Is there a way to set a mate tolerence? I'm trying to mate two components but I get this sillly error:
"The components cannot be moved to a position which satisfies this mate. Planar face and line are not parallel. Angle is 0.00014834deg."
Suffice to say that manufacturing tolerences etc will not allow precision to the ten-thousandth of a degree...
Thanks John, I should be more specific. I've got two concentric mates already specified, these previous mates constrain the part down to 1 DOF (sliding along the length of the axis). The final mate is a face-face which will eliminate the final DOF. Problem is, due to (unknown) the two "parallel" faces are out of plane by 0.00014834deg. Technically this is an invalid constraint... Question is, how do I workaround it?
face to face eliminates two degrees of freedom-which is why're you're over-constrained
Fix your modeling so that they are actually parallel or use a mate with fewer DOF reduction as John said.
Eddie,
One workaround is to pick a point on one of the faces and then mate the point to the other face.
Jerry Steiger
Jerry, that can be made to work. Thanks.
-you can try a limit mate with an angle but limit mates are tricky and unstable.
The problem is you've overconstrained the mates on the parts. In total, you only have 6 degrees of freedom. If you already have a coincident mate between two faces on either the components (and those mates are on the path to ground), then you've elmiinated two rotational and 1 translational degrees of freedom. Adding another coincident mate, duplicates one of the rotational constraints. If the faces were geometrically parallel, then the mate would solve because although it duplicates constraints, it doesn't produce conflicts amoung them.
Try creating the parallel mate between an edge on one component and a face on the other-or correct the geometry of the part with the fudge factor. You're shop's not gonig to build bad parts because the geometry is more precise than the tolerances indicate.