[sinatahmooresi]

Hi Foamers !
I was checking the source code of RAS models in OP3.0.1 and I found that there is no term for production due to buoyancy effect in none of RAS models! the only production term is G or p (that is the production due to stress and not buoyancy) so I checked k-e , LRR and SSG model and I couldn't find the buoyancy term. I just found buoyantKEpsilon in compressible RAS models that included the buoyancy effect due to density changes. so is that (the buoyantKEpsilon) the only buoyant turbulence model in OP3.0.1 ?
or I am missing something about this ? I thought maybe the correction could be in somewhere in buoyant solvers. but as I found, in the solver just modification are done by correction of momentum eqns. so what is going on ? advises are appreciated
Regards sina

[Attavino]

Hi Sina,

sorry for the late answer, at the moment the buoyantKEpsilon is the only turbulence model that includes production due to buoyancy force, however for both incompressible and compressible models it is not difficult to include the source therm, just follow how the buoyantKEpsilon model is implemented. However if you wish to use the kOmega you will also need to modify the basic kOmega model since the source functions are not included in there.

Best Regards,

Andrea

[rrsantos]

Did you solve this?

Now I am working on OpenFOAM 4.1, and I have the same problem. I want to implement buoyant terms to solve incompressible solver.

I implement a new model using Kassem's guide, based on buoyant K-epsilon. But, the code bellow, to use g is not recognised by the incompressible library.

buoyantKEpsilon<BasicTurbulenceModel>::Gcoef() const { const uniformDimensionedVectorField& g = this->mesh_.objectRegistry::template lookupObject<uniformDimensionedVectorField>("g");
return (Cg_*this->Cmu_)*this->alpha_*this->k_*(g & fvc::grad(this->rho_)) /(this->epsilon_ + this->epsilonMin_); }

My doubt is, how to use g to calculate the buoyant terms using incompressible library?

[agustinvo]

Hello

the problem is in rho. In incompressible solvers that variable does not exist, and when you try to use this code for the buoyant term it gives an error. Please check how to define there your density and replace it in this code.

[rrsantos]

Thank you Agustin, it helped.

I think I found a solution. As I said before, I used buoyantKEpsilon code to use to incompressible solver twoLiquidMixingFoam. The problem is when "this->rho_" is used in the equation.


Using the same command to bring "g", I brought the volScalarField rho

const volScalarField& rhoRA =
this->mesh_.objectRegistry::template
lookupObject<volScalarField>("rho");

And I used it in the equation.

(Cg_*this->Cmu_)*this->alpha_*this->k_*(g & fvc::grad(rhoRA))/(rhoRA*(this->epsilon_ + this->epsilonMin_));

As the equation is incompressible, it should be diveded by the density. So, I modified the equation

...*(g & fvc::grad(rho_))*(this->epsilon_ + this->epsilonMin_)

to

...*(g & fvc::grad(rhoRA))/(rhoRA*(this->epsilon_ + this->epsilonMin_))

[nitinkumar@cfd]

Hi rrsantos
I am working on incompressible buoyancy-driven flow using OpenFOAM-6. Since the openfoam do not have the code for the contribution of production due to the buoyancy(for incompressible flow). Can you provide your code for the incompressible flow that will help me to write my code for buoyancy production terms. That will be a great help.



Thanks
N Kumar

[agustinvo]

Hi,


which solver are you using? Normally, in the incompressible framework the Boussinesq approximation is implemented, so the production term should be something like:

Pb = -beta * nut/Prt * (g & gradT)

being nut the one from the turbulence model, and gradT the gradient of temperature. If you use other approaches you should check how to implement such buoyancy term

[Raphael_Santos]

Hello there, I do not have access to my files, now, so

Nittin,
I did what I mentioned above (rrsantos here). Have a look at 'buoyantKEpsilon' turbulent model and try to understand how source term is defined there.

Agustinvo,
in my case, the buoyancy effect was based on the difference of density due to different species concentration. So, I used the definition based on reduced gravity (g' = g.delta(rho)/rho). My flow was isothermal.

Regards,
Raphael

[nitinkumar@cfd]

Hi agustinvo
I am using buoyantbuosinesqPimpleFOAM. Yes you are correct the expression will be similar but should i change the code in the buoyant Kepsilon its self or in k Epsilon model.

[Elol]

Hi Raphael,

It really helped alot this finding for incombressible fluids. But I have couple of questions.

1- why did you declared new variable rhoRA despite of it is already there "this->rho_" ?

2- When I applied your way I found out that i don't have dimensinon consistency, how did you manage to solve that ?

--> FOAM FATAL ERROR: 
incompatible dimensions for operation 
    [epsilon[1 -1 -4 0 0 0 0] ] + [epsilon[0 2 -4 0 0 0 0] ]

[Raphael_Santos]

Hello, Elol.

1. With rhoRA, I wanted to have a new variable with a different name of "rho", because I was a little bit afraid to get lost with the code. But, yes, you already have rho, there is no problem to use it.

2. As I used for incompressible fluid, ie, a incompressible solver, to make dimensional consistent, it is needed to divide the new expression by the density, as fvc::grad(rhoRA))/(rhoRA) [grad(rho)/rho]. So, check if the solver you are using is to compressible or incompressible cases.
Look, the left one dimension [epsilon[1 -1 -4 0 0 0 0] ] means [kg/(m.s^4)], and the right one [epsilon[0 2 -4 0 0 0 0] ] means [m^2/s^4], the difference lies in the product or division by the density. If your solver is compressible, you need to remove the division by the density.

I hope that helps you.

Cheers