CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Post-Processing

wallHeatFlux utility with sonicFoam

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 27, 2015, 10:06
Default wallHeatFlux utility with sonicFoam
  #1
Senior Member
 
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13
hiuluom is on a distinguished road
Hi everybody,

When I tried wallHeatFlux the buoyantSimpleFoam OF 2.1.1 in hotroom tutorial it was no problem with thermotype:

Code:
thermoType      hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>;

pRef            100000;

mixture
{
    specie
    {
        nMoles          1;
        molWeight       28.9;
    }
    thermodynamics
    {
        Cp              1000;
        Hf              0;
    }
    transport
    {
        mu              1.8e-05;
        Pr              0.7;
    }
}
But in sonicFoam with prism tutorial has difference thermo:

Code:
thermoType      ePsiThermo<pureMixture<constTransport<specieThermo<eConstThermo<perfectGas>>>>>;

mixture
{
    specie
    {
        nMoles          1;
        molWeight       28.9;
    }
    thermodynamics
    {
        Cv              717.5;
        Hf              0;
    }
    transport
    {
        mu              1.8e-05;
        Pr              0.7;
    }
}
I used the wallHeatFluxRho and wallHeatflux (default) which was provide in forum, OF 2.1.1 and had been a problem:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : wallHeatFlux -latestTime
Date   : Jul 25 2015
Time   : 06:53:06
Host   : "CompEng"
PID    : 2979
Case   : /home/huynh/OpenFOAM/huynh-2.1.1/run/prism
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create mesh for time = 0.0003
Time = 0.0003
Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo<eConstThermo<perfectGas>>>>>

--> FOAM FATAL ERROR: 
Not implemented
    From function basicThermo::h()
    in file basicThermo/basicThermo.C at line 260.
FOAM aborting
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libOpenFOAM.so"
#2  Foam::basicThermo::h() in "/opt/openfoam211/platforms/linuxGccDPOpt/lib/libbasicThermophysicalModels.so"
#3  
 in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/wallHeatFlux"
#4  __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#5  
 in "/opt/openfoam211/platforms/linuxGccDPOpt/bin/wallHeatFlux"
Aborted
therefore, I copy the thermotype from buoyantSimpleFoam to sonicFoam calculation wallHeatFlux again. It was run but the result equal to zero.

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : wallHeatFluxRho -latestTime
Date   : Jul 25 2015
Time   : 22:05:09
Host   : "CompEng"
PID    : 4590
Case   : /home/huynh/OpenFOAM/huynh-2.1.1/run/prism
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0.0003

Time = 0.0003
Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>
Reading/calculating face flux field phi

Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    sigmak          1;
    sigmaEps        1.3;
    Prt             1;
}


Wall heat fluxes [W]
prismWall 0

End
I saw the source code wallHeatFlux which was compute by gradient of enthalpy h corresponding hPsiThermo. Otherwise, the ePsiThermo with internal energy e was not described in equation wallHeatFlux. I replace the enthalpy h by internal energy e and compile it unsuccessful.

Code:
fvc::interpolate(RASModel->alphaEff())*fvc::snGrad(h)
I would like to calculate wallHeatFlux for sonicFoam but it cannot. Could anybody can show me the solve for this, please?

Thank you so much
hiuluom is offline   Reply With Quote

Old   August 20, 2015, 00:34
Default
  #2
Senior Member
 
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13
hiuluom is on a distinguished road
Hi everybody,

I modified the wallHeatFlux that can be calculated for ePsithermo. Here is the code:
WallHeatFlux.C
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

Application
    wallHeatFlux

Description
    Calculates and writes the heat flux for all patches as the boundary field
    of a volScalarField and also prints the integrated flux for all wall
    patches.

\*---------------------------------------------------------------------------*/

#include "fvCFD.H"
#include "hCombustionThermo.H"
#include "basicPsiThermo.H"
#include "RASModel.H"
#include "turbulenceModel.H"
#include "wallFvPatch.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

int main(int argc, char *argv[])
{
    timeSelector::addOptions();
#   include "addRegionOption.H"
    #include "setRootCase.H"
    #include "createTime.H"
    instantList timeDirs = timeSelector::select0(runTime, args);
    #include "createNamedMesh.H"

    forAll(timeDirs, timeI)
    {
        runTime.setTime(timeDirs[timeI], timeI);
        Info<< "Time = " << runTime.timeName() << endl;
        mesh.readUpdate();

        #include "createFields.H"

        surfaceScalarField heatFlux
        (
            fvc::interpolate(turbulence->alphaEff())*fvc::snGrad(e)
        );

        const surfaceScalarField::GeometricBoundaryField& patchHeatFlux =
            heatFlux.boundaryField();

        Info<< "\nWall heat fluxes [W]" << endl;
        forAll(patchHeatFlux, patchi)
        {
            if (isA<wallFvPatch>(mesh.boundary()[patchi]))
            {
                Info<< mesh.boundary()[patchi].name()
                    << " "
                    << gSum
                       (
                           mesh.magSf().boundaryField()[patchi]
                          *patchHeatFlux[patchi]
                       )
                    << endl;
            }
        }
        Info<< endl;

        volScalarField wallHeatFlux
        (
            IOobject
            (
                "wallHeatFlux",
                runTime.timeName(),
                mesh
            ),
            mesh,
            dimensionedScalar("wallHeatFlux", heatFlux.dimensions(), 0.0)
        );

        forAll(wallHeatFlux.boundaryField(), patchi)
        {
            wallHeatFlux.boundaryField()[patchi] = patchHeatFlux[patchi];
        }

        wallHeatFlux.write();
    }

    Info<< "End" << endl;

    return 0;
}

// ************************************************************************* //
And createFields.H
Code:
    Info<< "Reading thermophysical properties\n" << endl;

    autoPtr<basicPsiThermo> pThermo
    (
        basicPsiThermo::New(mesh)
    );
    basicPsiThermo& thermo = pThermo();

    //volScalarField& p = thermo.p();
    volScalarField& e = thermo.e();
    //const volScalarField& psi = thermo.psi();

    volScalarField rho
    (
        IOobject
        (
            "rho",
            runTime.timeName(),
            mesh
        ),
        thermo.rho()
    );

    Info<< "Reading field U\n" << endl;
    volVectorField U
    (
        IOobject
        (
            "U",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    );

    #include "compressibleCreatePhi.H"


    Info<< "Creating turbulence model\n" << endl;
    autoPtr<compressible::turbulenceModel> turbulence
    (
        compressible::turbulenceModel::New
        (
            rho,
            U,
            phi,
            thermo
        )
    );
Then the result with my nozzle tube in example ran sonicFoam
Code:
Create time

Create mesh for time = 0.0090052

Time = 0.0090052
Reading thermophysical properties

Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo<eConstThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type RASModel
Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
    alphaK1         0.85034;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.85616;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    gamma1          0.05532;
    gamma2          0.4403;
    a1              0.31;
    c1              10;
    Prt             1;
}


Wall heat fluxes [W]
bottom_heat -104748
But it has been difference with wallHeatFlux default in OF and replace epsiThermo by hpsiThermo.
Code:
Create time

Create mesh for time = 0.0090052

Time = 0.0090052
Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>
Reading/calculating face flux field phi

Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
    alphaK1         0.85034;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.85616;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    gamma1          0.05532;
    gamma2          0.4403;
    a1              0.31;
    c1              10;
    Prt             1;
}


Wall heat fluxes [W]
bottom_heat -146611

End

Last edited by hiuluom; September 18, 2015 at 07:44.
hiuluom is offline   Reply With Quote

Old   September 18, 2015, 00:33
Default
  #3
Senior Member
 
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13
hiuluom is on a distinguished road
Dear all,

I know the difference result as I mention above. That is wrong at formula calculate heat flux in *.C. I check with paraview this formula after computing heat flux with ePsiThermo

wallHeatFlux*(Cp/Cv)

It will the same result when calculate heat flux with hPsiThermo. And then I modified the code wallHeatFlux.C by

Code:
//molecular weight number
		// scalar W(thermo.lookup("molWeight"));

		//Heat capacity
		// scalar Cv(thermo.lookup("Cv"));

        surfaceScalarField heatFlux
        (
            fvc::interpolate(turbulence->alphaEff())*(W + 8314/(Cv*W))*fvc::snGrad(e)
        );
I have error because OF cannot look up molWeight and Cv in thermoPhysicalProperties file
Code:
Making dependency list for source file wallHeatFluxCompressible.C
SOURCE=wallHeatFluxCompressible.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I.. -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/turbulenceModels     -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/turbulenceModels/compressible/turbulenceModel -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/reactionThermo/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/basic/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.1.1/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/wallHeatFluxCompressible.o
In file included from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/Field.H:360:0,
                 from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/labelField.H:39,
                 from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/primitiveFields.H:37,
                 from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/pointField.H:36,
                 from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/edge.H:40,
                 from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/edgeList.H:32,
                 from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/primitiveMesh.H:57,
                 from /opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/polyMesh.H:44,
                 from /opt/OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/lnInclude/fvMesh.H:50,
                 from /opt/OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/lnInclude/fvCFD.H:7,
                 from wallHeatFluxCompressible.C:34:
/opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/Field.C: In member function ‘void Foam::Field<Type>::operator=(const Foam::VectorSpace<Form, Cmpt, nCmpt>&)’:
/opt/OpenFOAM/OpenFOAM-2.1.1/src/OpenFOAM/lnInclude/Field.C:680:42: warning: typedef ‘VSType’ locally defined but not used [-Wunused-local-typedefs]
     typedef VectorSpace<Form,Cmpt,nCmpt> VSType;
                                          ^
In file included from /opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/eConstThermo.H:214:0,
                 from wallHeatFluxCompressible.C:36:
/opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/eConstThermoI.H: In member function ‘Foam::scalar Foam::eConstThermo<EquationOfState>::cp(Foam::scalar) const’:
/opt/OpenFOAM/OpenFOAM-2.1.1/src/thermophysicalModels/specie/lnInclude/eConstThermoI.H:108:28: error: ‘specie’ has not been declared
     return Cv_*this->W() + specie::RR;
                            ^
wallHeatFluxCompressible.C: In function ‘int main(int, char**)’:
wallHeatFluxCompressible.C:61:24: error: missing template arguments before ‘.’ token
   scalar W(eConstThermo.lookup("molWeight"));
                        ^
wallHeatFluxCompressible.C:64:25: error: missing template arguments before ‘.’ token
   scalar Cv(eConstThermo.lookup("Cv"));
                         ^
wallHeatFluxCompressible.C:61:10: warning: unused variable ‘W’ [-Wunused-variable]
   scalar W(eConstThermo.lookup("molWeight"));
          ^
wallHeatFluxCompressible.C:64:10: warning: unused variable ‘Cv’ [-Wunused-variable]
   scalar Cv(eConstThermo.lookup("Cv"));
          ^
make: *** [Make/linux64GccDPOpt/wallHeatFluxCompressible.o] Error 1
Someone can help me how to call Cv and molWeight in *.C

Thank you,
Thanh
hiuluom is offline   Reply With Quote

Old   September 18, 2015, 07:39
Default
  #4
Senior Member
 
Huynh Phong Thanh
Join Date: Aug 2013
Location: Ho Chi Minh City
Posts: 105
Rep Power: 13
hiuluom is on a distinguished road
Finally, I compiled successfully wall heat flux for "ePsiThermo" thermal type for sonicFoam or rhoCentralFoam. Here is the code:

for "createFields.h"
Code:
Info<< "Reading thermophysical properties\n" << endl;

    autoPtr<basicPsiThermo> pThermo
    (
        basicPsiThermo::New(mesh)
    );
    basicPsiThermo& thermo = pThermo();
	
    //volScalarField& p = thermo.p();
    const volScalarField& e = thermo.e();
	
	const objectRegistry& db = mesh.thisDb();
	
	//const IOdictionary& thermoProps = db.lookupObject<IOdictionary>("thermophysicalProperties");
	
	const dictionary& thermoProps =
        db.lookupObject<IOdictionary>("thermophysicalProperties");
	
	dictionary mixture
		(
			thermoProps.subDict("mixture")
		);
	dictionary specie
		(
			mixture.subDict("specie")
		);
	dictionary thermodynamics
		(
			mixture.subDict("thermodynamics")
		);
	const scalar Cv =
        readScalar(thermodynamics.lookup("Cv"));
		
	const scalar W =
        readScalar(specie.lookup("molWeight"));
	
	//double gamma = (Cv + 8314/(Cv*W));
		
	//const volScalarField& Cv = thermo.Cv();
	//const volScalarField& h = thermo.h();
    //const volScalarField& psi = thermo.psi();

    volScalarField rho
    (
        IOobject
        (
            "rho",
            runTime.timeName(),
            mesh
        ),
        thermo.rho()
    );

    Info<< "Reading field U\n" << endl;
    volVectorField U
    (
        IOobject
        (
            "U",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    );

    #include "compressibleCreatePhi.H"


    Info<< "Creating turbulence model\n" << endl;
    autoPtr<compressible::turbulenceModel> turbulence
    (
        compressible::turbulenceModel::New
        (
            rho,
            U,
            phi,
            thermo
        )
    );
for "wallHeatFLux.C"

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

Application
    wallHeatFlux

Description
    Calculates and writes the heat flux for all patches as the boundary field
    of a volScalarField and also prints the integrated flux for all wall
    patches.

\*---------------------------------------------------------------------------*/

#include "fvCFD.H"
#include "hCombustionThermo.H"
#include "basicPsiThermo.H"
#include "turbulenceModel.H"
#include "wallFvPatch.H"


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

int main(int argc, char *argv[])
{
    timeSelector::addOptions();
#   include "addRegionOption.H"
    #include "setRootCase.H"
    #include "createTime.H"
    instantList timeDirs = timeSelector::select0(runTime, args);
    #include "createNamedMesh.H"
	
    forAll(timeDirs, timeI)
    {
        runTime.setTime(timeDirs[timeI], timeI);
        Info<< "Time = " << runTime.timeName() << endl;
        mesh.readUpdate();

        #include "createFields.H"
				
        surfaceScalarField heatFlux
        (
            fvc::interpolate(turbulence->alphaEff())*(1 + 8314/(Cv*W))*fvc::snGrad(e)
        );

        const surfaceScalarField::GeometricBoundaryField& patchHeatFlux =
            heatFlux.boundaryField();

        Info<< "\nWall heat fluxes [W]" << endl;
        forAll(patchHeatFlux, patchi)
        {
            if (isA<wallFvPatch>(mesh.boundary()[patchi]))
            {
               Info<< mesh.boundary()[patchi].name()
                    << ": Total "
                    << sum
                       (
                           mesh.magSf().boundaryField()[patchi]
                          *patchHeatFlux[patchi]
                       )
                    << " [W] over "
                    << sum
                       (
                           mesh.magSf().boundaryField()[patchi]
                       )
                    << " [m2] ("
                    << sum
                       (
                           mesh.magSf().boundaryField()[patchi]
                          *patchHeatFlux[patchi]
                       )/
                       sum 
                       (
                           mesh.magSf().boundaryField()[patchi]
                       )
                    << " [W/m2])"
                    << endl;
            }
        }
        Info<< endl;

        volScalarField wallHeatFlux
        (
            IOobject
            (
                "wallHeatFlux",
                runTime.timeName(),
                mesh
            ),
            mesh,
            dimensionedScalar("wallHeatFlux", heatFlux.dimensions(), 0.0)
        );

        forAll(wallHeatFlux.boundaryField(), patchi)
        {
            wallHeatFlux.boundaryField()[patchi] = patchHeatFlux[patchi];
        }

        wallHeatFlux.write();
    }

    Info<< "End" << endl;

    return 0;
}

// ************************************************************************* //
This result have not been difference with "hPsiThermo" thermal type in section 2 above

Code:
Create time

Create mesh for time = 0.0090052

Time = 0.0090052
Reading thermophysical properties

Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo<eConstThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type RASModel
Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
    alphaK1         0.85034;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.85616;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    gamma1          0.05532;
    gamma2          0.4403;
    a1              0.31;
    c1              10;
    Prt             1;
}


Wall heat fluxes [W]
bottom_heat: Total -146673 [W] over 0.00909676 [m2] (-1.61237e+07 [W/m2])

End
I got much more time to discover this problem because I must do other simulations.

Best regards,
Thanh
hiuluom is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
wallHeatFlux utility for an incompressible case Mr.Jingles OpenFOAM Post-Processing 67 April 6, 2023 03:25
wrong calculation of wallHeatFlux utility in solid patches zfaraday OpenFOAM Post-Processing 6 January 12, 2016 16:39
Something doens't work with wallHeatFlux utility or externalWallHeatFluxTemperat BC!! zfaraday OpenFOAM Post-Processing 0 February 5, 2015 16:47
wallHeatFlux utility and chtMultiRegionFoam solver Lada OpenFOAM Post-Processing 4 June 7, 2012 09:46
wallHeatFlux utility in OpenFoam1.6 maruthamuthu_venkatraman OpenFOAM 29 October 3, 2011 10:43


All times are GMT -4. The time now is 00:27.