[matthias_hofmann]

Hi,

I want to use interPhaseChangeFoam on my case, but I can't find any information about the coefficients needed for the Kunze- Merkle- or SchnerrSauer phase change models, nor can I find any information about the models themselves.
Can anyone please tell me the dimensions of the coefficients? Some typical values would be great too.
Or does someone know a link which could help me?

Best regards
Matthias

[isabel]

Here you have a tutorial in wich perhaps you find interesting information:

http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2008/NaixianLu/REPORT_interPhaseC hangeFoam.pdf

[MartinaF]

The dimensions of the coefficients are:
KunzCoeffs
{
Cc Cc [0 0 0 0 0 0 0] 1000;
Cv Cv [0 0 0 0 0 0 0] 10000;
UInf UInf [0 1 -1 0 0 0 0] 6;
tInf tInf [0 0 1 0 0 0 0] 1;
}
MerkleCoeffs
{
Cc Cc [0 0 0 0 0 0 0] 1000;
Cv Cv [0 0 0 0 0 0 0] 10000;
UInf UInf [0 1 -1 0 0 0 0] 6;
tInf tInf [0 0 1 0 0 0 0] 1;
}
SchnerrSauerCoeffs
{
Cc Cc [0 0 0 0 0 0 0] 1000;
Cv Cv [0 0 0 0 0 0 0] 10000;
n n [0 -3 0 0 0 0 0] 10000;
dNuc dNuc [0 1 0 0 0 0 0] 1e-06;
}
The values of the coefficients depends on the simulation case.

[MartinaF]

cavitation
{
pSat pSat [1 -1 -2 0 0 0 0] -18000;
restart no;
rampN 200;
startN 10000;
}

[vahid.najafi]

Hi !!!
I transform Saur model to Zwart model successfully but transforming Saur model to Singhal model is faild!!!
I see this error :

phaseChangeTwoPhaseMixtures/phaseChangeTwoPhaseMixture/phaseChangeTwoPhaseMixture.C:48: error: no matching function for call to ‘Foam::dimensioned<double>::dimensioned()’

Can you help me???

[MartinaF]

Hi,

to help you, having your implementation would be great. Within the data you attached, I did not find any "Singhal model" implementation. Or have you used the phaseChangeTwoPhaseMixture/phaseChangeTwoPhaseMixture/phaseChangeTwoPhaseMixture.c, where also your error is located?
By the way: a documentation of the "Singhal model" could also help.

Best regards,
MartinaF

[sfigato]

Hi,

I would like also to implement th Singhal model in OpenFoam. Which is the best solver to use with this model? Moreover, I have to account for liquid, vapour and some non condensable gas (dissolved and undissolved). I am quite new in implementing a new model in OpenFoam. What are the steps that I have to follow?

Regards
Marco

[vahid.najafi]

Hi.
I do this completly.
Please Ask your question more clearly?

[sfigato]

Hi Vahid,

Have you already done it? I try to explain myself better...I would like to implement a cavitation model in OpenFOAM! The cavitation model is the FULL CAVITATION MODEL developed by Singhal at al.

The reference are : INDUSTRIAL TWO PHASE FLOW (Full cavitation model) Von karman Institute
`Mathematical basis and validaion of the full cavitation model` Singhal, A.

I have never implemented a new model in OpenFOAM! The interPhaseChangeFoam solver is the right solver to do it?

My model will account for two types of cavitation: the vapuor cavitation (due to a decrease of the pressure under the equilibrium vapor pressure) and the gas-cavitation (due to a release of the dissolved non condensable gas from the liquid) !

So my mixture would be liquid+vapour+dissoved nonCondensableGas+ undissoved nonCondensableGas. Does the interPhaseChangeFoam account just for two phase? It is difficult extend it for more than two components? Moreover, I would like to account for mass transfer between liquid and vapour as well as dissolved and undissolved Gas.


Anyway, as you understood I `m quite new with such staff! So please can you give some hints or outlines to start my project?

Thanks in advance

Regards
Marco

[vahid.najafi]

Hi dear Marco.
yes,I made this solver in five or six month ago.
and its working very very good.
Now I'm working on a paper,Next week i can get more help for you!!!

Please send me your email?

[sfigato]

Goodmorning Vahid,

it sounds great!!! I am very happy that you can share some knowledge with me!! I am very in trouble with this model! My mail is:

m.longhitano88@gmail.com

Can you give me also your mail or send me a mail! I will contact you the next week (when you are free to reply to me)!

Thank you very much!

Regards
Marco

[Diego13]

Hi all,

I already invested a lot of time, figuring out the source code of interPhaseChangeFoam and still there are some essential details I can't find any information to.

In the UEqn.H, there is the follwing equation i try to understand:

fvVectorMatrix UEqn
(
     fvm::ddt(rho, U)
   + fvm::div(rhoPhi, U)
   - fvm::Sp(fvc::ddt(rho) + fvc::div(rhoPhi), U)
   + turbulence->divDevRhoReff(rho, U)
);

And here are my questions:

• What is rho in this equation?
• What does the Sp-term do? I read this some kind of source-term, but if that is so, where is the connection to phasechange?
• What does divDevRhoReff mean?

I appreciate any kind of help!

Diego

[sfigato]

Hi Diego,

"rho" is the mixture density!

The Sp term is used to create a larger diagonal term (to aid the solver) so it only can be used if the linearization of the source term has a negative dependency on the variable being solved for!

The turbulence term accounts for the turbulence correction of the viscosity!

I hope that it helps you
Regards
Marco

[Diego13]

Hi Marco,

thank you for the answer, it helped me indeed. Just one more thing:
Is it correct to say, that the Sp-term has no physical significance? In comparison with the momentum equation, I can not find any analogy to this part. Would it therefore be valid to comment it out, as long as convergence is assured?

Diego

[abe]

Hi Diego,

You are right. I think Sp had been added to improve convergence and coupling between equations.

PS: in OF22, it has been removed!

I have a question from you, which OF version do you use (2.1 or oledr)?
Thank you in advance
ABE

[sfigato]

Hi Diego,

Abe and yo are right! Sorry For the late response!


Regards
Marco

[Diego13]

I am using 2.1. Thats interesting, I will try simulating without Sp in 2.1. Thanks for the good advice!

Diego

[sfigato]

Hallo Faomers,

I am using interPhaseChangeFoam (OpenFoam 2.2.x) to simulate cavitatation in an orifice (I have implemented the singhal mass transfer model)! Unfortunatly, my simulation blows uo due to too high turbulent variable values (kEpsilon model)
Have abyone experice to set boundary condition for tutrbulent on interPhaseChangeFoam

Regards
Marco

[sfigato]

Hi Foamers,

Sorry I was wrong and I posted the same post two times! Here are my turbulent boundary conditions

dimensions [0 2 -3 0 0 0 0];

internalField uniform $turbulentEpsilon;

boundaryField
{
OUTLET
{
type zeroGradient;
}
WALLS
{
type epsilonWallFunction;
value $internalField;
}
SYM1
{
type symmetryPlane;
}
SYM2
{
type symmetryPlane;
}
INLET
{
type fixedValue;
value $internalField;
}


#include "include/initialConditions"

dimensions [0 2 -2 0 0 0 0];

internalField uniform $turbulentKE;

boundaryField
{
OUTLET
{
type zeroGradient;
}
WALLS
{
type kqRWallFunction;
value $internalField;
}
SYM1
{
type symmetryPlane;
}
SYM2
{
type symmetryPlane;
}
INLET
{
type fixedValue;
value $internalField;

Thanks
Regards
Marco

[zhouhoucun]

Originally Posted by vahid.najafi

Hi dear Marco.
yes,I made this solver in five or six month ago.
and its working very very good.
Now I'm working on a paper,Next week i can get more help for you!!!

Please send me your email?

Dear Vahid,
I did the same job with you, I have add the Zwart and Singhal model into this solver without any error.But the simulation results of hydrofoil NACA0015 are quiet different from that the Kunz and Schnerr model.
Could you give me some advices? Or could you send me your models? My email address is 470861844@qq.com
Thank you in advance!