Modal analysis underwater 1

[oscar1057]

Hi everybody

I'm a little bit lost with a problem...
Does anyone know how to perform a modal analysis of a structure (3D) which is in a vessel full of water.
I have already tried several times but it does not find any logical solution, I tried before to perform the modal analysis in a "dry environment" which gave me really accurated solutions - checked experimentally in the laboratory- so I guess that something may be wrong in my "wet" model. Any idea?

Thank you very much in advance!

 

[seymours2571]

Hello Oscar,

It can be done, but it can be tedious and complex. You will need to create a solid mesh of the structure, in your case the vessel. If your vessel contains the water you will need to mesh the water domain with Fluid30 elements. The mesh between the solid elements and fluid elements will need to be conformal, meaning the solid and fluid elements share the same nodes at the interface.

Next, you will need to set the nodes at the interface of the solid and fluid elements as fluid structure interaction nodes by using the SF command with the FSI option.

Finally, you will have to perform a harmonic analysis with the full option and sweep the frequency over the desired range.

When the analysis is finished you graph the displacement at a couple of key nodal locations and observe the resonances.

This method performs the analysis completely within Ansys classic. However, you may be able to do the same analysis simpler by using the Ansys WB and CFX FSI coupling. However, I do belive the FSI interface between AnsysWB and CFX requires that the solution be determined in the time domain and not the frequency domain. So you may be forced to perform an analysis with a time varying load.

Pretty messy...but it can be done.

Good luck,

Steve

 

[oscar1057]

Thanj you Steve for your valuable help!!!
In fact all my problems come from the FSI -I think-. I have my vessel meshed (SOLID 92), the water meshed (FLUID30) and my "free beam" meshed (SOLID45).
Then I try to select all the solid-fluid interaction nodes between vessel-water and "free beam"-water.
Then I ask for a modal solution and it gives me a solution consiting of x vibrational modes, all of them at 0 Hz.
I'll keep on working.
Again, thanks a lot!

 

[seymours2571]

Oscar,

First make sure you do not have any rigid body modes. Next, I think I remember somewhere that you can only use a harmonic sweep to determine the resonant modal frequencies.

In the ansys verification manual see Case# 177. I believe the verification problem is very similar to yours.

Steve

 

[oscar1057]

Yep, VM177 has been my model.
Maybe you're right and I can only make a frequency sweep but it seems quite ilogical since I could made it in my "dry" model.

Again thanks Steve.

 

[omidomidi]

modal analysis solution in Ansys can only be applied to a model with no nonlinerity. so when you want to obtain the frequencies of a model which for example has material nonlinierities or contact has been defined between two objects in the model you only have to use harmonic analysis to gain the natural frequencies of your model as is in your model and performing a modal analysis cant bring you the correct result.

 

[nodalDOF]

Check the following regarding modal analysis. If damping can be applied to element then why not specify a equivalent damping coefficient and run the modal analysis?


3.3. Building the Model for a Modal Analysis
When building your model with the intention of performing a modal analysis, the following conditions apply:

(1)Only linear behavior is valid in a modal analysis.

(2)If you specify nonlinear elements, ANSYS treats them as linear. For example, if you include contact elements, their stiffnesses are calculated based on their initial status and never change.

(3)Material properties can be linear, isotropic or orthotropic, and constant or temperature-dependent.

Define both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form). ANSYS ignores nonlinear properties.

(4)If applying element damping, define the required real constants for the specific element type (COMBIN7, COMBIN14, COMBIN37, and so on).

 

[seymours2571]

The OP was asking for help with a problem involving viscous damping, not material damping.

Modal analyses are inherently linear.

However, the problem outlined in the verification manual (#177), which is well suited for the OP's particular problem, is a harmonic frequency sweep within a fluid structure interaction (FSI) problem.

While I understood the problem the OP was trying to solve based on the question presented, some may have found it more helpful if the question was phrased as: "I need to find the first four fundamental freqencies of structure submerged in a water medium...."

 

[nodalDOF]

Seymours,

Yes, that could have been a well posed question....

I am not a vibrations guy so may be dumb questions...... How diferent the response of a structure would be in material vs. viscous damping? Can't we incorporate viscous damping in to material damping which could be easily input through a real constant in ansys?

Also, i found the following article is very useful...It discusses about viscous damping too

http://www.ansys.com/industries/automotive/material-damping-properties.pdf

Thanks,
Nodal.

 

[seymours2571]

Nodaldof,

I would suspect that the damping that comes from the water environment would highly dominate compared to material damping of the metal vessel. You could in Ansys I believe include both effects, but the inclusion of the material damping may not affect the solution as much as the water environment viscous damping.

And with viscous damping, it is a function of the velocity of the body within the fluid medium, where as the structural damping (material damping) is just the loss of energy per cycle or during the deformation of the body. For instance, if you had a long cantiliever beam vibrating in a fluid medium such as water, I don't know if you could accurately account for the total damping (viscous + material) by modifying the constant material damping coefficient. Reason being, at the tip of the beam the velocity of the body would be higher than at the base. Therefore, the amount of damping would vary along the length of the beam. Furthermore, I am not sure how one would even determine the constant material damping coefficient to use to emulate the total damping for a structure vibrating in a fluid medium.

That article you provided is good. I love those quick little primers. I always find those things helpful and a good read.

Steve

 

[nodalDOF]

Steve,

You are right. I think people already thaught in those lines and concluded that there may be significant error if we represent viscous dampng through non-viscous and viceversa.

linkinghub.elsevier.com/retrieve/pii/S0022460X00933911
linkinghub.elsevier.com/retrieve/pii/S0022460X00933923

Thanks,
Nodal