Attach *.sldprt of your attempt and images of something similar that already exists in the real world.
Sketch a profile of a revolve on an arbitrary cutting plane through the revolve
Note: this is not asking how to sketch a revolve.
Given an arbitrarily shaped revolve in an arbitrary location in space, a fully defined plane is constructed to cut through the revolve in an arbitrary orientation. The plane cuts through the revolve creating an invisible silhouette profile on the plane. The question is how to turn that silhouette, the outline of the revolve, as it intersects the plane, into sketch entities, on the arbitrary plane.
Here's a way that will work.
Define a cutting plane A through the revolve. Plane A is arbitrarily defined in any orientation*. The only requirement is that it cuts through the revolve, somewhere between the center and extreme-outer-tangency. In the design tree, set plane A to show.
Then define a second plane B perpendicular to A and any desired secondary reference.
Select plane B, open an extruded cut and sketch a least one line coincident to cutting plane A and through the revolve. (In my case, I drew a corner rectangle that enclosed the entire revolve, except for one edge that was coincident to plane A, which cut through the revolve.) Cut the extrude to the desired thickness. In my case it was a through-all in both directions. This creates a cut through the revolve, exactly on plane A.
Change the transparency of the revolve, so that you see through it.
Select plane A, view normal to plane A, and open a sketch on plane A.
Hover your cursor over an entity that is made visible by the cut on plane A. Click to select and highlight. Then use convert entities to create actual lines of the exact shapes shown. When all desired features are selected, exit sketch.
Select the sketch just drawn. Ctrl + C to copy. Select a sketch plane that you want that sketch to be on, presumably A (if not A, then any other arbitrarily defined plane). Ctrl + V to paste the sketch onto that plane. The sketch will be undefined, and can be defined to your satisfaction.
If you don't want the extruded cut to be permanent, suppress the extruded cut. The sketch made from the extruded cut will also be suppressed. The sketch copy is separate and will not be suppressed.
In the sketch copy, you now have the sketch of a profile of a revolve on an arbitrary cutting plane through the revolve. That sketch is portable to any other plane on any part.
Here is a way that won't work. You can't use Section View at the arbitrary plane and while viewing normal to the section view, select features or lines on the revolve and use Convert Entities to create sketch lines. (Although you can see the exact shape you want, it is somehow external to the sketch.)
Phil Marra's answer above may produce an identical or easier result. I just don't know how to use sweep tools, 3D sketching, etc.
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