How to construct this feature.

[pbreed]

I'm trying to convert from using Rhino to Fusion 360. I can't seem to build this part...
Here is how I would build it in Rhino.
Simple Cylinder with holeDraw o-ring fgorve dimensionsCreate two spheres that intersect the edges of the oring gove and the center of th holeNow create a curve from the intersection of the shpere and the cylindernow sweep (2 rails) the profileSubtract theat shape and my pring grove is correctly sized and correctly perpindicular to my cyyliner face all the way around.

I have three Fusion problems...https://a360.co/2Lhvter
1)I Can't seem to draw the spheres based on features, only on dimensions.
Its easy to get the center of the spheres right, but I'd like to draw the sphere from the center to a point on my  oring grove.

2)I can do the math/trig and get the sphere dimension, alas even after drawing the sphere I can't generate a curve of the cylinder/sphere intersection.

3)I believe (bbut do not know) that once I create the curves I can sweep my o-ring grove.

Help...

[HughesTooling · Accepted solution]

Here's a screencast of something similar using only 1 sphere. Bit of advise, don't waste time trying to use the primitives just use sketches and revolves. I've attached my file, in the future export your design and attach, the share links are more trouble and you'll get help quicker if the file's attached.

Mark

[g-andresen]

Hi,

here is another way to do it.

The only difference is that the groove is not conical, but i think, the ring will fit better in a non conical groove.

günther

[pbreed]

Ok doing the subtraction from the sphere works just fine.
Now I have an edge I can sweep, and doing it with both spheres allows me to sweep a rail and a guide, doign exactly what I needed.

I have a way to build what I want...
Having to do the trigonometry for the 2nd sphere rather than just pick a point is a pain... but its at least possible.

[pbreed]

The problem with the 2nd here  approach is the depth of the o-ring grove is not constant,so
the o-ring will not make proper contact with the outside cylinder this sits in.
If you increase the diameter of the hole with respect to the cylinder you will see the limitations of this approach...

[HughesTooling]

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@pbreed wrote:

Having to do the trigonometry for the 2nd sphere rather than just pick a point is a pain... but its at least possible.

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Why do you have to do the trig? Can't you project references and sketch what you need?

Mark

[pbreed]

The only constructor for a sphere is a point and a diameter.
In your example you drew a half circle and did a revolve, so  that probably works without doing the trig.
I'm new to this and completely lost on how to tie one sketch to another, its easy if your object has planar surfaces, but on non planar objects I'm lost. (I just reference everything back to the origin)
I'll try to do some review of this process today...

[HughesTooling]

@pbreed Are both spheres on the same centre point?

Take a look this screencast where I create a hollow sphere, file's attached as well.

Mark

[HughesTooling]

Here's another idea using Split Face and Press Pull then chamfer. Note Chamfer, Distance and Angle doesn't let you choose the direction so in the screencast one chamfer is down the groove and the other is along the face of the cylinder!  I've come across this problem with a couple of other CAD programs as well, don't know why the programmers are blind to this shortcoming. File for this version attached as well. By the way how are you manufacturing this part?

Mark

[pbreed]

I went back this morning, watched some sketch tutorials,
Then rebuild the concept using projected points into the construction plane for the o-ring grove dimensions, and 
Hughes tool's idea of drawing a semi-circle and revolving to get the sphere rather than the sphere command...

And now I have a fully parametric driven version of this. I can change the o-ring series, the cylinder diameter, the hole diameter and  everything recalculates correctly.
I did the original in Rhino in about 3 min, the last incantation in Fusion only took me an hour
I still think the drawing constraint (pretzel generation tool) solver is evil, but I can usually beat it into submission...

[pbreed]

How am I making the part....
This feature is part of a much more complicated part...

Prototype for fit and assembly I will prototype on my Form 2.

I've had a part with similar features printed in DMLS aluminum in the past.
Hand polishing out all the rough to make sealing surfaces was a pain.
Most of what I build is tiny and intricate.
I have a Tormach CNC mill with 4th axis, alas this is a 5 axis part.
I've ordered a pocketnc  small 5 axis machine, supposed to arrive in early January.
My guess is that will be the fab solution of choice for things needing 5 axis. 
(I also have a 13x40 Chinese lathe I converted to CNC by replacing axis acme screws with ball screws  and driven by  Mach 3)

I keep lusting after a Haas MiniMill with TRT100 its just a bridge too far at this moment.

[chrisplyler]

Five minutes, max.

In reading this thread, I have seen versions utilizing a sphere, and versions that just extrude, project, or otherwise develop a circle onto the surface of the cylinder. You should be aware that although the results look very similar, they produce slightly different geometries. Depending upon your application, it might be important to pick one method over the other.

Here is the sphere version: