CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   CavitatingFoam Equations (http://www.cfd-online.com/Forums/openfoam-solving/59582-cavitatingfoam-equations.html)

morteza July 7, 2007 06:54

Hi I am studing about the new
 
Hi
I am studing about the new cavitatingFoam implemented in openfoam-1.4.
Can someone tell me about the governing equations are used in this solver(or reference to equations).

Thanks
morteza

schmidt_d July 7, 2007 11:36

Morteza, cavitatingFoam has a
 
Morteza,
cavitatingFoam has a few different models for the physics. I can tell you about the "Wallis" model. Wallis derived the equation for the speed of sound through a bubbly mixture in thermal equilibrium. I used this speed of sound relationship as the basis of a cavitation model in the mid 1990's. My other contribution was to find a closed-form integral to produce a barotropic equation of state.

cavitatingFoam shares the same physical basis, when used with the Wallis model. However, the numerics and behavior are quite different. My code used the explicit expression for pressure which produces a low-cost per time step, but can only be used efficiently for something like diesel fuel injection, where the velocity is the same order of magnitude as the speed of sound. The cavitatingFoam code can operate efficiently at lower velocities.

For more info, I have posted my dissertation at:
http://www.ecs.umass.edu/~schmidt/Sc...ssertation.pdf

morteza July 7, 2007 14:45

David, Thanks for your quick
 
David,
Thanks for your quick reply.

Morteza

zjucfd July 8, 2007 09:28

Is it possible to deal with lo
 
Is it possible to deal with low mach problems?

hi, Dr. Schmidt,

You said "The cavitatingFoam code can operate efficiently at lower velocities". But how could it be done? I attempted to simulate a cavitating flow around a hydrofoil at low mach number using cavitatingFoam, but can not get a physically reasonable results.

schmidt_d July 9, 2007 11:11

Connie, I am mostly an expe
 
Connie,

I am mostly an expert at my own code, which I wrote using very simple, but pretty stable numerics. The cavitatingFoam code comes from Henry Weller. Fabian Peng Karholm (spelling?) uses it a lot.

From what I see, the cavitatingFoam code tries to couple the pressure solution pretty tightly with the eqn. of state and continuity, so that you are treating accoustic waves implicitly. You are trying to avoid having to respect a Courant number that contains the speed of sound in the velocity, because then the stable time step size would have to be tiny. With cavitatingFoam you can take time steps where this accoustic CFL number is much greater than 1.0. I am not sure how high you can go, but the tutoral case operates at an accoustic CFL number of 50, if memory serves.

I've had some stability problems with cavitatingFoam too. I haven't invested enough time to know whether the problem is with my inputs or not. I can say this: pressure with a barotropic model should always be positive. But because of the discretization of the pressure equation, cavitatingFoam can predict negative pressures.

If you are going to do a hydrofoil, I am not sure how much sense it makes to use a barotropic model anyway. In my thesis, I justify using a barotropic model based on typical fuel injection conditions. As length scales get large, the physics might well change. And if you do something where you have to keep the accoustic courant number < 1 for a big old hydrofoil, you will have to wait a long, long time for the code to run.

DPS

Marta May 11, 2010 11:43

Dear Foamers, i am experiencing a negative pressure too with cavitatingFoam...i read in this post that this can be due to the pressure equation discretization, but what does this exactly mean? is there a way to avoid this that you can advice?

Thank you very much!

Marta

jml October 14, 2010 05:16

compressibility models
 
Hello,

I have read your post about compressibility models and I have some questions. I have used cavitatingFoam with diesel injectors with a linear model of compressibiliy, and it works quite well.

Now, I want to improve the realism of the simulations using a "Wallis" or a "Chung" model. However when I used these models the simulation has a lot of problems of convergence, giving unreasonable values of density, pressure.. The only difference between the linear and the other models in the configuration of the case is the rhomin parameter (0.1).

Anyone know what are the reason of these problems?

Thanks

yhy20081016 May 17, 2014 23:00

Quote:

Originally Posted by morteza (Post 204452)
Hi
I am studing about the new cavitatingFoam implemented in openfoam-1.4.
Can someone tell me about the governing equations are used in this solver(or reference to equations).

Thanks
morteza

You can go through the codes in the "barotropicCompressibilityModel" folder. There is a scalar field called "psi_". This variable is the product of density and the isentropic compressibility:
psi_=rho*alpha
where rho is density, and alpha is isentropic compressibility. The definition of "isentropic compressibility" can be found in many engineering thermodynamics text books, such as

Moran M. J. et al. Fundamentals of Engineering Thermodynamics, 7th ed. John Wiley & Sons, 2011

alvariten May 13, 2015 14:04

Quote:

Hello,

I have read your post about compressibility models and I have some questions. I have used cavitatingFoam with diesel injectors with a linear model of compressibiliy, and it works quite well.

Now, I want to improve the realism of the simulations using a "Wallis" or a "Chung" model. However when I used these models the simulation has a lot of problems of convergence, giving unreasonable values of density, pressure.. The only difference between the linear and the other models in the configuration of the case is the rhomin parameter (0.1).

Anyone know what are the reason of these problems?

Thanks
Hi jml,

I'm using cavitatingFoam (OF v.2.3.x) with diesel injectors and convergences issues similar to yours are appearing. I am using the default configuration of tutorial case. Did you get solve the problems finally? In this case, What did you do?

Thanks in advance.


All times are GMT -4. The time now is 18:45.