CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Programming & Development (https://www.cfd-online.com/Forums/openfoam-programming-development/)
-   -   Introducing a scalar field for buoyancy production in k-epsilon (https://www.cfd-online.com/Forums/openfoam-programming-development/209681-introducing-scalar-field-buoyancy-production-k-epsilon.html)

sinatahmooresi October 22, 2018 14:20

Introducing a scalar field for buoyancy production in k-epsilon
 
Hi dear FOAMers!
I want to add the gradient of a scalar filed (like S) for calculation the production term due to buoyancy in k and epsilon equations. So I can make the new turbulence model by defining the coefficients and gravitational acceleration which are needed for calculating the buoyancy production. But I have no idea how should I do the procedure to make the modified k-epsilon model read the scalar values from the case?!?
In brief:
production due to buoyancy=Gb=beta*C3e*g*(dS/dy)


Problem is dS/dy , S is the scalar filed which is advected in the domain by velocity.

Best REGARDS:)

sinatahmooresi October 23, 2018 10:12

Quote:

Originally Posted by sinatahmooresi (Post 711948)
Hi dear FOAMers!
I want to add the gradient of a scalar filed (like S) for calculation the production term due to buoyancy in k and epsilon equations. So I can make the new turbulence model by defining the coefficients and gravitational acceleration which are needed for calculating the buoyancy production. But I have no idea how should I do the procedure to make the modified k-epsilon model read the scalar values from the case?!?
In brief:
production due to buoyancy=Gb=beta*C3e*g*(dS/dy)


Problem is dS/dy , S is the scalar filed which is advected in the domain by velocity.

Best REGARDS:)




nothing?:confused::confused:

clapointe October 25, 2018 20:41

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

sinatahmooresi October 26, 2018 03:03

Quote:

Originally Posted by clapointe (Post 712698)
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

Hi Clealan!
Thank you for your help. I am already dealing with that. My another question is about the thermal expansion coefficient which is appearing in buoyancy tern (G) called beta. Is there any equivalent for this beta for scalar flux?? Because most of the literature is devoted to thermal plume and beta is adopted for buoyancy due to non-zero temperature gradient field.
Regards Sina.


G=(beta)*gi*(nut/Prt)*(DT/Dxi).
T is temperature or scalar filed. But beta is only defined for temperature not any scalar

mAlletto October 26, 2018 06:04

Quote:

Originally Posted by sinatahmooresi (Post 711948)
Hi dear FOAMers!
I want to add the gradient of a scalar filed (like S) for calculation the production term due to buoyancy in k and epsilon equations. So I can make the new turbulence model by defining the coefficients and gravitational acceleration which are needed for calculating the buoyancy production. But I have no idea how should I do the procedure to make the modified k-epsilon model read the scalar values from the case?!?
In brief:
production due to buoyancy=Gb=beta*C3e*g*(dS/dy)


Problem is dS/dy , S is the scalar filed which is advected in the domain by velocity.

Best REGARDS:)

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

if you have defined the scalarField somewhere you can retrieve it with the above function

sinatahmooresi October 27, 2018 08:40

Quote:

Originally Posted by mAlletto (Post 712798)
const volScalarField& S_ = U_.mesh().lookupObject<volScalarField>("S");

if you have defined the scalarField somewhere you can retrieve it with the above function

Hi Michael Alletto!
thank you for your answer yes exactly i figured this out. but do you have any idea about what i asked in my response to another friend Clealan:


My another question is about the thermal expansion coefficient which is appearing in buoyancy tern (G) called beta. Is there any equivalent for this beta for scalar flux?? Because most of the literature is devoted to thermal plume and beta is adopted for buoyancy due to non-zero temperature gradient field.
Regards Sina.


G=(beta)*gi*(nut/Prt)*(DT/Dxi).
T is temperature or scalar filed. But beta is only defined for temperature not any scalar

mAlletto October 27, 2018 12:36

Which scalar are you interested in? The term accounting for the buoyancy production in the k equation comes into the equation when the buoyancy is present also in the momentum equation. If one derives the equation for k from the momentum equation with the term accounting for the buoyancy one gets the terrm rho* beta * gi * ui'T'. So if you try to derive the k equation from the momentum equation with your scalar you should see which constant you need instead of beta.

sinatahmooresi October 27, 2018 12:52

Quote:

Originally Posted by mAlletto (Post 712982)
Which scalar are you interested in? The term accounting for the buoyancy production in the k equation comes into the equation when the buoyancy is present also in the momentum equation. If one derives the equation for k from the momentum equation with the term accounting for the buoyancy one gets the terrm rho* beta * gi * ui'T'. So if you try to derive the k equation from the momentum equation with your scalar you should see which constant you need instead of beta.

Dear Michael!
Thank you for your response again, I understand the general formulation of buoyancy and its relation with momentum equations. But the question is still remaining. My scalar filed is Salinity which is entering the domain due to momentum as a jet flow. So the density is affected by salinity with the Millero-Poission eqn of state (P=f(S,T)). So what should I do for beta, when I am dealing with salinity concentration as a scalar of my domain?
Regards

mAlletto October 27, 2018 14:39

A ok I got it. Ok the beta in the momentum equtions comes from the Boussinesq Approximation, i.e. you linearize the density around a a given value and expand it as a function of temperature. The same could be done for the salinity: you can expend it around a given salinity value (see http://www.o3d.org/eas-ocean-modelin...3-EqMotion.pdf)

so i assume you can substitude the coefficient of termal expansion beta by the coeffcient of salinity concentration, i.e

\frac{\partial \rho}{\partial S}|_T

this is what I assume after a short search about change of density as a function of salinity.

Hope this is usefull

sinatahmooresi October 28, 2018 02:47

Quote:

Originally Posted by mAlletto (Post 712995)
A ok I got it. Ok the beta in the momentum equtions comes from the Boussinesq Approximation, i.e. you linearize the density around a a given value and expand it as a function of temperature. The same could be done for the salinity: you can expend it around a given salinity value (see http://www.o3d.org/eas-ocean-modelin...3-EqMotion.pdf)

so i assume you can substitude the coefficient of termal expansion beta by the coeffcient of salinity concentration, i.e

\frac{\partial \rho}{\partial S}|_T

this is what I assume after a short search about change of density as a function of salinity.

Hope this is usefull


Hi!
Thank you for your research and quick response. I got your hints. Actually I am testing the results of this approach now. So for every specific scalar in a domain one should go after finding the relation between rho and that specific scalar to find a similar manner of beta? Is that true?
Regards, Sina.

mAlletto October 29, 2018 03:41

In some manner. You should really write down the derivation of the transport equation for the turbulent kinetic energy equation considering buoyancy to understand if everything is correct (see e.g. https://www.cambridge.org/core/books...A39631674EC3C9).

In principle what you do if you have a source term in the momentum equation: Source = C * S_i(x,y,z) you decompose it into mean and fluctuation and multiply it with the velocity velocity fluctuation and you end up something like this: SourceTKE = C * < S_i'(x,y,z) u_i' >

sinatahmooresi October 29, 2018 04:14

Quote:

Originally Posted by mAlletto (Post 713309)
In some manner. You should really write down the derivation of the transport equation for the turbulent kinetic energy equation considering buoyancy to understand if everything is correct (see e.g. https://www.cambridge.org/core/books...A39631674EC3C9).

In principle what you do if you have a source term in the momentum equation: Source = C * S_i(x,y,z) you decompose it into mean and fluctuation and multiply it with the velocity velocity fluctuation and you end up something like this: SourceTKE = C * < S_i'(x,y,z) u_i' >

thnaks a lot. I will go further with your helps and hints and I will notice the results here again.
Regards Sina

mAlletto October 29, 2018 05:38

Just one question out of curiosity:

What are the applications you are doing the modeling?

sinatahmooresi October 30, 2018 08:37

Quote:

Originally Posted by mAlletto (Post 713327)
Just one question out of curiosity:

What are the applications you are doing the modeling?

of coures. I am working on neagitve buoyant jets which are buoaynat due to salinity of the jet.
can I ask another question ? I want to make a if statement with < and > :
if ( a> ...)

do...
else
do...
but the error is concerned about "<" and ">" and value which I entroduced for comparison :a> 0 (the zero)! how come?
I am doing this in the .C of my solver.

the last part of the error is :
' Foam:: tmp<Foam::GeomtericField<double, Foam::fvpatchField, Foam::volMesh> >' is not derived from 'const Foam::Pair <Type>'
Regards Sina

mAlletto October 30, 2018 08:49

Form the short code you sent i presume you want to compare a volumetric viele with a float. But hard to say without and code.

sinatahmooresi October 30, 2018 09:11

Quote:

Originally Posted by mAlletto (Post 713532)
Form the short code you sent i presume you want to compare a volumetric viele with a float. But hard to say without and code.

More specific:



if (U.component(1) > 0)

var1=1.0;
else

var1=0.5;




and I want to consider U.component(1) as Uy (U.component(1)=Uy) of velocity field.
Regards Sina

mAlletto October 30, 2018 10:13

What you are doing ist comparing a volScalarField with a float.

You should write

Code:

forAll(U.component(0),Celli)
{
  If (U.component(0)[Celli] < 0)
{Do somethine}
Else
{Do something else}
}

But with a bit oft efford you will find a lot oft threads whitch deal with the topic oft Looping over fields in OF.

Michael

sinatahmooresi October 30, 2018 11:46

Quote:

Originally Posted by mAlletto (Post 713559)
What you are doing ist comparing a volScalarField with a float.

You should write

Code:

forAll(U.component(0),Celli)
{
  If (U.component(0)[Celli] < 0)
{Do somethine}
Else
{Do something else}
}

But with a bit oft efford you will find a lot oft threads whitch deal with the topic oft Looping over fields in OF.

Michael


I tried this now and I also checked the synax you wrote in other posts and discussions about forAll loops, the synax is correct but I get two error:
in brief:
..... has no member named 'size'
for (Foam::label i=; i<(list).size(); i++)


....in expansion of macro 'forAll'
forAll (U.component(1) , Celli)
^

...no match for operator []' ...
if (U.component(1)[Celli] > 0)
^

(***this ^ is under the [ ***)
Regards Sina

mAlletto October 30, 2018 12:06

Maybe
forAll (U , Celli)

U[Celli].component(0)

sinatahmooresi October 30, 2018 12:32

Quote:

Originally Posted by mAlletto (Post 713578)
Maybe
forAll (U , Celli)

U[Celli].component(0)

Thanks a lot. That was correct. solver compiled with no error:):)


All times are GMT -4. The time now is 20:43.