CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

CavitatingFoam Equations

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By schmidt_d

Reply
 
LinkBack Thread Tools Display Modes
Old   July 7, 2007, 06:54
Default Hi I am studing about the new
  #1
New Member
 
morteza
Join Date: Mar 2009
Posts: 18
Rep Power: 8
morteza is on a distinguished road
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
morteza is offline   Reply With Quote

Old   July 7, 2007, 11:36
Default Morteza, cavitatingFoam has a
  #2
Member
 
David P. Schmidt
Join Date: Mar 2009
Posts: 70
Rep Power: 8
schmidt_d is on a distinguished road
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
schmidt_d is offline   Reply With Quote

Old   July 7, 2007, 14:45
Default David, Thanks for your quick
  #3
New Member
 
morteza
Join Date: Mar 2009
Posts: 18
Rep Power: 8
morteza is on a distinguished road
David,
Thanks for your quick reply.

Morteza
morteza is offline   Reply With Quote

Old   July 8, 2007, 09:28
Default Is it possible to deal with lo
  #4
New Member
 
Connie Scofield
Join Date: Mar 2009
Posts: 12
Rep Power: 8
zjucfd is on a distinguished road
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.
zjucfd is offline   Reply With Quote

Old   July 9, 2007, 11:11
Default Connie, I am mostly an expe
  #5
Member
 
David P. Schmidt
Join Date: Mar 2009
Posts: 70
Rep Power: 8
schmidt_d is on a distinguished road
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
sharonyue likes this.
schmidt_d is offline   Reply With Quote

Old   May 11, 2010, 11:43
Default
  #6
Member
 
Marta's Avatar
 
Marta Lazzarin
Join Date: Jun 2009
Location: Italy
Posts: 69
Rep Power: 8
Marta is on a distinguished road
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
Marta is offline   Reply With Quote

Old   October 14, 2010, 05:16
Default compressibility models
  #7
jml
New Member
 
Jml
Join Date: Mar 2009
Posts: 23
Rep Power: 8
jml is on a distinguished road
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
jml is offline   Reply With Quote

Old   May 17, 2014, 23:00
Default
  #8
Member
 
yehanyu
Join Date: Mar 2012
Location: Beijing, China
Posts: 36
Rep Power: 5
yhy20081016 is on a distinguished road
Quote:
Originally Posted by morteza View Post
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
yhy20081016 is offline   Reply With Quote

Old   May 13, 2015, 14:04
Default
  #9
Member
 
alvaro
Join Date: Apr 2015
Posts: 33
Rep Power: 2
alvariten is on a distinguished road
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.
alvariten is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
CavitatingFoam psil psiv kyubi OpenFOAM Running, Solving & CFD 7 June 3, 2014 07:06
CavitatingFoam for Diesel injector nozzles javier_salvador OpenFOAM Running, Solving & CFD 0 July 16, 2008 09:37
CavitatingFoam with a moving mesh mass conservation error idosil OpenFOAM Running, Solving & CFD 3 November 27, 2007 18:27
Problem with cavitatingFoam clo OpenFOAM Running, Solving & CFD 1 June 7, 2007 11:53
LES equations Daniel Main CFD Forum 14 March 26, 2005 08:30


All times are GMT -4. The time now is 11:49.