I have a funnel with a curved top. I'm trying to project an inset of the border onto the curved surface and use the shell command to create a hollow funnel with an overhanging lip. I have projected the inset successfully, but cannot select the resulting smaller face, just the whole original face.
A similar problem that I tried while attempting to figure this out was shelling a sphere. 2d sketch -> 3d sketch project onto surface, and try applying shell to the resulting "face". However I can only select the whole face when trying to shell.
Hope this was clear, please let me know if i can explain further or add pictures!
Solved! Go to Solution.
Yeah, you lost me. Can you attach a pic of your finished product please, and maybe where you're up to so far?
For the sphere pick sphere from the primitives, pick one of the origin planes, pick the origin, pick a point on the sphere. This will give you a sketch that is a center point circle with a center line and automaticly revolves it a full 360 degrees. Then pick the revolution you just craeated from the browser, set the thickness you want the wall to be and check ok. Done!!! You can go back to the revolution sketch and dimeinsion the diamiter you want the sphere to be.
Hi and welcome to the forum!
It's hard to tell from your description exactly what you are trying to do, but my first guess is that splitting the face might be what you want to do. I'll second robmatthew's suggestion for posting a picture. Or better yet, can you post your file?
Until then, keep in mind that it isn't necessary to pick a face for the shell command. For a sphere, just start the shell command, specify the thickness and direction, then click OK. No need to pick a face. See the attached file (Inventor 2014) for an example.
Edit: I have also attached an example that demonstrates using the split tool.
Thanks for the responses, I'm checking out your split example now. I'm attaching a couple of picture to clarify what I'm trying to do.
The first is from Inventor, and it shows the projected 3d sketch on the surface of the sphere and the top of the funnel. I've got the shell command selected, and I can only choose the entire sphere or curved surface when selecting the 'face' I've created.
The second picture is a cutaway sketch of the profile I'm trying to achieve with the funnel.
1. I cannot tell from your image what version of Inventor you are using (it would be far far better to attach ipt file here).
2. It doesn't appear that you ever Split your face.
3. You don't need a 3D sketch to Split your face.
4. If you have tangent faces be sure to turn off tangent selection of faces (I think this is version specific).
Maybe something like attached is what you are after?
OK, thanks for posting the pictures. The split tool is what you need. Take a close look at the file JD posted. Go through it step by step from start to finish--there's a lot to be learned from the techniques he used to create that example.
As for shelling the part, JD mentioned this:
4. If you have tangent faces be sure to turn off tangent selection of faces
I struggled with this myself for a minute or two when I was creating the sphere example. I couldn't get the shell tool to pick the split surface--it just wanted to pick the entire surface. The option JD mentioned is called Automatic Face Chain (at least, that's what it's called in 2014):
This option has to be off, otherwise it will pick every surface that is tangent to the one you want.
Here is another example that has a tangent edge.
And another example....
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