I sometimes have to import files from customers. Every now and then it comes in "crooked". By this is mean, no face is mated to a plane.
How could I go about mating faces to the planes?
Use Body-Move/Copy, with the Mate Settings option. This way you can align the part the way you want. See attached.
Thank you. the part you attached worked perfectly.
In trying to replicate what you did, I am running into a problem.
I go to: Insert - features - Move/Copy. In the "Bodies to Move" box I select the face I want to mate. Then in the "Mate Settings" box, I select Top Plane. Then I select coincident. Then If I click the "add" button below the "Mate Settings" box, or the Green Check at the top. It asks to "Please select two mate entities".
I have had no luck trying to get this feature to finish out.
Please see attached screen shot. When you selected the face, all you were doing was telling SolidWorks which body you wanted to move.
Then in Mate Settings, you need to do your normal mate selections.
I would use the method suggested by Bill but I would go one step further to that.
I would orient the part or body as required using one of the following method:.
If you want to do part, insert the part into new assembly and mate. If you want to orient body, use Bill's method.
Now once you done, I'll export the file and re-import it. This would make the part/body aligned as required with no extra features.
For Assembly case: Save assembly as part file and then open/use that part.
For Part case: Save as Parasolid/IGES/STEP (either of these format would work) and then re-import exported file.
Keith go to reference geometry coordinate sys set a new where you want save back out as parasolid look at options on bottom output coordinate sys select coordinate system 1
Retrieving data ...