[sinatahmooresi]

Originally Posted by mAlletto

Maybe
forAll (U , Celli)

U[Celli].component(0)

Greeting!
During running a test case with my modified solver (pimpleFoam) and modified LRR turbulence model, I get an error :symbol lookup error:Undefined symbol .....
and it is referring to dimensioned Vector
I just defined g (9.81) as a dimensionedVedtor in LRR.C and it compiled with no error. But it seems the solver is unfamiliar with that!
I should say that the solver is working without problem with other cases.
Exactly before calculation the R (Reynolds stress tensor) during the run, it jumps out. Inside the LRR.C I exactly before Reynolds stress eqns added that g (9.81) definition to use it as a vector in calculation of buoyancy term (Gb) to add that in to the Reynolds strees eqns.
Regards
Sina

[sinatahmooresi]

Originally Posted by sinatahmooresi

Greeting!
During running a test case with my modified solver (pimpleFoam) and modified LRR turbulence model, I get an error :symbol lookup error:Undefined symbol .....
and it is referring to dimensioned Vector
I just defined g (9.81) as a dimensionedVedtor in LRR.C and it compiled with no error. But it seems the solver is unfamiliar with that!
I should say that the solver is working without problem with other cases.
Exactly before calculation the R (Reynolds stress tensor) during the run, it jumps out. Inside the LRR.C I exactly before Reynolds stress eqns added that g (9.81) definition to use it as a vector in calculation of buoyancy term (Gb) to add that in to the Reynolds strees eqns.
Regards
Sina

The problem changed to another thing:
no longer previous error! But I can't switch the wallReflection off now! The new modified LRR model is working properly, but it can't distinguish that the wallReflection is switched off! Is it coming from compilation procedure?

[calf.Z]

Originally Posted by clapointe

There already is a buoyant kEpsilon model : https://github.com/OpenFOAM/OpenFOAM...yantKEpsilon.H. If, after checking out its implementation, it is not what you want it should be a good starting point for implementing your own variation.

Caelan

I am now using Gcoef in buoyantKE. I am wondering the meaning of this->alpha_ in Gcoef and g should include the direction or not?
In epsilonsource/ksource:

return -fvm::Susp(...)

If it return -.... in code, G should be -G*... But in equation, it should be +G*...

I am confused about it. Thank you.

[jherb]

alpha is the phase fraction. So this is used for two phase flows.


g is a vector and it has a direction: https://github.com/OpenFOAM/OpenFOAM...Epsilon.C#L104
And it is used in scalar products.


SuSp does add a source implizitly to an solver equation if it is positive, because this increases the stability of the solution. This means it is added to the diagonal of the matrix to be solved. If it is negative, it will be added explicitly, so to the "right" side of the equation.


So it makes a difference, if you put something like -fvm::SuSp(-G, k) or +fvm::SuSp(G, k) to an equation, because it checks the sign of the first argument.

[clapointe]

In this case isn't alpha thermal diffusivity? See eg : https://github.com/OpenFOAM/OpenFOAM...lDiffusivity.H.

Caelan

[jherb]

If you look for tutorial, where buoyantKEpsilon is used, you find them in:
tutorials/multiphase/driftFluxFoam/RAS/mixerVessel2D (dahl, tank3D)
These are multiphase cases, where alpha is used.


But to make sure, this is correct, I patched the buoyantKEpsilon/buoyantKEpsilon.C to output alpha dimension:

alpha: [0 0 0 0 0 0 0]

compare this to the dimensions of the thermal diffusivity:

 
//- Thermal diffusivity for enthalpy of mixture for patch [kg/m/s]

https://github.com/OpenFOAM/OpenFOAM...usivity.H#L116

[clapointe]

Good to know -- thanks for checking.

Caelan

[snak]

Hi,

I don't think that the alpha in compressibleTurbulenceModels is the phase fraction.

alpha will be the phase fraction for the phaseCompressibleTurbulenceModels.
https://github.com/OpenFOAM/OpenFOAM...ulenceModels.C

However, for incompressible or compressible TurbulenceModels, alpha will be just a geometricOneField.
https://github.com/OpenFOAM/OpenFOAM...moModels.C#L30
https://github.com/OpenFOAM/OpenFOAM...tricOneField.H

[snak]

In incompressibleTurbulenceModels, rhoField is also just a geometricOneField (uniform value of 1, without dimension).
When we use these models in multiphase-solver such as interFoam, density of fluid is not considered in the turbulenceModel. rho is 1 at everywhere.

Sofisticated and elegant source-code of turbulence models makes the meanings of alpha and rho in turbulence models a little unclear, I think.
We can get the both compressible and incompressible models from the same code in return for this.