Simulation for Geneva Cam assembly (Inventor 2016)

[Anonymous]

I'm trying to run a simulation of a geneva wheel rotating, but I'm having trouble with the driven dimension. The rotation constraint is set to be the angle between 2 planes. (one to track rotation of the cam, the other stationary.) I keep having several problems:

1. The simulation gets stuck as the pin enters the slot on the geneva wheel

2. The simulation gets stuck when the pin is deepest in the geneva wheel's slot

3. The rotation changes direction occasionally when the the angle between the planes goes through 0.

I've alreay made sure that there's adequate clearance between all the parts. (0.005 in clearance between all parts included in the contact solver) Anyone know how to make this work? I tried using the dynamic simulation, but it immediately rotated the geneva wheel to a position where it intersected the other wheel, and wouldn't let me move it back. Any help would be much appreciated.

Files and assembly are located here.

[TheCADWhisperer]

This is (relatively) simple to do - attach your assembly here and end all doubt.

[johnsonshiue · Accepted solution]

Hi! I have taken a look at this assembly. The behavior is indeed confusing. It is not clear to the user why the collision happens. I need to investigate it deeper to say it for sure. But, I think it has something to do with the assembly level work geometry you created there. This particular assembly is relatively straight forward. May I ask why you need those assembly work geometry (axes and planes)?

The presence of assembly work geometry actually makes the constraint system unnecessarily complicated. Let me explain why. The work geometry at assembly level is actually like an invisible component as opposed to fixed geometry in a part. The angular relationship among these Geneva components can be established directly. There is no need to create assembly work geometry. Generally, assembly work geometry is for creating assembly modeling features or there isn't a clear geometry for a component to be constrained. The confusion here is that the assembly work geometry is considered component, entitled to the same 6 degrees of freedom as any component in the same assembly. When solving the constraint, work geometry does participate in solving as other constraint participants. These invisible components introduce additional degrees of freedom unclear to the users. You can get a sense of what I am talking about by turning on the visibility of the assembly work geometry and suppressing Mate:24 for example. You will see the Geneva Rotation Plane would deviate from the axis when the index plate rotates. The mechanism still runs ok but the workplane becomes wild. This is what I meant by unnecessary degrees of freedom irrelevant to the assembly.

I am able to make this system work by simply deleting the assembly work geometry and create a driving angular constraint between the index plate's YZ plane and the global YZ plane. Please take a look and let me know if you have any question.

Many thanks!

[TheCADWhisperer]

1. Do not use Windows Explorer to rename files - the assembly links are broken when you do that.

2. The hole for your 10-32 UNF on the Geneva is much too large.  There will be no threads.  What is the correct tap drill size for a 10-32?

3. Be sure to download the latest Service Packs and Updates for your version of Inventor.

...back in a few minutes with corrected assembly.

[TheCADWhisperer]

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@Anonymous wrote:
....I've already made sure that there's adequate clearance between all the parts. (0.005 in clearance between all parts included in the contact solver)

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I do not see any clearance between the Bushing and the slots in the cam.  Both measure .2  now I have to wonder how many other errors I will find?

[TheCADWhisperer]

The attached will work by dragging with mouse, but -

it is better if you use only right click on the Drive This constraint and select Drive

or

better yet

go into Environments>Dynamic Simulation and play the simulation in that environment.

[WHolzwarth]

It's still hanging when driven in Assembly environment, Jeffrey.

IMO the issue is caused by placing the shafts only on workplanes or axes in 3D Space.

A common base brings it back to normal. 2016 fileset in Zip

Walter

[WHolzwarth]

In my treasure box I found a universal version based on VBA. Initial files were done with Inventor 6, now 2016

In Malteser.xls value a changes the size, value n sets the number of slots.

Have fun.

[JDMather]

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@WHolzwarth wrote:

It's still hanging when driven in Assembly environment, Jeffrey.

...

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It isn't hanging on my machine? (I didn't touch with mouse - it can be reset to home position by temporarily unsuppressing the two Home Position constraints.  I wonder why it hung on your machine?)

[WHolzwarth]

What happens if you set step size to more than 1 deg?

[JDMather]

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@WHolzwarth wrote:

In my treasure box ....

Have fun.

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My students have fun fixing this one from your treasure box every year.

[JDMather]

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@WHolzwarth wrote:

What happens if you set step size to more than 1 deg?

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Well, I'm not going to do that.  If I ran into trouble I would decrease step, not increase...  ... I'll just go over to Dynamic Simulation anyhow.  Not interesting in assembly environment....

[WHolzwarth]

Did you test it?

[Anonymous]

I deleted the planes and drove the rotation between the global YZ plane and the side of the keyway on the index plate, and that solved most of my problems. (I hadn't originally included the keyway, so I didn't have any vertical planes to base the angle on when first assembling, hence the work planes.) The only problem after changing that was that the animation would hang when the bushing was exiting the slot, but changing the increment from 1 degree to 2 degrees seems to have solved that. 

Thanks!

(Sorry for the bad file packaging, I'm still new to sharing Inventor files. Hope it didn't make things too difficult for you.)