Create O-ring Groove on Radial surface

[rdkd]

Does anyone have any suggestions on how to create O-ring groove on a radial surface. (face seal on radial surface) I have tried to use Cut sweep/loft with no luck. I have also used the wrap feature but this creates a groove with tapered walls.

 

[EngJW]

Not sure I understand (you may have a complex shape) but a groove on a shaft is just a revolved cut, and on the end of a shaft it would be an extruded cut. A loft or sweep should not be needed.

 

[CorBlimeyLimey]

Check out the Tools > Feature Palette > Palette Features > Shaft. It has an o-ring feature. Just drag-n-drop onto the shaft & adjust sizes to suit.


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[rdkd]

I wasn't clear, what I am trying to create is. The groove is on the OD of the shaft and not around the OD. I have a round shaft that has a hole perpendicular to the shaft centerline. Around this hole is the O-ring groove.

 

[Muggs828]

OK, if I understand you correctly, you have a hole in a shaft like a finger hole in a flute?!

What I would do is offset the outer surface of the shaft the O-ring depth before you cut the hole in the shaft. Then cut up to surface the diameter of the O-ring.
I hope that makes sense!
I’d be happy to send you an example if you like.

Muggs

 

[TheTick]

Face seal on a cylindrical surface.

Got it. I'm doing something similar at this time.

My case is easier, since the face is spherical, resulting in a planar O-ring groove.

Is your part molded or machined? A machined part will probably be easier, since you won't need to incorporate draft.

For a machined part, I would try wrapping a curve for the groove centerline or edge. Then use the wrapped curve as a guide for a sweep cut. The section for the sweep should be on a datum plane made especially for the purpose using normal to curve, constrained normal to the guide. The section sketch should be constrained w.r.t. the guide curve with a pierce constraint.

For a molded part, start like one would for a machined part, then add features to provide draft as needed. there is a way to do this with a single sweep, but it is too much to explain here.

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[rdkd]

OK I got it. I was able to create the type of groove I was looking for by wrapping a curve for the groove for the OD of the groove then creating a composite curve along with the section of the groove then cut-sweep. thanks for everyones input.