Cannot make a cut on one end of a revolve, but could extrude.

[Anonymous]

Made a fairly simple revolve for an axle hub.  Want to make 1/8 deep cuts on either end.  Make drawing, closed shape, will extrude but will not allow me to make a cut until I go far beyond my intended distance.....like 3/8+. 

Used the face of the end as the sketch location, which happens to be on one of the planes.

Thanks

[davebYYPCU]

We'll need the File, pics or Screencast, cause what you said, should work.

[Anonymous]

Sceen shot and file at that point

[I_Forge_KC]

Your hub body is a surface instead of a solid. It appears like you were in the patch workspace when you did the revolve (see the revolve surface command in the timeline?).

Either go back into the timeline and make that a solid revolve or stitch that back into a solid. If you go back in the timeline, you'll need to respecify the plane that the sketch sits on.

[davebYYPCU · Accepted solution]

Why was the revolve done in the Patch workspace?

Why is the extrude cut profile not in the hub Component?

Why are you Selecting to extrude from an Object when the sketch is on the same face?

That said, all works as expected when the Revolve is a solid.

Sketch can be moved to the Hub Component now before doing anything else, Click and Drag to the Component name.

Select the profile, and extrude cut -0.125, and the system works as expected.

Might help....

[Anonymous]

I did not know I was in patch workspace. 

Uhm, not sure on that

The last was a try of something different.

I think I will just start this part over and do it correctly.  I have no idea how I screwed this up this badly.

[davebYYPCU]

You can follow my timeline, 

move the sketch, Activate the hub, 

drag the timeline in front of the hidden patch revolve and make the solid one, then extrude the cut.

Easy fix, and its these things that teach the best lessons.

If starting again, use the origin as the centreline of the hub sketch.

Might help....