How to create a lid on a cut sphere

[Anonymous]

I have an example here http://a360.co/1PU5mnZ

I would like to close off one end of the ring (which is a slice out of a regular sphere) with a 2mm lid, same wall thickness as the ring alredy has.

I just cannot think of a way to do it and I am sure its dead easy and I might just be too tired.

Any help would be appreciated.

[Anonymous · Accepted solution]

Nevermind, figued it out. Just needed to project the ring as a body onto a new sketch which then created the lid.

[mstrater]

There are several different ways to do that.

One option is to create a sketch on the end that you want to close off, and then extrude by 2mm, selecting the ring profile and the circle profile it encloses. The issue with this approach is that the cap won't match the curvature of the sphere, but that might be ok depending on what you want.

If I was to do it, though, I would delete the previous shell command from the timeline (so you end up with a solid slice of a sphere) and then do a new shell command with a thickness of 2mm on the solid sphere slice, selecting the side you want to be open.

Edit: Oops, didn't see your response. Glad you figured it out.

-Max

[Anonymous]

Well just tried this again on my actual model and I get an error: Tool body creation failed. It seems when I choose the option "match shape" it fails for some reason. I attached a screencast.

https://knowledge.autodesk.com/community/screencast/e6b89f42-ae50-4f9a-a5e9-149648470fc5

[Anonymous]

Here is the link to the model I am working on

http://a360.co/1PJ5YPs

[mstrater]

Instead of choosing the sphere part as the match shape, try placing a point in a sketch at the place you want to extrude to and then use that as the match shape for the "extrude to" command.

You could also extrude by a specific distance and that should work too.

-Max

[Anonymous]

Thank you for your input. I have tried your suggestions but I still can't make it work. I attached a screencast but I suppose I must be doing something wrong. The lid is supposed to follow the curvature of the ring, so just plopping an extruded lid on top would give me a lip/edge which I dont want. I jus can't get my head around this one so again, thanks for any help.

[Anonymous · Accepted solution]

Well I tinkered a bit more with a new idea using Loft and that worked.

[jeff_strater]

Hi @Anonymous,

Loft works well, I agree.  Not meaning to pile on, but here are couple more options you can consider (for future reference):

1.  If you want the lid on top of your current model, you can just use Extrude, then a Split Body to trim away the unwanted piece of the extrude.  Like in this screencast:

2.  If you want the lid inside of your current model, it's even easier.  You can just Extrude downward, and choose Join.  In this case, the geometry just works out nicely

Jeff Strater (Fusion development)