3 Cones

Dennis_Varkevisser

Hello all! I'am trying to create a skeleton model for a bevel-gear drive. In this drive the centers of 2 outside gears lay on a plane. These gears are fixed in position. Now I want to model the in-between gear that has to be tangent to both other gears. I modeled the 2 outside bevel gears as cones. The center of the cones are at the same position.
How do I model this in-between gear correctly? I tried to model and to assemble, failed to achieve one of them. (Modeling has the preference)
I can use Solidworks to model this using the 3D curve functionality, but I want to be able to solve this puzzle in Onshape. Hope someone can help me.

Best regards,
Dennis Varkevisser

steve_shubin

I added 2 Mirror features to get this

steve_shubin

@Dennis_Varkevisser

is this what you’re looking for?

What you see in the animated GIF was done with one sketch, which I would consider your skeleton, and three revolves

Dennis_Varkevisser

Hello Steve,

Thanks for the reply, my target is more difficult: the in-between cone needs to be able to increase in size such that the center  line of the in-between cone is not on the same plane as the other two cones anymore. Sorry for not making that clear in my original question.

steve_shubin

@Dennis_Varkevisser

If you let us know where you want that middle cone, somebody here in the forum will likely be able to help you out

EvanReese

if you've got an example of one you did in Solidworks that would help a lot. I can't exactly picture your goal from the description.

steve_shubin

@Dennis_Varkevisser

OK I think I got it. Hopefully I’ll be able to lessen the amount of steps overtime. But if nothing else, this is one way of doing it

https://cad.onshape.com/documents/b24a091be9a8a4e172e7c911/w/9bec6a351383876a4ee4016c/e/52c3763c9c99b731f6878081

steve_shubin

@Dennis_Varkevisser

OK in the ABOVE POST, I added one more feature to the document. And that was an interference checking feature.

In the GIF below you could see how I use it to make sure there is no interference from one part to the other

By playing with Sketches 2 & 3 you can adjust the size of that middle cone. But make sure you unsuppress the interference check feature when you adjust these sketches so you could see whether or not things are intersecting

Sorry I couldn’t make it more automatic but that’s the best I could come up with right now

steve_shubin

Dennis_Varkevisser

Okay Steve that's a smart solution, I did not get so far myself. With some goniometrics it should be possible to calculate the correct angles. But after some rough sketches all the tangens, cosinus and arc-sinuses made me dizzy.

Dennis_Varkevisser

Hereby some info about my Solidworks approach: 

This is the parametric assembly.
The centerlines of the green gears are all in one plane. There centerlines cross at the same point. The centerline positions of the green gears are fixed by the rest of the construction (that I kept invisible…)
The grey gears are in between the green gears and their positions are determined by their diameters and the fact that their center points (at the tip of their cones) are at the same position as the center points of the green gear cones.

Here the skeleton that steers all gears. The skeleton does not cover the green and grey gear on the right, these are mirrored.

Now it becomes difficult (to explain)  
The green lines are the center lines of the 3 gears (cones) the middle one starts floating and is for the grey gear.
The yellow line start in the green gear centers at the working plane of the gears. The lines lay on the working plane of the green gears. The line ends are connected.
The intersection of the yellow lines is then attached to the center line of the grey gear.
Then the 2 blue lines are made. They are both equal length (= radius of grey gear)
They are both perpendicular to the centerline of the grey gear
They are both intersecting the yellow lines and the running circles of the green gears.
This is all done with the SW 3D sketch functionality were you can relate the sketch to all sorts of references. It is a quite tricky feature...
With this skeleton I am able to design correct bevel gears that are parametric. 

This is what I would like to acheive with Onshape….
Hope you understand the above, if not: let me know!

john_mcclary

ooh, pretty

steve_shubin

@Dennis_Varkevisser

I think this is what you’re looking for

When you started getting into it real heavy, I really didn’t read that too much

The greens are all in line
The grays and the center green are in line
The greens are all the same size
The grays are the same size

Is this what you’re looking for?

https://cad.onshape.com/documents/8101415e1cb68ef774dd577b/w/fff5edb604a74c6e07d8a325/e/5aaf4cf5de8343616e1ae87c

steve_shubin

I added 2 Mirror features to get this

Dennis_Varkevisser

looks nice Steve! Thanks for your efforts!!

steve_shubin

@Dennis_Varkevisser

Thanks Dennis !
It was my pleasure 

Fun to work on

steve_shubin

@Dennis_Varkevisser

There is one quirk

So with the cones, you want symmetry. That means you want the degree measurement on Sketch 2 to be the same as Sketch 3. But with the Interference Check FeatureScript unsuppressed, when you set both sketches to the same exact degree, for some reason, the gray cone goes away.

I don’t think it’s because of the way I set things up in the document. It’s possible. But I think it might have to do with some kind of a quirk in the way the Interference Check FeatureScript works. And I say this because I can set Sketch 3 to 56°, and I can set Sketch 2 to a fraction above or below 56°, either 56.053° or 55.947°, and everything will work fine. But if I set Sketch 2 to exactly the same as Sketch 3, the gray cone goes away

So what I do is this. With the interference check feature unsuppressed, I dial the two sketches in where they are as close to one another as possible, without there being any interference. For example, if I set Sketch 3 to 56°, then I set Sketch 2 to 56.053°. Now if the gray cone is still visible when I do this, then I would suppress the interference check feature and just set them both to 56°. Because in all likelihood, it’s probably gonna work out good if you fab these parts.

But if somebody out there has an explanation why this is, let me know

steve_shubin

@Dennis_Varkevisser


https://cad.onshape.com/documents/44a0344350e680a82edc9f85/w/d9b3cea07c05b952f838cdb1/e/191f386072a96fe2c6dad268

NO QUIRKS IN A SIMPLER DESKTOP VERSION 

I do most things in Onshape on my iPhone. This 3 Cones document I did on my iPhone. As such, I used what was available to me in the mobile app for version 2, one of those tools being the interference detection FeatureScript — as the mobile app does not have any native interference detection

But — about 15 minutes ago, it popped into my mind that the desktop version of Onshape does have interference detection built-in as a native function

So now, using Onshape’s browser version — I’ve made a version 3 document that relies upon the user engaging Onshape’s built-in interference detection, instead of the interference detection FeatureScript.

Using the built-in interference detection, I verified that using symmetry across Sketches 2 & 3 would give the results desired. And there was no odd behavior with this built-in interference detection, such as detailed in the post directly above

Nonetheless, I’m going to keep both the version 2 doc and version 3 doc so that those that only use an iPhone will have access to this tangent cones document, if they want (without having to rely on the desktop version)

So in this latest version — version 3 — I put a variable in that automatically enters the dimensions into Sketches 2 & 3. And then the only other thing you have to adjust is Sketch 1