Wrapping a Sphere

kevin_wood958

Hello! 

First time posting, but have visited the forum for many solutions in the past. Kind of at a loss here. Forgive me, as I'm all self-taught with CAD. So I may not give the best technical description of what I'm trying to achieve. 

In short, I want to wrap a drawing around a sphere (series of small circles). With the ultimate goal of being able to use those circles to locate holes in the sphere (which will also be hollow). 

I was kind of able to accomplish this by creating a two cylinders around the sphere. Wrapping the sketch and extruding the circles. Then used the replace face feature to mate them with the sphere's surface. The main problem with this is that any of the circles (holes) that aren't along the center line of the cylinder were distorted.

I did some digging, and was able to find a "Project" feature script. And while this projected the circles exactly as I'd want them. There was nothing I could do in respect to creating holes in the sphere with them. 

Again, I apologize if I'm not describing this in the best way I can. Below is an image of the sphere and associated sketch I wish to wrap around it for locating each hole. 

Thanks in advance!

EvanReese

See this thread, which could be relevant: https://forum.onshape.com/discussion/comment/73949#Comment_73949

If your end result will be clustered circles like that, you could probably just sketch them on the top/right/front planes and use extrude to cut them out of a hollow sphere like so. You'll still get a little bit of distortion around the outer holes. If that's a problem, let me know and I have another idea that's more complex.

EvanReese

Ah I can't help myself, here's the other example. I placed spheres onto the main sphere, then split the main sphere face with them followed by a shell feature. Since it looks like your patterns are on a 3x3 grid, I just added all of those spheres, and choose which ones to include in the split feature. The nice thing about this is you don't get any distortion from projecting them with Extrude. Here's the studio https://cad.onshape.com/documents/8ed5ffc34d5e855c9126e3d6/w/6543b4bf04d0747b74ac6954/e/d7fd5fae81ddfdbdff28e92e

kevin_wood958

Evan_Reese said:

Ah I can't help myself, here's the other example. I placed spheres onto the main sphere, then split the main sphere face with them followed by a shell feature. Since it looks like your patterns are on a 3x3 grid, I just added all of those spheres, and choose which ones to include in the split feature. The nice thing about this is you don't get any distortion from projecting them with Extrude. Here's the studio https://cad.onshape.com/documents/8ed5ffc34d5e855c9126e3d6/w/6543b4bf04d0747b74ac6954/e/d7fd5fae81ddfdbdff28e92e

Thank you! Played around with this solution in the linked file (learned some new skills in the process). It wasn't the perfect solution, as the placement of each hole needs to be very precise (each "cluster" is unique and oriented in a very specific location). So trying to dial in the Vertices U and V Parameters for each 3d point was very difficult to do with any degree of precision. 

However, walking through your solution led me to a massive "ah ha" realization. Which is that I could use projected curves (the circles in my drawing) to split a face of a solid. And could then thicken (remove) those projected curves from the solid. With this approach, dialing in the precise size and placement of each "hole" was incredibly easy. 

The summary of what I did is as follows...

1. Revolved a sphere (now realize there's a feature script for this)
2. Created a plane (oriented to where it was touching the edge of the sphere)
3. Made my drawing of the circles (future holes)
4. Extruded a surface (equal diameter to the sphere) on both the X and Y axis
5. Wrapped my drawing around the surface on each respective axis
6. Used the Project FS to project the wrapped drawing (curves) onto the sphere
7. Split the face of the sphere with the projected curves (circles/holes)
8. Created the sphere's shell
9. Used Thicken to remove the holes from the sphere

Hope that makes sense. I owe you a big thank you. As without realizing I could use projected curves to split the surface of a solid, I would have never figured out this solution. With your help and insight, I now have a sphere with the perfectly concentric holes located in precisely all the right places.

EvanReese

Awesome! glad it helped. Unless you're projecting the circles normal to the sphere, the edges will still get a little bit distorted (become slightly ellipse-like, not circles). I added a second tab in the same doc showing how you might address this if you care to. https://cad.onshape.com/documents/8ed5ffc34d5e855c9126e3d6/w/6543b4bf04d0747b74ac6954/e/e29a588018adca7981e91cf6

kevin_wood958

Evan_Reese said:

Awesome! glad it helped. Unless you're projecting the circles normal to the sphere, the edges will still get a little bit distorted (become slightly ellipse-like, not circles). I added a second tab in the same doc showing how you might address this if you care to. https://cad.onshape.com/documents/8ed5ffc34d5e855c9126e3d6/w/6543b4bf04d0747b74ac6954/e/e29a588018adca7981e91cf6

@Evan_Reese

You're correct that a couple of the "holes" are ever so slightly distorted. Appears to be happening with those that are the farthest "off-axis" (if that makes sense). Will play around with this other solution and appreciate the continued effort to help!

If you're curious, my doc is linked below.

https://cad.onshape.com/documents/bec6cbc241c72af010485e4b/w/6a936f53ee01b59e51ffb197/e/690583d0382fb20f4b3b68b6

The first tab is the projected holes method that I just figured out how to achieve. Thanks to the "ah ha" moment you provided where I learned I could split the face of the solid with the surface of the curves.

The second tab was a far more intensive model I did prior to posting the question. Same idea of wrapping the sphere with the drawings. But I instead created T Planes at every single dot/hole. Then drew a circle on the plane (appropriately sized and located). Then extruded it through the solid. Took quite a bit more time to do, but yielded good results.

EvanReese

Sure thing! I like this stuff. What you're doing on the second one seems like it'll work to limit distortion. With mine I'm essentially using a workaround to project the hole centers onto the main sphere, then using a smaller sphere at that center point to intersect with the big one (the intersection of spheres is a perfect circle).

kevin_wood958

Evan_Reese said:

Sure thing! I like this stuff. What you're doing on the second one seems like it'll work to limit distortion. With mine I'm essentially using a workaround to project the hole centers onto the main sphere, then using a smaller sphere at that center point to intersect with the big one (the intersection of spheres is a perfect circle).

I enjoy it as well. Professionally, the work I do is entirely unrelated to design. So learning CAD has been a fun little side quest. And appreciate the help from the community!

Agreed that my second one is the most accurate in terms of what I set out to achieve. Just seemed like a "clunky" solution. And I figured there might be an easier way (or at least more technically sound). Projecting the hole centers was a great idea, and I've been playing around with it.

Fortunately, this is likely a "one and done" design once I have it dialed in. But still doesn't hurt to learn something new that'll come in handy with future designs.

joseph_ennis277

something I made that might help
https://cad.onshape.com/documents/d4802c4822b36e36ded605a5/w/7adffde7b4c9ee5db953f945/e/a3211e0f84444c4c91a490fc
the idea is I condense the sketch on 2 cylinders and then use a ruled surface to bring it onto the sphere and remove anything sticking out