I'm currently designing an ATV stand for personal use and ran into a bit of an issue. I am trying to center a 2x2 square tube over a bolt hole on a base plate. I've been trying for awhile using mates but have been unsuccessful. If someone could point me in the right direction to go about this mate I would appreciate it.
BTW, I am self-taught/still learning Solidworks 2014
You can also use width mate to achieve that.
There are 3 reference planes and an origin in every part file, you can use them or you can use existing sketch entities, or create new sketch(es) for mate references.
Deepak is correct, use the Width Mate. Control select the two flat opposing sides and the round surface and choose the width mate.
Bernie and Deepak are right. But width mates are computationally very costly. A concentric mate to a sketch entity may be the computationally simplest mate in SolidWorks.
Mike is right too! For a permanent fix that isn't going to FEA or further studies of that nature I sometimes cheat and extrude cut a hole into the inner walls of tubing. That cut only needs to be as deep as can easily be visually recognized. Some of mine are .100 and some are just .010 deep.
Sometimes I just make an extra sketch with circle in it for similar purpose.
I should make a new axis by the crossing of the X and Y plane, mate that axis with your bolt hole and it stand nice in line with your hole
Darryl,
If you were using SW 2015 you could use the Profile Center mate in the Advanced mates section. If the bolt hole is on a flat plate, pick the edge of the bolt hole & the end face of the tube.
The extrude of your tube should have a sketch that looks something like this. Ensure your origin is at the midpoint of the diagonal line. Then, at the assembly, mate the origin concentric to the circle.