CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   [Pictures] Pressure distribution problem (https://www.cfd-online.com/Forums/cfx/120476-pictures-pressure-distribution-problem.html)

Badi July 8, 2013 06:55

[Pictures] Pressure distribution problem
 
5 Attachment(s)
Hello,
maybe some of you will know (probably Glenn :D) but I am trying to simulate acoustic induced cavitation with a sonotrode. I attached the pictures of the setup and my problem.

Problems:

- I have a really strange pressure distribution within the domain. Somehow the pressure isnt working well. Once I have a pretty low pressure somewhiere in the domain (below saturation pressure, due to the movement of the top cylinder) it stays pretty low and doesnt go up anymore.

- Convergence problem: The RMS are fine but the Max Res are sometimes way above the target and the linear solution is always critical.


I would be glad if you have any hints how to fix this.

Attachements:
1. Setup
2. Timestep 0
3. Timestep 5
4. Timestep 60
5. CCL File

ghorrocks July 8, 2013 08:07

I have never heard of a sonotrode before. I have learnt something today :).

Have a look in CFD-Post where the maximum residuals are located but I bet they are in the narrow gap, which I presume is the oscillating bit.

You have defined the time step size. Have you any justification for this time step size or is it just a guess? For an extremely complex simulation like this I would use adaptive time stepping, with 5-10 coeff loops per iteration and define max and min time step sizes wide enough that the solver will never reach them. I suspect this model will need very small time steps to run successfully.

Badi July 8, 2013 08:15

Thanks for the quick and helpful reply. I did a sensitivity test on the model with straight movement. It worked best with 20 Timesteps from 0 to 2pi. I didnt work with adaptive time step yet but it sounds correct what you suggest. I try it with a mesh of only 1e6 nodes and see if it runs.

Badi July 8, 2013 08:37

1 Attachment(s)
Sorry for the doublepost but I have a general question.

At the moment I used to run incompressible solutions. I tryed to have a fully closed system (the opening in top was a free slip wall aswell). I thought that the strange pressure distribution was due to the closed system and incompressibility.

Since the Volume grows due to cavitation (vapour) and no compressibility is alowed I get extremly strange pressure (either extremly high or extremly low).

Does it makes sense to you and should I try it with the opening or rather the closed system (like i would like to do it)


edit: I am now trying to do it compressible too with the following functions:

1. Water Vapour density: p, li { white-space: pre-wrap; } 0.0006 [kg m^-3]+(7e-6*Absolute Pressure)/1 [Pa] * 1[kg m^-3]


2. Water density:
998.161 [kg m^-3] + (5e-7 *Absolute Pressure)/1 [Pa] *1 [kg m^-3]


edit: I posted a pretty strange initial pressure distribution from the very first timestep (0)

ghorrocks July 13, 2013 07:09

You always need to have some way of the simulation to handle small variations in mass/volume. An incompressibel simulation in an enclosed volume will never converge. Adding compressibility can fix that, so can adding a pressure outlet. You choose what is more appropriate.

You diagram is meaningless. You have magnified tiny pressure variations which are so small they are under 1Pa. It is hard to say whether this is meaningful or not, but I suspect not.

Badi July 13, 2013 07:17

Hello,
you are right, the way I was doing it was basically just trying to get more accurate data from invalid physics.
I changed the setup now so it should work better now since the cavitation is mostly due to acoustics.

The system is closed now (it has a free slip topwall), I changed the viscosity to a minimal value (so I have really laminar flow) and a density-pressure function for vapour and water.

What bothers me is that the solver starts with the right value for speed of sound of water (~1400 m/s I have a linear function for that) but with a wrong value for vapour (1e30, where my function is giving me ~300 m/s).
Is this maybe because of the default starting volume fraction of 1e-15 of water vapour?

ghorrocks July 13, 2013 07:48

Umm - low viscosity = high Re = turbulent flow. If you want low Re and laminar flow you need to INCREASE the viscosity.

I would only look at the acoustic velocity of regions where the volume fraction is high enough that something is happening - maybe 0.1. The acoustic velocity of regions with volume fraction of just about zero is going to be silly numbers.


All times are GMT -4. The time now is 11:23.