PSD Input in certain direction

[karthik.mamudur]

Hello there,

I am trying to carryout random vibration analysis on a cab using Inventor Nastran. I did a modal analysis as a first step and followed it with a Random Response analysis. As part of Random response analysis, I would like to input my PSD in a certain direction (Say vertical direction =Y direction in my Cad model). I don't see an option to make sure that the PSD is applied in a certain direction when I go to Dynamic Setup => Random Analysis Option. Can you please help me out?

I am using Autodesk Inventor Nastran 2020 version on a Windows 10 Machine.

Thanks in advance,

Karthik

[John_Holtz]

Hi @karthik.mamudur 

You have applied a load to the model, or at least you are supposed to apply a load. The direction of the load determines the direction of the PSD.

For example, your PSD is in G^2/Hz (an acceleration PSD) or m^2/Hz (a displacement PSD). Therefore you need to apply an acceleration load or displacement to define the direction and magnitude for the PSD. In most cases, the load magnitude is not "1". For example, this forum post uses a PSD that is related to an 18.1G load, so the acceleration load = 18.1*9810 mm/sec^2. (See Re: PSD Random Vibration - Autodesk Community - Inventor Nastran)

See How to run a random response analysis with no outside loads in Nastran | Inventor Nastran | Autodesk... for more details about applying the load.

Let us know if you have any questions.

John

[karthik.mamudur]

Hello John,

Thank you for a quick reply. I don't have any loads in my model other than self weight. I am trying to study the effect of random ground excitation on the structure. So I would like to give a PSD representing the ground excitation in a certain direction. I know that Simulation mechanical had this feature in it, where in I can choose a direction for base excitation PSD. Is this available in Autodesk Nastran?

Thank you,

Karhtik

[John_Holtz]

Hi Karhtik,

You said the ground is moving. That is a load! You need to apply it to the model using the instructions in the article How to run a random response analysis with no outside loads in Nastran | Inventor Nastran | Autodesk.... The direction of the load determines the direction of the PSD.

John

[karthik.mamudur]

Hello John,

That helps. 2 last questions please, Instead of applying the enforced motion to all the nodes representing my supports, I will make a rigid connector and add the constraints only at the center node where the rigid connections meet (as indicated in that article). Question-1 I have is , do I need to run my modal analysis also with this same boundary condition? (I assume that it has to) but wanted to double check. 

Step 1: Modal analysis: With the rigid beams and center point constrained

Step 2: Duplicate modal analysis, change analysis type to Random response and input the PSD and then solve.

Is this correct?

Question 2: If I fix the center node in all the directions, then my PSD input will go in all those directions, is that correct? If I want my PSD just to act in the vertical direction, I need to pin my center node of the rigid connectors in the vertical direction and constrain at other locations to avoid rigid body motion and then run Response spectrum analysis.- Can you confirm if my understanding is correct?

Thank you agian,

Karthik

[John_Holtz]

Hi,

You are correct that the modal analysis and random response analysis need to be the same model (same mesh, same constraints, same connectors).

• By default, the random response analysis starts by performing a modal analysis so you only need one analysis if using the default setup. If the runtime is short, you do not need to do the modal analysis separately.
• If the runtime is long and you do not need to make changes to the mesh or constraints, then you can setup the analyses to run the modal analysis separately from the random response analysis.
• Did you setup the random response analysis to fetch the results from the modal analysis? If you did not do that, then the random response analysis is also solving for the natural frequencies, so you do not need to run the modal analysis separately.

You constrain the center of the rigid connector in all directions because (I assume) your model is connected to something (the ground, a building, another structure that you are not including in your model, and so on) that prevents your model from moving freely in all directions. In other words, the model moves with the ground in all 6 directions (X, Y, Z translation, X, Y, Z rotation). When you setup the analysis to simulate the ground moving in the X direction, the model follows in the X direction. Since you tell the analysis the ground does not move in Y and Z, the model does not move in the Y and Z.

You add an enforced motion to tell the analysis how the ground moves. If it moves in the X direction, you apply the enforced motion in the X direction. If the ground moves at a 30 degree angle to the X axis, you enter the X magnitude as 0.866 (=cos(30)) and the Y magnitude as 0.5 (=sin(30)). In other words, the enforced motion moves the constraints, and the constraints move the model.

The only thing the PSD does is tell the analysis how to scale the results.

• If the PSD data is in G's, you apply an enforced motion > Acceleration with a magnitude of 386.4 in/sec^2 or 9810 mm/sec^2 -- whatever the value of 1 G is in the units you are using.
• If the PSD is based on velocity, you use an enforced motion > velocity.
• If the PSD is based on displacement, you use an enforced motion > displacement.
• If the PSD is a force at some other location in the model other than the constraints, you apply the force to the model at the correct location. (One of the few times I have seen a load that was a force and not an acceleration is in the Inventor Nastran verification manual for the PSD analysis.)

The PSD only scales the results appropriately due to the load you apply. The PSD is not the load, and it does not indicate a direction.

John

[karthik.mamudur]

Hello John,

Thank you for a super detailed response. If I understood your response to my second question, you are saying that even if I plan to apply my PSD in one direction (say vertical direction -Y) , I should still constrain all the DOFs on my center node where all the rigid beams meat, but when I apply my enforced motion, I will apply it only in the Y direction. Please do me a favor and confirm it my understanding is correct.

I am analyzing a cab for vertical vibrations induced my the road, so I want to enforce my motion only in vertical direction and not in the other 5 DOF directions.

Thank you,

Karthik

[John_Holtz]

I have some additional explanation. So the answer is "yes" that the PSD load will only be applied in the vertical (-Y) direction. You need to determine how the cab (the parts being modeled) is restrained in real life (relative to the vehicle) and setup the rigid connector and constraint to simulate that condition.

Think of doing a laboratory vibration test on your cab. You weld or bolt the cab to the vibration test fixture, and the test fixture is vibrated in the vertical direction. Because the test fixture is not moving in the X or Z direction, because the fixture is relatively rigid, and because the cab is bolted/welded to the test fixture, the mounting location of the cab is rigidly "constrained" in the X and Z directions. In the analysis, you are modeling this by setting the rigid connector to be rigid in X and Z (and Y of course, the direction of the load), and the center of the connector is constrained in X, Y, Z to indicate the test fixture is not free to move in those directions relative to the test fixture. (The enforced motion load in Y is the same load that is moving the test fixture in the Y direction.)

In the real situation, the cab is mounted to the vehicle which may or may not be infinitely stiff. You assume the vehicle is rigid if you do not know the stiffness, and the connector and constraints on the cab model are simulating the rigidity of the vehicle. Any flexing in the X and Z directions is resisted by the vehicle and stiffness of the cab.

The opposite extreme is you assume the vehicle has 0 stiffness and therefore the mounting locations of the cab have zero resistance to motion in X and Z. Any flexing in the X and Z directions due to the vertical loading must be resisted entirely by the strength of the cab. You would need to uncheck the Tx and Tz directions for the rigid connector. Otherwise if the connector is rigid in X and Z, the mounting locations will be rigid. 

In summary, the different is like the difference in these frames. Which constraint is correct to get the appropriate displacement of the frame.

Sorry for the long explanation.

John

[karthik.mamudur]

Very helpful. Thank you!