Fatigue study based on motion-loads from Inventor Dynamic Simulation

[Anonymous]

Hi there,

This is my first post, so I hope, I get this right. I'm a little stuck at a project including dynamic simulation and Nastran-In-CAD.

To illustrate my problem, I've created a little demo assembly that is a simplified 2D-represenation of the real problem.

In the assembly there is a rotating wheel (component: TDS01_Rad) with a non-round geometry. It has one degree of freedom that in dynamic simulation is driven via an imposed motion at 35 degree/sec.

The second part of the assembly is a beam (component: TDS01_Hebel) that is fixed at one end with one rotational degree of freedom.

At the other end a small pulley (component: TDS01_Rolle) is attached which can freely rotate around its pivot pin. (The decal is only for visual feedback of the happening motion)

In the Dynamic Simulation Environment gravity pulls the beam toward the wheel while the geometry of the wheel ensures that the beam is catapulted in the air again resulting in a cyclic event.

I'd like to create a fatigue study in Nastran-In-CAD that analyses effects on the beam after a certain number of cycles.

I'm struggling to create the time-dependent loads in Nastran.

In the past I already created fatigue studies with simple loads, where it was possible to input the desired data manually, but especially the real assembly is far more complex.

I'm able to export timesteps to the Stress Analysis Environment and open the generated loads in Nastran, but I don't know how to set up the fatigue study loads.

Here is a screenshot of my assembly:

 

Please see the attached files for further clarification.

Help is really appreciated.

--Mark

[John_Holtz]

Hi @Anonymous

Since a fatigue analysis (at least in In-CAD) is based on a static analysis, you need to find an alternate way to do your fatigue calculation. You cannot perform a transient/dynamic analysis to use in a fatigue analysis.

Some situations can be analyzed as a static analysis, and the static results are cycled using a "load curve". This is what In-CAD's Multi-Axial fatigue does. (Vibration fatigue uses a random response analysis which could be considered as a dynamic analysis, but not a time dependent analysis like you are asking.) In your situation, you may be able to create a static analysis that duplicates the peak load from the transient analysis. Then the load curve cycles the load from 0 to max to 0 for the fatigue analysis (or whatever the results curve looks like).

An alternative to perform a nonlinear transient response analysis to capture the large displacement results (caused by the rotation) and time dependent results. From the peak results, you can then do a hand calculation for the fatigue life.

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Hi @John_Holtz,

Thanks for the fast reply and clarifying the static character of the fatigue study. I totally forgot about that. Doing the fatigue calculation at hand seems to be the way to go.

I’m now going to create a nonlinear transient response analysis to determine the peak results, like you mentioned in your post. For now, I simply used the “Enforced Motion” to describe the movement of the wheel, but got to know that it isn’t available in nonlinear transient response.
So I’m asking myself which of the following approaches is better:
I. Using Dynamic Simulation inside Inventor Professional to log a load curve and copy-paste it to the Nastran In-CAD study for the specific component where I used enforced motion before?
II. Creating the load curve by a subcase with a different study and enforced motion?

--Mark

[John_Holtz · Accepted solution]

Hi @Anonymous

What part is failing in fatigue? What action is causing the fatigue? I would think the rotation of the wheel does not generate any significant stress, so there is no need to simulate the rotation. The only stress-inducing event that I see is the impact of the beam and pulley. In this case, you can perform a transient analysis where the beam/pulley has an initial velocity and gravity and it impacts the wheel.

From the stress that is generated, you can try to reproduce that stress distribution in a static stress analysis of the beam and pulley. If that can be done, that is the load that you apply in a fatigue analysis, and the results cycle from 0 to maximum to 0.

[Anonymous]

Hi @John_Holtz,

That sounds perfectly clear to me.
I'm going to model the impact like this.
Thank you very much for your help!

--Mark