[shivani17]

I have modified the viscosity model giving viscosity variation with temperature. It has been compiled successfully but while running a case with transportModel mentioned as temppowerLaw, it is unable to identify it.The error is
--> FOAM FATAL ERROR:
Unknown viscosityModel type temppowerLaw

Valid viscosityModels are :

7
(
BirdCarreau
Casson
CrossPowerLaw
HerschelBulkley
Newtonian
powerLaw
strainRateFunction
)


From function static Foam::autoPtr<Foam::viscosityModel> Foam::viscosityModel::New(const Foam::word&, const Foam::dictionary&, const volVectorField&, const surfaceScalarField&)
in file viscosityModels/viscosityModel/viscosityModelNew.C at line 49.

FOAM exiting
The code is:

#include "temppowerLaw.H"
#include "addToRunTimeSelectionTable.H"
#include "surfaceFields.H"

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

namespace Foam
{
namespace viscosityModels
{
defineTypeNameAndDebug(temppowerLaw, 0);

addToRunTimeSelectionTable
(
viscosityModel,
temppowerLaw,
dictionary
);
}
}


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

Foam::tmp<Foam::volScalarField>
Foam::viscosityModels::temppowerLaw::calcNu() const
{
const volScalarField& T=U_.mesh().lookupObject<volScalarField>("T"); // added
return max
(
nuMin_,
min
(
nuMax_,
//k_*pow
(k_-kslope_*(T-Tbase_))*pow //added
(
max
(
dimensionedScalar("one", dimTime, 1.0)*strainRate(),
dimensionedScalar("small", dimless, small)
),
n_.value() - scalar(1)
)
)
);
}

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

Foam::viscosityModels::temppowerLaw::temppowerLaw
(
const word& name,
const dictionary& viscosityProperties,
const volVectorField& U,
const surfaceScalarField& phi
)
:
viscosityModel(name, viscosityProperties, U, phi),
temppowerLawCoeffs_(viscosityProperties.optionalSu bDict(typeName + "Coeffs")),
k_("k", dimViscosity, temppowerLawCoeffs_),
n_("n", dimless, temppowerLawCoeffs_),
kslope_(temppowerLawCoeffs_.lookup("kslope")), //added
Tbase_(temppowerLawCoeffs_.lookup("Tbase")),
nuMin_("nuMin", dimViscosity, temppowerLawCoeffs_),
nuMax_("nuMax", dimViscosity, temppowerLawCoeffs_),
nu_
(
IOobject
(
name,
U_.time().timeName(),
U_.db(),
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
calcNu()
)
{}


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

bool Foam::viscosityModels::temppowerLaw::read
(
const dictionary& viscosityProperties
)
{
viscosityModel::read(viscosityProperties);

temppowerLawCoeffs_ = viscosityProperties.optionalSubDict(typeName + "Coeffs");

temppowerLawCoeffs_.lookup("k") >> k_;
temppowerLawCoeffs_.lookup("n") >> n_;
temppowerLawCoeffs_.lookup("kslope") >> kslope_; //added
temppowerLawCoeffs_.lookup("Tbase") >> Tbase_;
temppowerLawCoeffs_.lookup("nuMin") >> nuMin_;
temppowerLawCoeffs_.lookup("nuMax") >> nuMax_;

return true;
}

Please help!

[mAlletto]

Did you include the path of the library you compiled in the controlDict like:

libs("path/yourlib.so")

[shivani17]

In controlDict it is required to write solver name right?, in transportproperties of constant folder the transportModel is mentioned
controlDict:
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application temperaturesimpleFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 2000;

deltaT 1;

writeControl timeStep;

writeInterval 100;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression off;

timeFormat general;

timePrecision 6;

runTimeModifiable true;

functions
{
#includeFunc streamlines
}

transportProperties:
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

transportModel temppowerLaw;

nu [0 2 -1 0 0 0 0] 1e-05;

temppowerLawCoeffs
{
k [0 2 -1 0 0 0 0] 2800;
n [0 0 0 0 0 0 0] 0.64;
kslope [0 2 -1 -1 0 0 0] 0.5;
Tbase [0 0 0 1 0 0 0] 300;
nuMin [0 2 -1 0 0 0 0] 0.1;
nuMax [0 2 -1 0 0 0 0] 10000000;
}

TempD [ 0 2 -1 0 0 0 0] 1e-8;

[shivani17]

I changed in controlDict file as:My library is in /src/transportModels/incompressible/viscosityModels/temppowerLaw
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
libs ("src/transportModels/incompressible/viscosityModels/temppowerLaw.so");

application temperaturesimpleFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 2000;

deltaT 1;

writeControl timeStep;

writeInterval 100;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression off;

timeFormat general;

timePrecision 6;

runTimeModifiable true;


functions
{
#includeFunc streamlines
}


Tried with 1.libs ("src/transportModels/incompressible/viscosityModels/temppowerLaw/temppowerLaw.so");
2. libs ("libtemppowerLaw.so");

[shivani17]

While compiling .so file is not created in linux64GccDPInt32Opt
msg displayed after compiling
wmake libso .
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file temppowerLaw.C
g++ -std=c++11 -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -Wno-attributes -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam6/src/transportModels/incompressible/lnInclude -I/opt/openfoam6/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam6/src/OpenFOAM/lnInclude -I/opt/openfoam6/src/OSspecific/POSIX/lnInclude -fPIC -c temppowerLaw.C -o Make/linux64GccDPInt32Opt/temppowerLaw.o
g++ -std=c++11 -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -Wno-attributes -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam6/src/transportModels/incompressible/lnInclude -I/opt/openfoam6/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam6/src/OpenFOAM/lnInclude -I/opt/openfoam6/src/OSspecific/POSIX/lnInclude -fPIC -shared -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPInt32Opt/temppowerLaw.o -L/opt/openfoam6/platforms/linux64GccDPInt32Opt/lib \
-lfiniteVolume -o /home/shivani/OpenFOAM/root-6/platforms/linux64GccDPInt32Opt/lib/temppowerLaw.so

[mAlletto]

It is probably created in /home/shivani/OpenFOAM/root-6/platforms/linux64GccDPInt32Opt/lib/temppowerLaw.so

[shivani17]

Thank You !! So much. I wrote the path in controlDict file and it has identified the new library

[aa399@aub.edu.lb]

Hello.

I have the same problem, and I wrote in the controlDict the libs with the correct path to it, but unfortunately the problem was not solved, and I am getting the following message again:

--> FOAM FATAL ERROR:
Unknown viscosityModel type tempdeppowerLaw

Valid viscosityModels are :

7
(
BirdCarreau
Casson
CrossPowerLaw
HerschelBulkley
Newtonian
powerLaw
strainRateFunction
)


From function static Foam::autoPtr<Foam::viscosityModel> Foam::viscosityModel::New(const Foam::word&, const Foam::dictionary&, const volVectorField&, const surfaceScalarField&)
in file viscosityModels/viscosityModel/viscosityModelNew.C at line 49.

FOAM exiting

can you please help me discover the problem?
Thank you in advance