[franciscofelis]

Hello to everyone.

I'm trying to build a modify version of the incompressible kEpsilon turbulence introducing a variable density formulation for the transport equations to describe a two phase mean flow (air+water).

I'am using the twoLiquidMixingFoam as a base and I have created my personalized k-epsilon model from the incompressible part. My idea is to change the ddt(k) with ddt(rho, k) and add other source terms also as a function of "rho".

I'm rather new to this, but until now every problem that I have encountered I have managed to solve it by reading, reading and reading... until now:

I couldn't find a way to inherit the volScalarField rho and surfaceScalarField rhoPhi to the kEpsilon class.

Is there any efficient way to do that? Here is what I want:

To go from this:

        fvm::ddt(k_)
      + fvm::div(phi_, k_)
      - fvm::laplacian(DkEff(), k_)
     ==
        G
      - fvm::Sp(epsilon_/k_, k_)

To this:

        fvm::ddt(rho_, k_)
      + fvm::div(rhoPhi_, k_)
      - fvm::laplacian(rho_*DkEff(), k_)
     ==
        rho*G
      - fvm::Sp(rho*epsilon_/k_, k_)

And for that, to my understanding, rho and rhoPhi must be inherited from turbulencemodel->RASModel->mykEpsilon.

I would really appreciate your help!

- Francisco

[kmooney]

Hi Francisco,

A few things:
1. When you mention inheriting a field, what you probably want to do is use a object registry lookup. Its an extremely powerful and easy thing that makes OpenFOAM super cool. If you wanted to pull in the density field, as long as its declared as a regIOobject, you can do this:

volScalarField& rho = mesh().lookupObject<volScalarField>("rho")

Basically, as long as you can get a reference to the mesh class, you can load up pretty much any field which is registered.

2. Compressible turbulence models already assume a non uniform density so that might be a better place to start then the incompressible turbulence classes.

3. This whole conversation might be moot because foam 2.3 has a multiphase kEp model .

http://www.openfoam.org/version2.3.0/multiphase.php

Cheers!
Kyle

[franciscofelis]

Hello Kyle,

Thanks for your answer. Effectively I looked also into the incompressible side of the Turbulence model constructor, however, It seemed more simple to add "rho" than modify the thermophysical part to work along the Multiphase transport one.

I've started also to look into the 2.3 version and the new universal turbulence models for multiphase, however I don't feel myself so "strong" in OpenFOAM for using it yet...

For now, I've tried the Mesh lookup method that you mentioned and it didn't work. Here is the output:

rhokEpsilon.C:144:33: error: ‘mesh’ was not declared in this scope
     volScalarField& rho_ = mesh().lookupObject<volScalarField>("rho");

To my understanding, the way that the turbulence model is constructed, he doesn't know that there is any mesh, a part from the constructors, any other variable that works beneath the "turbulence model" has to be inherited or read directly from an IO file, like k for instance:

k_
    (
        IOobject
        (
            "k",
            runTime_.timeName(),
            mesh_,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        autoCreateK("k", mesh_)
    ),

From the constructor inherited from RASModel and Incompressible Turbulence Model these are the only available:

rhokEpsilon::rhokEpsilon
(
    const volVectorField& U, // hoping to add rho somewhere here
    const surfaceScalarField& phi,
    transportModel& transport,
    const word& turbulenceModelName,
    const word& modelName
)
:
    RASModel(modelName, U, phi, transport, turbulenceModelName),

So, to my understanding, it seems a little more complicated... Do you have any other inside on a way to call rho into the KEpsilon class ?

Many thanks in advance.

--Francisco

[alexeym]

Hi,

as kEpsilon is a child of RASModel class, which in turn is a child of trubulenceModel class it has mesh_ property. So your call should be

const volScalarField& rho = mesh_.lookupObject<volScalarField>("rho");

or, if we forget about inheritance, you can use

const volScalarField& rho = U_.mesh().lookupObject<volScalarField>("rho");

maybe in final implementation you'll move this call into the constructor of derived kEpsilon model.

[franciscofelis]

Hello Alexey,

Thanks, it works like a charm!

So, finally, what I've done was to change the transport model for k and epsilon to a variable density formulation, which I think is more real when the difference between rho1 and rho2 is important. Here is the final code:

1) change in the production term of k: Do you think that this form of the variable density boussinesq is good? (rho is added at the end into the equations)

volScalarField G
    (
        GName(), 
        (((2.0/3.0)*I)*k_ - 2.0*nut_*(symm(fvc::grad(U_))-(1.0/3.0)*I*(fvc::div(U_))))
        && fvc::grad(U_)
    );

2) Read rho and phiRho from the mesh:

    const volScalarField& rho_ = mesh_.lookupObject<volScalarField>("rho");
    const surfaceScalarField& rhoPhi_ = mesh_.lookupObject<surfaceScalarField>("rhoPhi");

3) Modify k and epsilon equations:

// Dissipation equation
    tmp<fvScalarMatrix> epsEqn
    (
        fvm::ddt(rho_, epsilon_)
      + fvm::div(rhoPhi_, epsilon_)
      - fvm::laplacian(rho_*DepsilonEff(), epsilon_)
     ==
        C1_*rho_*G*epsilon_/k_
      - fvm::Sp(C2_*rho_*epsilon_/k_, epsilon_)
    );

// Turbulent kinetic energy equation
    tmp<fvScalarMatrix> kEqn
    (
        fvm::ddt(rho_, k_)
      + fvm::div(rhoPhi_, k_)
      - fvm::laplacian(rho_*DkEff(), k_)
     ==
        rho_*G
      - fvm::Sp(rho_*epsilon_/k_, k_)
    );

All of this works inside a slight variation of the twoLiquidMixingFoam, which describes the dispersed phase (water droplets into air) into a single equation (alpha1). I hope that'll do the work...

Many thanks to everyone.

-- Francisco

[Fanfei]

Originally Posted by franciscofelis

Hello Alexey,

Thanks, it works like a charm!

So, finally, what I've done was to change the transport model for k and epsilon to a variable density formulation, which I think is more real when the difference between rho1 and rho2 is important. Here is the final code:

1) change in the production term of k: Do you think that this form of the variable density boussinesq is good? (rho is added at the end into the equations)

volScalarField G
    (
        GName(), 
        (((2.0/3.0)*I)*k_ - 2.0*nut_*(symm(fvc::grad(U_))-(1.0/3.0)*I*(fvc::div(U_))))
        && fvc::grad(U_)
    );

2) Read rho and phiRho from the mesh:

    const volScalarField& rho_ = mesh_.lookupObject<volScalarField>("rho");
    const surfaceScalarField& rhoPhi_ = mesh_.lookupObject<surfaceScalarField>("rhoPhi");

3) Modify k and epsilon equations:

// Dissipation equation
    tmp<fvScalarMatrix> epsEqn
    (
        fvm::ddt(rho_, epsilon_)
      + fvm::div(rhoPhi_, epsilon_)
      - fvm::laplacian(rho_*DepsilonEff(), epsilon_)
     ==
        C1_*rho_*G*epsilon_/k_
      - fvm::Sp(C2_*rho_*epsilon_/k_, epsilon_)
    );

// Turbulent kinetic energy equation
    tmp<fvScalarMatrix> kEqn
    (
        fvm::ddt(rho_, k_)
      + fvm::div(rhoPhi_, k_)
      - fvm::laplacian(rho_*DkEff(), k_)
     ==
        rho_*G
      - fvm::Sp(rho_*epsilon_/k_, k_)
    );

All of this works inside a slight variation of the twoLiquidMixingFoam, which describes the dispersed phase (water droplets into air) into a single equation (alpha1). I hope that'll do the work...

Many thanks to everyone.

-- Francisco

Hellow Francisco:
I add the
const volScalarField& rho_ = mesh_.lookupObject<volScalarField>("rho"); the process suggest that mesh_ is not defined, while i try to use
const volScalarField& rho_ = U.mesh().lookupObject<volScalarField>("rho");
I was tell the U is not defined. what's the matter with it?

Best regards
Fan Fei

[franciscofelis]

Hello Fan Fei,
My solver works with binary mixture, so it is a variable density solver for incompressible flows, hence the "rho" (of the mixture).
If you have a volScalarField "rho" somewhere in your case, it should be able to find it.
Best regards,
Francisco

[Fanfei]

Originally Posted by franciscofelis

Hello Fan Fei,
My solver works with binary mixture, so it is a variable density solver for incompressible flows, hence the "rho" (of the mixture).
If you have a volScalarField "rho" somewhere in your case, it should be able to find it.
Best regards,
Francisco

Hi Francisco:
Thanks for you reply me so quick. I add the rho to incompressible Ke model with the the above method, when i compile, it always suggested me that, the mesh_ is not defined in this cope.

Best regards
Fan Fei

[Fanfei]

Originally Posted by franciscofelis

Hello Fan Fei,
My solver works with binary mixture, so it is a variable density solver for incompressible flows, hence the "rho" (of the mixture).
If you have a volScalarField "rho" somewhere in your case, it should be able to find it.
Best regards,
Francisco

Hi Francisco:
It's work now, yesterday i Put the on the wrong place, so it's always hint me the mesh_ is not define. Thanks.

Best Redrads
Fan Fei

[app1e]

Hi,Francisco

I tried to modify the k&epsilon equation exactly the same as you posted at #5.But i got a worse result compared to the simulation without implement.So i was wondering if you got the desired result after the implement.
Thank you in advance.

Aloha

[franciscofelis]

Hi Aloha,
I havn't yet arrived to a proper conclusion. I use this formulation only to be consistent with the Favre-Averaged RANS equations of my problem (turbulence in binary mixture).
Maybe next year... I hope.
Best Regards
Francisco

[app1e]

Hi,francisco
Thanks all the same
Best wishes

[Fanfei]

Originally Posted by app1e

Hi,Francisco

I tried to modify the k&epsilon equation exactly the same as you posted at #5.But i got a worse result compared to the simulation without implement.So i was wondering if you got the desired result after the implement.
Thank you in advance.

Aloha

hi Aloha：
Have you found the reseaons of your worse result. Nowadays, I am building a new template for multiphase turbulence model base on incompressible turbulence model and compressible turbulence model .Did you try to add the 'rho' Item from the laminar to RAS model. It looks like the wall funtion filed also need to add the the "rho" item.

Best regards
Fanfeisohu

[franciscofelis]

Hello,

Currently I'm using the same but in the RSM model. I couldn't say that the results are worst, but rather different, mostly because of the large density ratio of the mixture in my problem, so the results changes a lot by adding the variable density effects to the turbulence modelling. Nevertheless, compared to LDA measurements, it works pretty well.

I've done so by using the old of-2.2. I know that with the new generic turbulence template one shouldn't do it like I did... but I'm almost at the end of my thesis now, I won't change everything at the end...

Best regards.

Originally Posted by Fanfei

hi Aloha：
Have you found the reseaons of your worse result. Nowadays, I am building a new template for multiphase turbulence model base on incompressible turbulence model and compressible turbulence model .Did you try to add the 'rho' Item from the laminar to RAS model. It looks like the wall funtion filed also need to add the the "rho" item.

Best regards
Fanfeisohu

[Luis F]

Hi Fanfei,

Where exactly did you paste this?

const volScalarField& rho_ = mesh_.lookupObject<volScalarField>("rho");
const surfaceScalarField& rhoPhi_ = mesh_.lookupObject<surfaceScalarField>("rhoPhi");

Best regards