Assembly are greyed out in my version. Do you know if I perhaps have some other setting that is causing that, or just due to the version I have (Design 1)? Currently I'm rebuilding the assembly with no sub-assemblies (not something I'm a fan of).
btw what is the proper process for eliminating a mate? I've been highlighting the part, click Assemble, scroll to the mate I want to eliminate, which is then visible in the small window but it's not highlighted so I can't delete it, so I select it again but that just shows all the mates again, so I have to highlight it again, then I can delete it. I'm guessing there's a better way?
Also is there a way to temporarily deactivate/activate a mate?
When you 'turn off' a part, (luckily) the constrains stay.
When you want to suppres a constrain, RMB click on the constrain an click Suppress
Eliminate a constrain:
Click on a part
RMB click on the constrain
click on the part
click (left mouse button) on the constrain
hit the Delete button
I have been wondering what the differance between mate and planar are. My mate'sm are almost always are backwards and I typically use mate. I will now switch to using planer align. Maby I won't have to flip everything now. I will likly still end up with negative offset values most of the time!