create holes in a hollow sphere?

[bdg215]

Hi there. I have an 8" hollow sphere with a 3mm thick shell. There are holes all over the sphere already which I created by plotting them all, one by one. This wasn't too hard because I already had the pattern recorded, and the math was basically just a translation. Now I have to go back and put 3-4 square holes between some of the existing holes in specific places, and the holes have to be perfectly tangent to the surface of the sphere. (so that square objects would fit straight into the holes. It would take and enormous amount of time and effort to plot the square holes in Matlab and then input them on my model like I did the existing hole pattern. Is there any way at all that I can take care of this with the tools in Fusion 360? The one saving grace of the new holes is that they don't have to be *perfectly* placed like the initial holes do. They just have to be roughly spaced evenly between existing holes, grouped around the "bottom" of my model. They do have to be straight (tangent) to the sphere though. I included a little snapshot of the sphere and some holes to aid in the mental picture. You then just have to imagine that I will need some square holes in specific spots between those holes towards one end of the sphere.

[jhackney1972]

I am assuming you have the Fusion 360 model or are you just showing us a pretty picture?  If you do, please attach the model to your question so others can give you the best solution.

[jhackney1972]

While I wait for you model to be posted, I did a quick screencast showing the cutting of square holes in a sphere.  The holes are cut, as you asked, so a square pin would slide right in.  I then pattern the square hole to create multiple cutouts.  If you need cutouts on different orientations, it is just a matter of creating the original sketch plane where you need it.  Take a look at the screencast.  Model is attached.

[bdg215]

Hi jhackney, thanks for the reply!

I think you might be on to a solution, but I'm still not sure how I would place the squares between existing holes, I am going to include a version of the sphere with just some holes on it just so you can see basically what I'm going for. I placed those holes with a plugin that let's you input point from x,y,z coordinates. That was how I got planes tangent to the sphere, and then cut these holes. I can see how your method can get the squares tangent, but as is, it is limited to the six directions from o,o,o. In order for this to work, I have to get the tangent planes to occur between the existing holes. Perhaps there is a way for me to rotate the plane from the origin?

[davebYYPCU]

Just as you had points for the round holes, you will need another set of points for the square holes.

[jhackney1972]

I cannot find any pattern to your existing holes in the attached model.  So I am going to have to agree with @davebYYPCU you will have to find the centers of your square cutouts using the same method you did with your holes, by plotting points.

[bdg215]

I figured out how to do this with some help on the fusion 360 reddit page.

If anyone comes looking for an answer, then what I did was to create a plane through three points using two adjacent holes and the origin, which is the center of the sphere. I then traced an arc on the sphere between the two points i chose for the plane and put a sketch point between them. (using center point arc and choosing the origin as the center) Then, I created a plane tangent to the surface of the sphere at that point, created a center rectangle sketch on it, created an axis through the origin and the sketch point, rotated the rectangular sketch to the position i needed it in, and cut it out.

best, 

[jasonhomrighaus]

Perhaps a little simpler approach would be to create a sketch of the rectangle profile centered at the origin then create a new body that extends beyond the sphere, then use move to rotate the sphere about the origin to the desired position of the hole which will be visible.  Then combine/Cut while saving your tool.  Then just move sphere to next location and repeat.

[etfrench]

@jasonhomrighaus: Moves are expensive in terms of Fusion 360's compute routine and should be avoided.

@bdg215:  Your workflow seems to have a few unnecessary steps: Creating an axis and rotating the sketch.  It would also have been much simpler to create the square holes if you had not deleted the sketches for the round holes.  Since you didn't say what the rules were for orienting the square holes, I showed two methods in the screencast.

[jasonhomrighaus]

that really depends on what your trying to accomplish. It may add some time on compute but is a lot faster and quicker in people time and can be done in three steps, most other methods require considerably more than that.

[jasonhomrighaus]

As a point of comparison Here is my method

It takes 5 commands to execute

it takes 2 min or less of people times less than 1 minute per hole.

Your method as shown took 5.6 min and required 40 Commands to execute.  So i guess my question is

"What are we saving by avoiding a move for such a simple requirement to place a rectangular hole in an approximate area around a sphere?"

[Anonymous]

Hello, this solves 90% of the issue I ran into.  I have a pattern of 5mm holes going through my hollow sphere.  Now I need to extrude to the inside a 3 mm hollow tube having an I.D. of 5 mm and an O.D. of 8 mm.  These extrusions are for the LEDs to sit in.  I feel like I am missing something so basic but as a beginner I am not sure what that is.  Thank you.

[laughingcreek]

I think you would be better served starting a new post, along with attaching your file and some pics explaining what your wanting to do.

[bdg215]

I think the other comment is correct, it's best to start your own thread, and you should be prepared to upload the model so they can help you.

I would try, but I'm not in front of the PC I run fusion on recently and can't work through it in my head.

[jasonhomrighaus]

One quick option is to use a shell command to create a hollowed shell.  To do this adjust the thickness of your sphere to the an amount that is greater than the length you want for the standoffs 

Next use the shell command on the inside surface and select a 3mm wall thickness.  this will hollow out the sphere leaving a shell with your standoffs.  Then you can adjust the outside wall thickness using press pull.