CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

Adding new model to transportProperties

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

Like Tree2Likes
  • 1 Post By agustinvo
  • 1 Post By agustinvo

Reply
 
LinkBack Thread Tools Display Modes
Old   November 4, 2015, 04:45
Default Adding new model to transportProperties
  #1
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Brussels
Posts: 165
Rep Power: 7
agustinvo is on a distinguished road
Hello everyone

I want to create a model to include inside the transportModel the thermal diffusivity, as it is already done with the viscosity (nu) for incompressible solvers.

I have modified the viscosityModel files in order to create the new model, but when I compile, I get this error:

Quote:
thermalDiffusivityModels/thermalDiffusivityModel/thermalDiffusivityModel.C: In constructor ‘Foam::thermalDiffusivityModel::thermalDiffusivity Model(const Foam::word&, const Foam::dictionary&, const volVectorField&, const surfaceScalarField&)’:
thermalDiffusivityModels/thermalDiffusivityModel/thermalDiffusivityModel.C:53:13: error: no matching function for call to ‘Foam::dictionary::dictionary(<unresolved overloaded function type>)’
phi_(phi)
^
thermalDiffusivityModels/thermalDiffusivityModel/thermalDiffusivityModel.C:53:13: note: candidates are:
In file included from thermalDiffusivityModels/thermalDiffusivityModel/thermalDiffusivityModel.H:48:0,
from thermalDiffusivityModels/thermalDiffusivityModel/thermalDiffusivityModel.C:26:
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:232:9: note: Foam::dictionary::dictionary(const Foam::Xfer<Foam::dictionary>&)
dictionary(const Xfer<dictionary>&);
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:232:9: note: no known conversion for argument 1 from ‘<unresolved overloaded function type>’ to ‘const Foam::Xfer<Foam::dictionary>&’
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:229:9: note: Foam::dictionary::dictionary(const Foam::dictionary&, const Foam::Xfer<Foam::dictionary>&)
dictionary(const dictionary& parentDict, const Xfer<dictionary>&);
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:229:9: note: candidate expects 2 arguments, 1 provided
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:226:9: note: Foam::dictionary::dictionary(const Foam::dictionary*)
dictionary(const dictionary*);
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:226:9: note: no known conversion for argument 1 from ‘<unresolved overloaded function type>’ to ‘const Foam::dictionary*’
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:222:9: note: Foam::dictionary::dictionary(const Foam::dictionary&)
dictionary(const dictionary&);
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:222:9: note: no known conversion for argument 1 from ‘<unresolved overloaded function type>’ to ‘const Foam::dictionary&’
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:219:9: note: Foam::dictionary::dictionary(const Foam::dictionary&, const Foam::dictionary&)
dictionary(const dictionary& parentDict, const dictionary&);
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:219:9: note: candidate expects 2 arguments, 1 provided
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:216:9: note: Foam::dictionary::dictionary(Foam::Istream&, bool)
dictionary(Istream&, const bool keepHeader);
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:216:9: note: candidate expects 2 arguments, 1 provided
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:212:9: note: Foam::dictionary::dictionary(Foam::Istream&)
dictionary(Istream&);
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:212:9: note: no known conversion for argument 1 from ‘<unresolved overloaded function type>’ to ‘Foam::Istream&’
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:203:9: note: Foam::dictionary::dictionary(const Foam::fileName&, const Foam::dictionary&, Foam::Istream&)
dictionary
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:203:9: note: candidate expects 3 arguments, 1 provided
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:199:9: note: Foam::dictionary::dictionary(const Foam::fileName&)
dictionary(const fileName& name);
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:199:9: note: no known conversion for argument 1 from ‘<unresolved overloaded function type>’ to ‘const Foam::fileName&’
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:196:9: note: Foam::dictionary::dictionary()
dictionary();
^
/software/alternate/openfoam/fc20/2.3.0/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/dictionary.H:196:9: note: candidate expects 0 arguments, 1 provided
make: *** [Make/linux64GccDPOpt/thermalDiffusivityModel.o] Error 1
It seems there is a problem called no matching function for call to ‘Foam::dictionary::dictionary(<unresolved overloaded function type>)’ but all I found there are references in C++ that are not related with my problem.

Did you guys face this problem before?

Thank you!
agustinvo is offline   Reply With Quote

Old   November 4, 2015, 11:16
Default
  #2
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Brussels
Posts: 165
Rep Power: 7
agustinvo is on a distinguished road
Hi, I was able to solve it, there was a mistake inside the code.

Now I have to link it to one solver and try it.
agustinvo is offline   Reply With Quote

Old   November 5, 2015, 03:21
Default
  #3
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,199
Rep Power: 21
akidess will become famous soon enough
Why not make this thread useful and share how you solved your problem? Someone in the future will thank you for it.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
akidess is offline   Reply With Quote

Old   November 5, 2015, 03:35
Default
  #4
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Brussels
Posts: 165
Rep Power: 7
agustinvo is on a distinguished road
Hello,

the error was a typing one, so the rest of the code was ok. But you are right in the fact I could explain a bit my procedure for other people who wanted to implement it.

The idea was to replace any term related with viscosity with the thermal diffusivity. Instead of creating the function "nu" you should type "alpha", "kappa"...

I defined as well a transport thermal model (transportModel) and a singlePhaseTransportModel, where "alpha" is used instead the kinematic viscosity.

In the solver, in yout readTransportProperties, you should add:

Code:
singlePhaseTransportThermalModel laminarTransportThermal(U, phi);
so in your case you have to give something like this in your transportProperties:
Code:
transportThermalModel  Newtonian;

alpha              alpha [ 0 2 -1 0 0 0 0 ]  1.75048355e-007;
My next step is to use this new transportModel in turbulence thermal models (working on it ).

EDIT:

now, in order to integrate your new transportModel in your turbulence models, you have to create a new turbulenceModel library. In my case it is an incompressible one. If you copy & paste the already existing one, you have to do some modifications:

Code:
autoPtr<turbulenceThermalModel> turbulenceThermalModel::New
(
    const volVectorField& U,
    const surfaceScalarField& phi,
    const volScalarField& T,
    transportModel& transport,
    transportThermalModel& transportThermal,
    const word& turbulenceThermalModelName
)
and you should add transportThermalModel& transportThermal, each time you see this kind of declaration.

In this other declaration you have to do similarly:
Code:
(U, phi, T, transport, transportThermal, turbulenceThermalModelName)
Inside the turbulenceModel.H you can define your equation terms for T (like turbulence->divDevReff()).

Ok. Now the turbulent thermal models are there, but RAS models must be created as well to use them in our simulations.

Other library RASModel must be created. Copying the existing one, applying the second replacement I explained, and modifying a bit the RASModels.C and .H it should be ok. After that you have to implement your own turbulence RAS thermal models.

Passing throught the first library (models for nut) to the thermal one (alphat) is quite straightforward, in the sense there are already some terms that need a little modification (ie, change nu for alpha, U for T ...). If further explanation is required, please make me know. Even this could be considered to create another thread .
akidess likes this.

Last edited by agustinvo; November 5, 2015 at 07:12. Reason: Adding modifications in turbulence libraries
agustinvo is offline   Reply With Quote

Old   November 5, 2015, 07:15
Default
  #5
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Brussels
Posts: 165
Rep Power: 7
agustinvo is on a distinguished road
I have modified my second post in order to include the use of the new transport model in the turbulence models.

Maybe for C++ users and programmers, it is quite obvious the way to do it, but for people like me, it can be very helpful.
agustinvo is offline   Reply With Quote

Old   November 6, 2015, 12:07
Default
  #6
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Brussels
Posts: 165
Rep Power: 7
agustinvo is on a distinguished road
Hello,

once this library is working, I want to implement a polynomial expression for alpha, in the same way I did it already for nu. It was just a copy and paste, and replacements of nu, viscosity ... for their equivalents.

But I get this error when I compile:
Code:
Making dependency list for source file thermalDiffusivityModels/TempPolyLaw/TempPolyLaw.C
thermalDiffusivityModels/TempPolyLaw/TempPolyLaw.dep:489: warning: overriding recipe for target `Make/linux64Gcc48DPOpt/TempPolyLaw.o'
viscosityModels/TempPolyLaw/TempPolyLaw.dep:489: warning: ignoring old recipe for target `Make/linux64Gcc48DPOpt/TempPolyLaw.o'
SOURCE=thermalDiffusivityModels/TempPolyLaw/TempPolyLaw.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -O3  -DNoRepository -ftemplate-depth-100 -I/software/alternate/openfoam/fc20/2.3.1/OpenFOAM-2.3.1/src/transportModels/incompressible/lnInclude -I/software/alternate/openfoam/fc20/2.3.1/OpenFOAM-2.3.1/src/transportModels/incompressible/twoPhaseMixture/lnInclude -I/software/alternate/openfoam/fc20/2.3.1/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -IlnInclude -I. -I/software/alternate/openfoam/fc20/2.3.1/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/software/alternate/openfoam/fc20/2.3.1/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64Gcc48DPOpt/TempPolyLaw.o
TempPolyLaw.o:(.bss+0x18): multiple definition of `Foam::thermalDiffusivityModels::TempPolyLaw::typeName'
TempPolyLaw.o:(.bss+0x18): first defined here
TempPolyLaw.o:(.bss+0x10): multiple definition of `Foam::thermalDiffusivityModels::TempPolyLaw::debug'
TempPolyLaw.o:(.bss+0x10): first defined here
TempPolyLaw.o:(.bss+0x8): multiple definition of `Foam::thermalDiffusivityModels::addTempPolyLawToDebug_'
TempPolyLaw.o:(.bss+0x8): first defined here
TempPolyLaw.o:(.bss+0x0): multiple definition of `Foam::thermalDiffusivityModels::addTempPolyLawdictionaryConstructorTothermalDiffusivityModelTable_'
TempPolyLaw.o:(.bss+0x0): first defined here
TempPolyLaw.o: In function `Foam::thermalDiffusivityModels::TempPolyLaw::calcAlpha() const':
TempPolyLaw.C:(.text+0x880): multiple definition of `Foam::thermalDiffusivityModels::TempPolyLaw::calcAlpha() const'
TempPolyLaw.o:TempPolyLaw.C:(.text+0x880): first defined here
TempPolyLaw.o: In function `Foam::thermalDiffusivityModels::TempPolyLaw::TempPolyLaw(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&)':
TempPolyLaw.C:(.text+0xb60): multiple definition of `Foam::thermalDiffusivityModels::TempPolyLaw::TempPolyLaw(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&)'
TempPolyLaw.o:TempPolyLaw.C:(.text+0xb60): first defined here
TempPolyLaw.o: In function `Foam::thermalDiffusivityModels::TempPolyLaw::TempPolyLaw(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&)':
TempPolyLaw.C:(.text+0xb60): multiple definition of `Foam::thermalDiffusivityModels::TempPolyLaw::TempPolyLaw(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&)'
TempPolyLaw.o:TempPolyLaw.C:(.text+0xb60): first defined here
TempPolyLaw.o: In function `Foam::thermalDiffusivityModels::TempPolyLaw::read(Foam::dictionary const&)':
TempPolyLaw.C:(.text+0x1100): multiple definition of `Foam::thermalDiffusivityModels::TempPolyLaw::read(Foam::dictionary const&)'
TempPolyLaw.o:TempPolyLaw.C:(.text+0x1100): first defined here
collect2: error: ld returned 1 exit status
make: *** [/students/phd_ea/villaortiz/OpenFOAM/villaortiz-2.3.1/platforms/linux64Gcc48DPOpt/lib/libmyIncompressibleTransportModels.so] Error 1
Has someone had this error before? It seems there is something already defined over there, but I am not able to see it. I tried to change the name of my model (TempPolyLaw) but it does not work.

file.C
Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011 OpenFOAM Foundation
     \\/     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/>.

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

#include "TempPolyLaw.H"
#include "addToRunTimeSelectionTable.H"
#include "surfaceFields.H"

// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //

namespace Foam
{
namespace thermalDiffusivityModels
{
    defineTypeNameAndDebug(TempPolyLaw, 0);

    addToRunTimeSelectionTable
    (
        thermalDiffusivityModel,
        TempPolyLaw,
        dictionary
    );
}
}


// * * * * * * * * * * * * Private Member Functions  * * * * * * * * * * * * //

Foam::tmp<Foam::volScalarField>
Foam::thermalDiffusivityModels::TempPolyLaw::calcAlpha() const
{


    const volScalarField& T= U_.mesh().lookupObject<volScalarField>("T"); 
    //const volScalarField& rho= U_.mesh().lookupObject<volScalarField>("rho");     
    
    return (base_+slope_*T+slope2_*pow(T,2.0)+slope3_*pow(T,3.0));
}


// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

Foam::thermalDiffusivityModels::TempPolyLaw::TempPolyLaw
(
    const word& name,
    const dictionary& thermalDiffusivityProperties,
    const volVectorField& U,
    const surfaceScalarField& phi
)
:
    thermalDiffusivityModel(name, thermalDiffusivityProperties, U, phi),
    TempPolyLawCoeffs_(thermalDiffusivityProperties.subDict(typeName + "Coeffs")),
    base_(TempPolyLawCoeffs_.lookup("base")),
    slope_(TempPolyLawCoeffs_.lookup("slope")),
    slope2_(TempPolyLawCoeffs_.lookup("slope2")),
    slope3_(TempPolyLawCoeffs_.lookup("slope3")),
    alpha_
    (
        IOobject
        (
            name,
            U_.time().timeName(),
            U_.db(),
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        calcAlpha()
    )
{}


// * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * * //

bool Foam::thermalDiffusivityModels::TempPolyLaw::read
(
    const dictionary& thermalDiffusivityProperties
)
{
    thermalDiffusivityModel::read(thermalDiffusivityProperties);

    TempPolyLawCoeffs_ = thermalDiffusivityProperties.subDict(typeName + "Coeffs");

    TempPolyLawCoeffs_.lookup("base") >> base_;
    TempPolyLawCoeffs_.lookup("slope") >> slope_;
    TempPolyLawCoeffs_.lookup("slope2") >> slope2_;    
    TempPolyLawCoeffs_.lookup("slope3") >> slope3_;
    

    return true;
}


// ************************************************************************* //
file.H
Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011 OpenFOAM Foundation
     \\/     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/>.

Class
    Foam::viscosityModels::TempPolyLaw

Description
     Standard polynomial-law non-Newtonian viscosity model.
     
     mu=a0+a1*T+a2*T2+...

SourceFiles
    TempPolyLaw.C

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

#ifndef TempPolyLaw_H
#define TempPolyLaw_H

#include "thermalDiffusivityModel.H"
#include "dimensionedScalar.H"
#include "volFields.H"

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

namespace Foam
{
namespace thermalDiffusivityModels
{

/*---------------------------------------------------------------------------*\
                           Class TempPolyLaw Declaration
\*---------------------------------------------------------------------------*/

class TempPolyLaw
:
    public thermalDiffusivityModel
{
    // Private data

        dictionary TempPolyLawCoeffs_;

        dimensionedScalar base_;
        dimensionedScalar slope_;
        dimensionedScalar slope2_;
        dimensionedScalar slope3_;    

        volScalarField alpha_;


    // Private Member Functions

        //- Calculate and return the laminar viscosity
        tmp<volScalarField> calcAlpha() const;


public:

    //- Runtime type information
    TypeName("TempPolyLaw");


    // Constructors

        //- Construct from components
        TempPolyLaw
        (
            const word& name,
            const dictionary& thermalDiffusivityProperties,
            const volVectorField& U,
            const surfaceScalarField& phi
        );


    //- Destructor
    ~TempPolyLaw()
    {}


    // Member Functions

        //- Return the laminar viscosity
        tmp<volScalarField> alpha() const
        {
            return alpha_;
        }
    
        //- Return the laminar viscosity for patch
        tmp<scalarField> alpha(const label patchi) const
        {
            return alpha_.boundaryField()[patchi];
        }    
    

        //- Correct the laminar viscosity
        void correct()
        {
            alpha_ = calcAlpha();
        }

        //- Read transportProperties dictionary
        bool read(const dictionary& thermalDiffusivityProperties);
};


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

} // End namespace viscosityModels
} // End namespace Foam

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

#endif

// ************************************************************************* //
SOLVED

I was using the same fileName.C
for the polynomial of nu() and alpha, so there was a conflict with the internal functions (the only difference between both files are the viscosity and thermal diffusivity references, not the C++ and functions ones). I changed the names, so I have
Quote:
viscosityModels/TempPolyLaw/TempPolyLaw.C
thermalDiffusivityModels/TempPolyLaw/thermalTempPolyLaw.C
and they are present in corresponding *.o files. Before they have the same *.o file name.


Now it is possible to implement the same functions for each diffusion term (nu and alpha), just be sure the names are different!

Last edited by agustinvo; November 9, 2015 at 06:57.
agustinvo is offline   Reply With Quote

Old   November 9, 2015, 06:59
Default
  #7
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Brussels
Posts: 165
Rep Power: 7
agustinvo is on a distinguished road
The previous problem was solved. It is explained on its post.

I think it would be interesting to create a post of "How to implement a new transport model library", in a nicer way than the one here.
akidess likes this.
agustinvo is offline   Reply With Quote

Old   December 5, 2016, 08:34
Default
  #8
New Member
 
Hasan Celik
Join Date: Sep 2016
Posts: 14
Rep Power: 2
PositronCascade is on a distinguished road
Dear agustinvo, thank you so much for this post. I try to do the exactly the same thing with you and your post helped me a lot to understand where I should start. In your code, these lines below refer to viscosity or thermal conductivity? I am little bit confused.

Code:
//- Calculate and return the laminar viscosity
        tmp<volScalarField> calcAlpha() const;
Would you mind to share TempPolyLaw and thermalTempPolyLaw source code and header files with me, if you don't mind?

And my other question is, how did you compile it? Did you add these models to src folder or did you compile them individually using usr libbin?

Thanks a lot for your answer and time.


Quote:
Originally Posted by agustinvo View Post
The previous problem was solved. It is explained on its post.

I think it would be interesting to create a post of "How to implement a new transport model library", in a nicer way than the one here.
PositronCascade is offline   Reply With Quote

Old   December 5, 2016, 09:47
Default
  #9
Senior Member
 
Agustín Villa
Join Date: Apr 2013
Location: Brussels
Posts: 165
Rep Power: 7
agustinvo is on a distinguished road
Quote:
Originally Posted by PositronCascade View Post
Dear agustinvo, thank you so much for this post. I try to do the exactly the same thing with you and your post helped me a lot to understand where I should start. In your code, these lines below refer to viscosity or thermal conductivity? I am little bit confused.

Code:
//- Calculate and return the laminar viscosity
        tmp<volScalarField> calcAlpha() const;
Would you mind to share TempPolyLaw and thermalTempPolyLaw source code and header files with me, if you don't mind?

And my other question is, how did you compile it? Did you add these models to src folder or did you compile them individually using usr libbin?

Thanks a lot for your answer and time.
Hello,

for me, alpha is the thermal diffusivity, it is \alpha=\frac{\kappa}{\rho c_p}. Since I have other libraries, I put them in USER_LIBBIN, so I don't mess up the installation folder with all my implementations. What you can use to know how to implement different models is this PDF, more or less they explain what to do in each part. My implementations are done in OF 2.3.1, but I don't know if it changed a lot or not for OF 3.0.x or OF 4.x
agustinvo is offline   Reply With Quote

Old   December 5, 2016, 18:01
Default
  #10
New Member
 
Hasan Celik
Join Date: Sep 2016
Posts: 14
Rep Power: 2
PositronCascade is on a distinguished road
Thank you so much!
PositronCascade is offline   Reply With Quote

Reply

Tags
thermal diffusivity, transportproperties

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Adding new temperature dependent viscosity model vabishek OpenFOAM Programming & Development 3 May 15, 2016 21:05
Adding different properties to Thermophysical Model DanAndrea87 OpenFOAM Programming & Development 9 May 1, 2014 10:37
adding lift model to twoPhaseEulerFoam mehrdad_kbg OpenFOAM Programming & Development 8 September 17, 2013 16:08
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
K - epsilon VS SST turbulence model Maicol Main CFD Forum 0 November 30, 2012 17:25


All times are GMT -4. The time now is 04:40.