Revolve Around An Ellipse

[maple15207]

I want to add several small rings protruding out of the outside of the pot, horizontal from top to bottom of the pot. I assume I can't use revolve with a elliptical pot, so how can this be done?

Should I copy an ellipse, extrude the thickness for the ellipse, then change dimensions of the ellipse so it will fit the pot at several heights with difference radii?

Thanks.

[jhackney1972 · Accepted solution]

If you mean like the attached model, then use a Sweep Feature to add as many rings as you desire. 

[maple15207]

Thanks. Will check out the sweep feature.

[jeff_strater]

Interesting factoid:  It is all Sweep underneath:

• Extrude is Sweep along a line segment path, where Fusion just supplies the line without you having to, based on the sketch normal
• Revolve is Sweep along a circular arc path, where Fusion supplies the arc path for you, based on an axis
• Pipe is Sweep, where you supply the path, and Fusion supplies the profile for you (circle, square, triangle)
• Coil is Sweep, where both the path and the profile are built for you, you just provide the parameters on the size and shape of the helix curve, and the size and shape of the profile
• all the primitives are variations of the above:
  • Box and Cylinder are Extrudes
  • Sphere is a Revolve
• [edit - I forgot Hole/Thread!]  Hole, I think, is actually a Revolve (that's how you get the countersunk and counterbore geometry)
  • Thread is a Coil
• Rib and Web are also advanced extrudes
• Sheet metal Flange is built using Sweep (but a lot of other stuff, too, so maybe that one doesn't really count)

There really are not that many bits of true core geometry creation functionality here...

[maple15207]

For the path, do I create an ellipse from, say, the bottom of the pot, and modify its size so it is the right size for various points up the side of the pot?

[jhackney1972 · Accepted solution]

I would create the paths the same way I created the one I sent to you, by using an offset plane through a point.  I illustrate this in the attached video.  By the way, the method I use creates a mark on the original model which of course is used as the path of the Sweep.  If you do not want to have the mark on the surface of the original body, you can the Surface Offset command to create a surface to received the mark instead.  It will still serve as the path, just does not leave a mark on the original body.  This is on important if you are creating a feature that does not cover up the mark such as a Pattern on Path.

[maple15207]

Got it. Thanks so much!