Hello,
I have a part with a hole, a small ruby ball, and a nother part with a hole (a leafspring). The ball is bigger than the holes and is supposed to be clamped between the two parts. How can I tell SW to "connect" (don't know the English menu item) a sphere to a circular edge?
--Daniel
You will need to create a layout sketch in one or more of the parts to use for mating (assembly mates is the English phrase you needed). You can't currently mate a sphere to a circular edge. At least, id didn't work when I tried it.
Couple ways -
Easiest would be to create a plane in the sphere that would be where the sphere would contact the surface of the mating part, then mate the plane to the face....
Another would be to create a point on the surface of the sphere and dim to where the sphere would contact the mating part, then mate the point coincident with the face....
I'm doing this on the fly and didn't try it, but it seems simple enough...
Hope this helps...
Scott
BTW, of course the negative about this is if you change the size of the sphere, you'll have to adjust the plane (or you could set up an equation)...
I just tried this and it worked...
Use ad 2D or 3D sketch to place 3 points on the edge of the hole. equal spacing is nice but not really necessary. Mate the surface of the sphere to each of the 3 points.
You can make the sketch at the assembly level so your part doesn't have to carry the sketch around out of context.
Cool... gonna' remember that...
MT
You can also place a 2d sketch in your sphere's part containing a point at the center of the sphere ( or use an existing point if thats how you defined your sphere ). Create concentric relationships between the point and the holes.
Small radii on the edges of your holes ( can be extremely small, ie. .001" ) should allow you to create tangent relationships between the surface of the radius and the surface of the sphere.
Thanks guys for all the suggestions. --Daniel
Personally, I don't ever like the "small radii" type solutions. If I wanted a small radii, I would make one, if I don't, then I won't. The tool should not dictate my geometry. Ever.
Fortunately, I use SW, so in this regard I am generally not bound.
In this type of case I usually use a co-incident relation between the sketch that created the hole, and the spherical face. It depends how you made your hole where the sketch point comes from - if it is a circle and extrude-cut then you might have to add a sketch point to the cut sketch...
Cheers!
"Brian" at the center of the sphere ( or use an existing point if thats how you
Daniel
Another easy way to accomplish this is to create a surface revolve of a sphere on the perimeter of the hole in the leafspring part, and mate the surface revolve with the ball. Hide the surface revolve after mating.
Dan Sommerfeld
Daniel Haude wrote:
supposed to
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