Optistruct/Nastran Transient Response - Wing simulation

[IngCane]

Hi guys.

I'm trying to solve the following issue: we have a racecar with a rear wing, whose supports fail (or crack) after few races. The static analysis didn't show any problem, so it's evidently a fatigue issue. We have accelerometers in the car, bonded just next to the wing support's attachments to the chassis.

To solve this, I'm running a Direct Transient Analysis on the wing's structure, where the applied load is an imposed acceleration (the accelerometer's reading) to its attachments to the chassis, in order to get the stress time history and later perform a durability analysis.
The problem with this strategy, is that I get very large displacements (in the order of thousands of meters - as wide as the racetrack) and I'm not sure that I can really trust the analysis.

So I was wondering how would you deal with a problem like this, or if you know any simulation technique well suited for such type of problems?

Thanks all for reading

 

[ThomasH]

Hi

I don't know how you have done the analysis exactly but if I speculate a little.

You have your structure, the wing. At the support you can introduce a large mass and then make a time-dependent force. By using a simple F = m * a you can get the correct acceleration as function of time. Does that, more or less, sum up your approach?

Since you move the support to get the correct accelerations the displacements will be meaningless. But the stresses can be correct.

You can also do a response spectra analysis and move from time-domain to frequency-domain. Then I think you can get meaningful results for both stresses and displacements. There may also be a possibility to get the displacements relative to the support node and not in a global coordinate system. But I don't remember how to do that. I am not even sure that it is possible.
But if you look at this as a seismic analysis with the vehicle being the moving ground I think you can find some tips on how to approach the problem.

Also, when you say the static analysis does not show any problem. What loading do you use for the static analysis?

Anyway, I hope this helps a little.

Thomas

 

[Zadrobu]

Hmmm, it might be that the accuracy of stress solutions starts to suffer due to numerical round-off errors when the difference between the displacements and the dimensions of the structure becomes really too large. I don't know though how large exactly the difference has to be before these errors become significant.

What you could do is analyze the wing within a moving reference frame instead of within an earth-fixed reference frame. This eliminates the rigid-body motion from the displacement solutions. Then you would be on the safe side regarding numerical accuracy. Additionally it could also make some other post-processing tasks (e.g. checking structural deformations) easier.

To accomplish this in Nastran: fix the support point(s) of your wing with SPC (single-point-constraints) and apply the accelerations with GRAV (gravity loading).

 

[IngCane]

Thanks for your replies.
As ThomasH was correctly saying, there's actually a command that make Nastran calculate everything in a relative coordinate system, rather than absolute, and this solved my problem.

FYI see PARAM, ENFMOTN, REL
It only works with the modal transient (not direct) analysis.

Thanks both.