I have a part in an assembly with a reamed hole. I would like to drag a 1inch long dowel pin into the assembly and have it mate concentric to the hole and also out of the hole 1/2". How do I create this smart mate?
See Help file
You can add mates automatically between features that have a "peg-in-hole" relationship. The requirements are:
One of the features must be a base or boss, and the other must be a hole or a cut.
The features must be extruded or revolved.
The faces that are used in the mate must both be of the same type (either a cone or a cylinder, not one of each type).
A planar face must be adjacent to the conical/cylindrical face of both features.
To create peg-in-hole SmartMates:
Do one of the following:
In the FeatureManager design tree of a part document, select a feature with a cylindrical or conical face. Drag the feature name into an assembly graphics window.
In the graphics area, select the circular edge of the screw head and drag the component into an assembly graphics window.
When the pointer is over another cylindrical or conical face of a hole or cut (when you drag the feature name), or a circular edge of a hole or cut (when you drag the component), the pointer changes to .
A preview of the part snaps into place. If the preview indicates that you need to change the alignment condition, press the Tab key to flip the alignment (aligned/anti-aligned).
Drop the part.
Two mates are applied: a Concentric mate between the cylindrical or conical faces, and a Coincident mate between the planar faces that are adjacent to the conical faces.
When I do this, the dowel is concentric but either out of the hole 1" or in the hole 1". I want it in the hole 1/2".
Unfortunately Smart Mate (™?), isn't smart enough to accept a distance mate as one of the mate types. Mate references aren't smart enough either. So, you have to add some kind of circular edge to your dowel in the position you want it to mate. You can use a split line, or you can add a surface body (hidden) to add the smart mate reference to.
I made a round flat surface and added a mate reference to the edge. It just doesn't work. Change the mate reference to the edge of the round solid, it works, but the dowel is in or out all the way. I can't get sketches or split lines to work with a reference mate either. I can create a little solid ledge in the center of the dowel that works fine, but this isn't really what I was after. I don't understand why I can't create a reference mate using an axis and a plane.
Mate references are hairy and hard to make work. The major pain is that they aren't any good at finding suitable geometry to mate to. You can create a named mate reference on the part you want to put the dowel in, but you have to do that for every hole. Last I checked, library features can't contain mate references, so that door is closed too.
I did it! I created a disjoint SOLID inside the solid dowel pin with a face and edge at the correct position. Just extrude and detick the merge result option. Now add a reference mate to the edge and coincident face. Hide the burried solid body. Works perfectly. No seam lines on the drawings either.
I'll give you the star since your hidden surface idea led me to this solution. Thanks.
Hey, you're welcome. I'm surprised that you needed a solid body though. I know my dowels (sorry, my company's...) use a revolved surface. Hopefully that extra solid won't be significant to any of your mass properties calculations.
I don't need a mass calculation for anything I have done yet, but I would like to get the dowels to mate with a revolved surface just in case I do need to calculate mass some day. Could you reply and attach one of your dowels? I just tried again and I can't get a revolved surface to work. I can get a concentric smart mate but not a coincident to lock the height. Thanks.
I can't give you my company's model, but I think this screen shot shows what I did.
That did it. The reference mate must be on the edge that you have shown where two surfaces meet. I attached my file in case anyone else might want it.
Nice workaround, but that's pretty lame how SolidWorks has to use a circular edge. It's funny, but before this, I never paid much attention to the details of how the mate references work. After reading the help, the mate references are very limited in what they can do.
I can see some ER's for this...
Try inserting a reference plane into the dowel pin model that is the distance you want. Then edit your mate reference and replace whatever is used for the coincident mate with the reference plane.
You can use the Front - Top Or Right plane you used to model the dowel pin.
Then use Distance the Offset mate to the face you want to be .500 away from.
This works Great.
You can add mate references for the concentric mate (dowel to the hole)
but not the distance. That will have to be manually added with the distance mate.
Now, if this is a re-occurring condition you may want to consider recording a macro for this.
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