CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   kappatJayatillekeWallFunctionFvPatchScalarField changes between OpenFOAM 171 and 201 (http://www.cfd-online.com/Forums/openfoam-solving/93398-kappatjayatillekewallfunctionfvpatchscalarfield-changes-between-openfoam-171-201-a.html)

makaveli_lcf October 13, 2011 16:34

kappatJayatillekeWallFunctionFvPatchScalarField changes between OpenFOAM 171 and 201
 
Hi everyone!

I discovered following while simulating buoyant flow with 1.7.0 and 1.7.1 versions (Ubuntu 10.04 LTS packages from apt):

1. Comparable to 1.7.0 in version 1.7.1 kappat field is introduced in TEqn for incompressible SIMPLE and PIMPLE solvers.

v1.7.0:
Code:

{
    volScalarField kappaEff
    (
        "kappaEff",
        turbulence->nu()/Pr + turbulence->nut()/Prt
    );


    fvScalarMatrix TEqn
    (
        fvm::ddt(T)
      + fvm::div(phi, T)
      - fvm::laplacian(kappaEff, T)
    );

    TEqn.relax();
    TEqn.solve(mesh.solver(T.select(finalIter)));

    rhok = 1.0 - beta*(T - TRef);
}

v1.7.1:
Code:

{
    kappat = turbulence->nut()/Prt;
    kappat.correctBoundaryConditions();

    volScalarField kappaEff("kappaEff", turbulence->nu()/Pr + kappat);

    fvScalarMatrix TEqn
    (
        fvm::ddt(T)
      + fvm::div(phi, T)
      - fvm::laplacian(kappaEff, T)
    );

    TEqn.relax();
    TEqn.solve(mesh.solver(T.select(finalIter)));

    rhok = 1.0 - beta*(T - TRef);
}

2. For kappat field Jayatille wall function is introduced, but it has a bug in kappat calculation which is fixed in v2.0.1:

diff for kappatJayatillekeWallFunctionFvPatchScalarField.C between 1.7.1 and 2.0.1 results in

Code:

210c210
<    const scalarField& nuw = rasModel.nu().boundaryField()[patchI];
---
>    const scalarField& nuw = rasModel.nu()().boundaryField()[patchI];
238c238
<            scalar kt = nu*(yPlus/(Prt_/kappa_*log(E_*yPlusTherm) + P) - 1/Pr);
---
>            scalar kt = nu*(yPlus/(Prt_*(log(E_*yPlus)/kappa_ + P)) - 1/Pr);
264c264,268
< makePatchTypeField(fvPatchScalarField, kappatJayatillekeWallFunctionFvPatchScalarField);
---
> makePatchTypeField
> (
>    fvPatchScalarField,
>    kappatJayatillekeWallFunctionFvPatchScalarField
> );

I noticed this issue because got a floating point operation error actually coming from
log(E_*yPlusTherm) where yPlusTherm can be equal zero.

You cal also notice that parenthesis around (log(E_*yPlus)/kappa_ + P)) result in different expression
than
Prt_/kappa_*log(E_*yPlusTherm) + P.

Hope it would be helpful for someone))))

Cheers,
A.

Oke'e October 17, 2011 11:52

Please can you help me with an explanation of what rhok is?

makaveli_lcf October 17, 2011 12:34

http://en.wikipedia.org/wiki/Boussin...%28buoyancy%29

Oke'e October 19, 2011 10:06

Thanks for the prompt response. I know about the boussinesque approximation. My question is because of a case I'm setting up in OpenFOAM. I am simulating stratification in a cylindrical tank. I have modified the 'hotroom' example under the bouyantBoussinesqPimpleFoam solver and changed the entries in the 'transportProperties' file to those of water. When the run the case with the original entries (which I suspect to be for air), I get realistic results - the stratification is obvious. But when I change the properties - Pr, beta, nu, to those of water the results when viewed show no signs of stratification. Could you be of help please?

makaveli_lcf October 19, 2011 15:13

Hello Howard!

It is always better when you ask detailed questions. Because for the obvious ones you can find answers yourself and it is more useful for you to learn finding answers.

Would you please post you pictures which do not satisfy you and also the parameters which you used?

Cheers,
A.

makaveli_lcf October 19, 2011 15:41

Do you mean simulating compressible flow? Of couse for water (almost incompressible liquid) there is no such stratification as for e.g. air.

Oke'e October 24, 2011 16:58

1 Attachment(s)
Hello Dr. Alexander,

Please pardon the delay in my response. I travelled out of town without my laptop and was without access to computer facilities.

The changes I made in the transportProperties file were

nu : changed from 1e-05 to 4.5e-07 (m2sec-1)
beta: changed from 3e-03 to 5e-04 (K-1)
Pr: changed from 0.9 to 3.0
Prt: changed from 0.7 to 2.3.
Tref was left unchanged.

The RASModel keyword in the RASProperities file was changed to laminar.

In the 0/p file the wall pressures were set with the $internalField entry, while the p_rgh value was set to constant 0 in the 0/p_rgh file.

You'll see from the attached picture that there is no evidence of stratification. Stratification is obtainable in incompressible flows (the 'buoyantBoussinesqPimpleFoam' solver is for "Transient solver for buoyant, turbulent flow of incompressible fluids" according to the user guide.) This is the basis for stratified hot water storages which is what I'm trying to study.

Howard

chiragomshanti January 14, 2012 11:27

kappatw instead of kappat?
 
Dear Dr.Alexander,
In the file "kappatJayatillekeWallFunctionFvPatchScalarField.C" kappatw shouldn't be kappat? I searched much, but didn't find any use of kappatw.
With Regards,
Chirag Patel

mabinty January 31, 2012 15:48

dear all,

i wonder why the JayatillekeWallFunction is not available for the the calculation of alphat in the compressible RANS version. for now, in the compressible version alphat is evaluated as mut/Prt at the wall. i m thinking of implementing the procedure of the JayatillekeWallFunction for compressible RANS in alphatWallFunctions.

does it make sens or is
alphatw = mutw/Prt resonable anyway??

@
Chirag Patel

kappatw is taken from the expression

Code:

scalarField& kappatw = *this;
thanks in advance for your input!

cheers,
aram

mabinty February 1, 2012 04:25

hi,

I though about something like this:

Code:

// Populate boundary values
scalarField& alphatw = *this;

forAll(alphatw, faceI)
{
      [ ... ]

        if (yPlus > yPlusTherm)
        {
            scalar mu = muw[faceI];
            scalar at = mu*(yPlus/(Prt_*(log(E_*yPlus))/kappa_ + P) - 1/Pr);
            alphatw[faceI] = max(0.0, at);
        }
        else
        {
            alphatw[faceI] = 0.0;
        }

in turbulenceModels/compressible/RAS/derivedFvPatchFields/wallFunctions/alphatWallFunctions/alphatWallFunction/alphatWallFunctionFvPatchScalarField.C (OF 1.7.1)

cheers,
Aram

makaveli_lcf February 1, 2012 05:53

hi Aram!

you are right) But I found an implementation in version OF 2.10:

see http://foam.sourceforge.net/docs/cpp...ce.html#l00195

Code:

00195 void alphatJayatillekeWallFunctionFvPatchScalarField::updateCoeffs()
00196 {
00197    if (updated())
00198    {
00199        return;
00200    }
00201
00202    const label patchI = patch().index();
00203
00204    const RASModel& rasModel = db().lookupObject<RASModel>("RASProperties");
00205
00206    const scalar Cmu25 = pow025(Cmu_);
00207
00208    const scalarField& y = rasModel.y()[patchI];
00209
00210    const scalarField& muw = rasModel.mu().boundaryField()[patchI];
00211
00212    const scalarField& alphaw = rasModel.alpha().boundaryField()[patchI];
00213    scalarField& alphatw = *this;
00214
00215    const tmp<volScalarField> tk = rasModel.k();
00216    const volScalarField& k = tk();
00217
00218    const fvPatchVectorField& Uw = rasModel.U().boundaryField()[patchI];
00219    const scalarField magUp(mag(Uw.patchInternalField() - Uw));
00220    const scalarField magGradUw(mag(Uw.snGrad()));
00221
00222    const scalarField& rhow = rasModel.rho().boundaryField()[patchI];
00223    const fvPatchScalarField& hw =
00224        rasModel.thermo().h().boundaryField()[patchI];
00225
00226    // Heat flux [W/m2] - lagging alphatw
00227    const scalarField qDot((alphaw + alphatw)*hw.snGrad());
00228
00229    // Populate boundary values
00230    forAll(alphatw, faceI)
00231    {
00232        label faceCellI = patch().faceCells()[faceI];
00233
00234        scalar uTau = Cmu25*sqrt(k[faceCellI]);
00235
00236        scalar yPlus = uTau*y[faceI]/(muw[faceI]/rhow[faceI]);
00237
00238        // Molecular Prandtl number
00239        scalar Pr = muw[faceI]/alphaw[faceI];
00240
00241        // Molecular-to-turbulent Prandtl number ratio
00242        scalar Prat = Pr/Prt_;
00243
00244        // Thermal sublayer thickness
00245        scalar P = Psmooth(Prat);
00246        scalar yPlusTherm = this->yPlusTherm(P, Prat);
00247
00248        // Evaluate new effective thermal diffusivity
00249        scalar alphaEff = 0.0;
00250        if (yPlus < yPlusTherm)
00251        {
00252            scalar A = qDot[faceI]*rhow[faceI]*uTau*y[faceI];
00253            scalar B = qDot[faceI]*Pr*yPlus;
00254            scalar C = Pr*0.5*rhow[faceI]*uTau*sqr(magUp[faceI]);
00255            alphaEff = A/(B + C + VSMALL);
00256        }
00257        else
00258        {
00259            scalar A = qDot[faceI]*rhow[faceI]*uTau*y[faceI];
00260            scalar B = qDot[faceI]*Prt_*(1.0/kappa_*log(E_*yPlus) + P);
00261            scalar magUc = uTau/kappa_*log(E_*yPlusTherm) - mag(Uw[faceI]);
00262            scalar C =
00263                0.5*rhow[faceI]*uTau
00264                *(Prt_*sqr(magUp[faceI]) + (Pr - Prt_)*sqr(magUc));
00265            alphaEff = A/(B + C + VSMALL);
00266        }
00267
00268        // Update turbulent thermal diffusivity
00269        alphatw[faceI] = max(0.0, alphaEff - alphaw[faceI]);
00270
00271        if (debug)
00272        {
00273            Info<< "    uTau          = " << uTau << nl
00274                << "    Pr            = " << Pr << nl
00275                << "    Prt            = " << Prt_ << nl
00276                << "    qDot          = " << qDot[faceI] << nl
00277                << "    yPlus          = " << yPlus << nl
00278                << "    yPlusTherm    = " << yPlusTherm << nl
00279                << "    alphaEff      = " << alphaEff << nl
00280                << "    alphaw        = " << alphaw[faceI] << nl
00281                << "    alphatw        = " << alphatw[faceI] << nl
00282                << endl;
00283        }
00284    }
00285
00286    fixedValueFvPatchField<scalar>::updateCoeffs();
00287 }
00288

I didn't go into details, but I think you can use it. It would be nice if you comment on what is the differece between what you suggest (I also would write similar code).

Cheers,
Alex

mabinty February 1, 2012 09:26

hi Alex,

thanks for the hint (still using OF 1.7). I had a look on the implementation of OF 2.1. Three main differences in the why how i proposed it:

1) alphat isnt set to zero for yPlus < yPlusLam, but I couldn t find a reference so far were the equation comes from
2) The BC calculates alphaEff and updates alphat by subtracting alpha (laminar)
3) For yPlus > yPlusLam the calculation of alphaEff differs from the version I proposed by an additional term in the denominator which contains velocities (which I couldn t find out yet where it comes from):

Code:


alphaEff = mu*(yPlus/(Pr_t*log(E *yPlus)/kappa_ + 0.5*rhow*uTau*(Pr_t*sqr(mag(Up)) + (Pr_t - Pr)*sqr(mag(Uc)))))

For yPlus < yPlusLam a similar term can be found. I was searching for a reference on that but couldn t find one so far. Any comments on that are appreciated!! I think I will give it a try in OF 1.7 anyway.

cheers,
Aram

makaveli_lcf February 1, 2012 09:34

Hi,

those additional terms are for compressible flow, thus there are none of them in incompressible BC version. Check for the full version:

http://my.fit.edu/itresources/manual...pdf/flu_th.pdf, (page 124)

Sorry for the wrong link to the Theory Guide)

Cheers!

mabinty February 1, 2012 11:44

That s great! Got it now!!

Thanks again!!

Cheers,
Aram

vahid.najafi July 29, 2012 02:01

help me plz
 
Hi every foamers.

I want to add k(kinetic turbulence energy) in one solver.

for this work, added next line in the code of solver:

const volScalarField &k=U_.db().lookupObject<volScalarField>("k")
and wmake was Successfully .

but How can I Understand that this k is the same with k(kinetic turbulence energy)???Is it true?????or not????

Because I replase another word in this :

const volScalarField &M=U_.db().lookupObject<volScalarField>("M")
but nothing error was not occured!!!!!!??????

makaveli_lcf July 29, 2012 04:33

Could the lookup method just give you a null pointer, then no error is detected

vahid.najafi July 29, 2012 04:46

Thanks
 
Thanks Dr. Alexander A. Vakhrushev for your answer.

its means this work not true???this k is not kinetic turbulence energy???
if your answer yes!!!Please suggest me one way to Correction this code with k(kinetic turbulence energy)!!!

makaveli_lcf July 29, 2012 04:51

Could you show more information, e.g.post your solver (if it is not secret) to understand your problem. Actually it should be ok what yo use to get k field.

vahid.najafi July 29, 2012 05:28

my solver is in Appendix
 
1 Attachment(s)
Thanks for your answer Dr.
it is not secret!!!:)
my solver is in Appendix.I want to added kinetic turbulence energy in Directory:
OpenFOAM/vahid 2.0.1/run/myinterPhaseChangeFoam/phaseChangeTwoPhaseMixtures/SchnerrSauer/SchnerrSauer.c
in file:SchnerrSauer.c

I have add (turbulence kinetic Energy or k ) in a part of this solver.
first:
added:
-I$(LIB_SRC)/turbulenceModels \
-I$(LIB_SRC)/turbulenceModels/incompressible/RAS/RASModel \

in option.


and then:
added
//.................................................. .....changed
// Construct incompressible turbulence model
autoPtr<incompressible::RASModel> turbulence
(
incompressible::RASModel::New(U, phi, twoPhaseProperties())
);
//.................................................. .....changed


in creatField.

and then:
added

#include "RASModel.H"
and:

//.................................................. .............
volScalarField turbKinEnergy = turbulence().k(); //turbKinEnergy = turbulence().k();
volScalarField turbDisEnergy = turbulence().epsilon();
in this and turbkinEnergy=k
//.................................................. .............


in myinterPhaseChangeFoam.c

and wmake is ok!!!



but
I want in this solver in directory:
/run/myinterPhaseChangeFoam/phaseChangeTwoPhaseMixtures/SchnerrSauer/SchnerrSauer.c




I added
#include "RASModel.H"

in it and:


Foam::tmp<Foam::volScalarField>
Foam::phaseChangeTwoPhaseMixtures::SchnerrSauer::p Coeff
(
const volScalarField& p
) const
{
volScalarField limitedAlpha1(min(max(alpha1_, scalar(0)), scalar(1)));
volScalarField rho
(
limitedAlpha1*rho1() + (scalar(1) - limitedAlpha1)*rho2()
);

return
//......I want to change it( <<k>> turbulence multiple in it):
(3*rho1()*rho2())*sqrt(2/(3*rho1()))*k()
*rRb(limitedAlpha1)/(rho*sqrt(mag(p - pSat()) + 0.01*pSat()));
//.................................................. ......
}


dont successful wmake, and seen(was not declared ):

I/opt/openfoam201/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/SchnerrSauer.o
phaseChangeTwoPhaseMixtures/SchnerrSauer/SchnerrSauer.C: In member function ‚€کFoam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::phaseChangeTwoPhaseMixtures::SchnerrSauer::p Coeff(const Foam::volScalarField&) const‚€™:
phaseChangeTwoPhaseMixtures/SchnerrSauer/SchnerrSauer.C:113: error: k() was not declared in this scope
make: *** [Make/linux64GccDPOpt/SchnerrSauer.o] Error 1


please help me.

another way that I worked:


Foam::tmp<Foam::volScalarField>
Foam:haseChangeTwoPhaseMixtures::SchnerrSauer: Coeff
(
const volScalarField& p
) const
{
volScalarField limitedAlpha1(min(max(alpha1_, scalar(0)), scalar(1)));
volScalarField rho
(
limitedAlpha1*rho1() + (scalar(1) - limitedAlpha1)*rho2()
);

return
const volScalarField &k=U_.db().lookupObject<volScalarField>("k");

(3*rho1()*rho2())*sqrt(2/(3*rho1()))*k()
*rRb(limitedAlpha1)/(rho*sqrt(mag(p - pSat()) + 0.01*pSat()));


and wmake was Successfully .

but How can I Understand that this k is the same with k(kinetic turbulence energy)???Is it true???
Because I replase another world in this :
const volScalarField &M=U_.db().lookupObject<volScalarField>("M")
but not error occured!!!!!!??????


please help me more about this problem????Thanks.

camoesas February 24, 2014 09:57

Hello Everybody,

I am exhuming this thread because it is the only one were somebody talks about yPlustherm. So maybe the Pro's see their old thread poping up and somebody can give me a reply:

I am working with the above mentioned wall function. What I dont understand is the calculation of yPlustherm. The docu says it is the value of yPlus at the edge of the thermal laminar sublayer. But where does the formula come from:

Code:

00084        scalar f = ypt - (log(E_*ypt)/kappa_ + P)/Prat;
00085        scalar df = 1.0 - 1.0/(ypt*kappa_*Prat);
00086        scalar yptNew = ypt - f/df;

Fluent uses a similar alphajayatillekewallfunction but says that yPlusTherm is the point where the linear and the log law intersect.
So my question is: What is yPlustherm and whats the background for this formula?
So I would be gratefull if somebody could lift the fog.


Thanks!

Camoesas


All times are GMT -4. The time now is 11:55.