Beam elements elongating unexpectedly in Dynamic Response 3D

barrti

Greetings
I am continuing to explore the capabilities of Mecway using Dynamic response 3D as well as constraint equations.
This is useful of course to model mechanisms, inertias etc.

I have uploaded a very simple model which is the beginnings of a simple car differential. It uses three line2 beam elements for two axles with 100mm long pieces on the ends whose purpose is simply to indicate rotation. There is a similar input shaft which constitutes the third line2 beam element.

I have use a single constraint equation 0=1(1/rad)xrz8 + 4(1/rad)xrx7 to link node 8 to node 7.

This does indeed give a 4:1 reduction from the input shaft to the LHS axle so that bit works.

I have applied a 1Nm moment to the input drive shaft with an inertia applied to it as well.

When one views the results, two of the beam elements extend way beyond what one would expect at such low angular velocities. They should not do this as they are beam elements with suitable properties (Steel, E=200 GPa etc).

What seems to be happening is that the z coordinate is being maintained but as the beams rotate, the x&Y coordinates extend to maintain a constant Z coordinate.

I have noticed this tendancy before.

How can we prevent this?

barrti

Victor

Since it's a linear analysis, rotation angles have to be small. Under this small angle assumption, rotation of a mesh is really a linear translation of each node in the direction tangent to its circular path. If the angle is bigger, then the translation distance is bigger too but it's still only moving in a straight line.

Since those translating nodes are only for display, I suspect it's probably harmless but be careful not to use those extra beams to drive something. The rotation of the shafts about their axes that's described by the rotational DOFs can be greater because it's a "proper" rotation, not just a translation.

barrti

Victor
Thanks for that. I guess I should also be using ccx with nonlinear dynamic analysis because I will be using large deflections. Recently I got an unconstrained rotating link to rotate with a very light spring.
Tim

DaveStupple

I am puzzled by the rotational inertia constraint about the x-axis. What does this simulate? I have tried suppressing it. or increasing it, but I haven't spotted the effect it has. Keep it simple for me!

barrti

Hi Dave,
This model is really a very simple trial model just to explore if I can use this software for modelling rotational shafting systems with inertias and the like eg a motor with a reduction drive, a coupling and a large flywheel.

In this model of a car differential, I have a shaft on the z-axis driving a shaft on the x-axis via a constraint equation. Since the beam elements are massless in this case (If I remember correctly), I simply added a rotational inertia to represent the inertia of the shaft. I did this so that the angular acceleration would be finite and measurable.
Actually, I should have just allowed the beam elements to have density and the inertia would have been automatically modelled.

This model is really incomplete - sorry if it is confusing!

If I were to complete this model, I would add rotational inertia to the other shafts and also at the end of the "axles" to represent the inertia of the wheels.

These nodal inertias are a very cool and simple way of adding the effect of a flywheel without actually creating the mesh for it by using say solid elements etc.

I don't remember the magnitudes of the torques and inertias, but because I was having trouble with the link extending as Victor described above, I stopped working on it.

If, you wanted to check out the validity, you would have to use the T=I x alpha equation and check the magnitude of the angular acceleration of the shafting.

Now that I've written all of that, I reloaded it and I see why u asked those questions! Sorry!

I too do not see a change in the Angular Velocity Z if I click on a node - no matter what I do to the magnitude of the inertia or input torque!?

What are we missing Victor?

DaveStupple

Thanks for that. I initially assumed it was to give the rotation some resistance, but then I noticed the inertia was applied for an x-axis. So maybe you should apply it for the z-axis? I tried this and got a kind of sinusoidal pattern on the rotation. I was thinking that the reason the shaft resisted infinitely fast rotation with no inertia applied to z, was that the shaft (and its indicator rod) has density, and hence some inertia.

DaveStupple

If I leave the inertia on the x-axis, and set the material density to 0, the solver fails, presumably because there is no resistance to the moment, as you predicted. Makes sense.

Victor

Yes, all correct. It looks like it should be on the Z-axis to have any effect because there's no rotation about the X-axis. And yes, the massive beam elements have their own rotational inertia which allows it to solve. Otherwise "I" would be zero in T=I*alpha. Even if it's connected to the point rotational inertia by an elastic element ( T=I*alpha + k*theta ), it still wouldn't be able to solve that because theta should change instantaneously in response to an applied torque.

barrti

Aha! Thanks Victor. I missed the fact that I needed to specify the correct axis for the inertia. I never did get around to finishing the model. The model now seems to be doing what you'd expect.

Cheers