[pashazanousi]

I simulated a NWT to study an elastic plate vibration fixed on the tank floor exposed to group waves. but the generated waves disappear before reaching the plate.
I used ANSYS CFX with VOF model and Laminar flow model.

NWT.PNG

[ghorrocks]

I have no idea what a NWT is. Please do not assume people know what your acronyms mean.

But the answer to your question is you have too much dissipation. This is probably due to a poor simulation setup, possibly things like:
* Mesh too coarse
* Not converging tight enough
* Not high enough order advection scheme
* Other numerics too diffusive (interpolation schemes on other variables)
* Unsuitable advection scheme on VOF equation (should use compressive)
* Time step too large
* Need double precision numerics

[pashazanousi]

Thanks, ghorrocks

Sorry for late reply
You're right. I'm sorry for that mistake.
The NWT is the abbreviation for Numerical Wave tank.

Let's back to my problem:
The excitation period is about 2.96 sec and I considered the timestep equal to 0.01 sec.
My computational mesh is 100 per wavelength and 21 per wave height in the free surface area. The free surface area height is about two-wave height.
I used RMS residual target with 1E-4. Max. Coefficient loop of 200 used in CFX-pre and Max 20 Iteration for the coupling solver.
Simulation Time=180 sec
I selected these parameters according to recommendations in references and papers.
What is your idea about these parameters?

[ghorrocks]

Max coeff loops of 200 sounds way too high. 10 is more like what you want.

Coupling solver? What does this mean? What coupling solver? Are you doing this as a FSI simulation? If so, why?

[pashazanousi]

Thanks for your quick reply
I'm working on vibration of an elastic plate exposed to some group waves.
I need to validate with a paper results.
The paper used non-dimensional parameters. It's made it hard to validate for me!
I think the 2 way FSI is the right solution!
Do you have an other idea?

[ghorrocks]

I would get this model working accurately as a CFD only simulation before adding FSI. Putting it another way, there is no point doing the FSI model when the CFD sub-model is inaccurate.

So just do a CFD only model and get it working accurately. Then add the FSI bits.

[pashazanousi]

You mean at first I should do a simulation with 1 way FSI or a simple numerical wave tank with rigid plate?
I simulated an empty tank to validate Wavemaker theory! The results were in agreement with the theory!
Please explain more if you can!
Thanks ghorrocks!

[ghorrocks]

A simple numerical wave tank with a rigid plate sounds like a good next step.

[pashazanousi]

Thanks, ghorrocks
I will try it and share the results here

[ghorrocks]

You don't have to share it. What I describe is just good engineering practise: If you have a complex system of many parts and it does not work, then what is wrong? It is hard to fix as it is so complex.

So separate out all the individual component systems and get them working properly by themselves. Time spent doing this at the beginning means that when the complex system fails to work (like it always does first time around) then you know the problem has to be the interaction between the systems, because all the systems by themselves work OK.

This applies to any engineering system, not just CFD.

[pashazanousi]

Thank you for your generosity ghorrocks
You are so good and right is yours.
I will do as you said.

[pashazanousi]

Hi ghorrocks
I'm using a Desktop PC with these configurations:
CPU: Intel 10600 corei5
Ram: 16 GB ram
SSD & HDD: 240 GB+ 4 TB
I want to set up a MPI Local Parallel but I don't know how should I do it.

[ghorrocks]

Setting up parallel simulations is all described in the installation manual.

[pashazanousi]

Thank you ghorrocks
I study the manual about how set up a MPI Local parallel but honestly I understand almost nothing!

But I defined a MPI Parallel Partition for CFX Solver with specified direction(1,0,0) and High Priority! I set 2 for allocated factor!
I don't know are they the correct settings or not but Now the system is running well with 4 core (Max allowed partitions for free student version of Ansys).

Thank you for your attention and the time you spent

[pashazanousi]

Hi ghorrocks
I set the coupling residual equal to 0.01 (default value) and maximum coupling iteration equal to 20.
Does this setting lead to a good result?

[ghorrocks]

If you have parameters which you do not know if they are set correctly then do a sensitivity analysis to find out if they are important. Try coupling residuals of 0.001, 0.01 and 0.1 and see if it makes any difference. Likewise try max coupling iterations of 10, 20 and 40.

[pashazanousi]

Thank you ghorrocks
OK, I got it! I will do it!
But I want to know what is the meaning of residual target in the coupling regions!
For example for mesh transfer data from transient structural to CFX, I choose 0.01! It means 0.01 m as residual target? Or for Force Data transfer, 0.01 for residual target means 0.01 Newton?
I need the residual target equal to 0.0001 m for the mesh displacement!
I can't anything about that in Ansys help or other documents!

[ghorrocks]

I don't know the exact definition of that residual target. All I can say is to look in the documentation.

If you do a sensitivity analysis and show that you have set it tight enough that it is not affecting results then it does not matter what the exact definition is. It just means you have set it tight enough that your results are accurate (for that parameter at least).