[Sun]

Hi,
I am trying to modify the BirdCarreau viscosity model. The current expression in OpenFOAM is:

 nuInf_
      + (nu0_ - nuInf_)
       *pow(scalar(1) + sqr(k_*strainRate()), (n_ - 1.0)/2.0);

where nuInf, nu0, k_ and n_ are constants (dimensionedScalar and being read from the transportProperties). But I should implement two time-dependent correlations for nuInf and nu0. The equations look like the following:

nu0_tmdep = a/(1+b*t+c*t^2)
nuInf_tmdep = exp(e+f*t+g*t^2)

a,b,c,d,e,f, and g are given constants whereas t is time. I have created two volScalarFields in the .C file and deleted reading of nu0_ and nuInf_ everywhere in the .H file.

Foam::tmp<Foam::volScalarField>
Foam::viscosityModels::ModifiedBirdCarreau::calcNu() const
{
	
	volScalarField nu0_tmdep 
	    (
	     scalar(84.455311)/(scalar(1)-scalar(0.0309746)*runTime.value()+scalar(0.00024088)*sqr(runTime.value()))
	    );

	volScalarField nuInf_tmdep
	    (
	     Foam::exp(scalar(12.022048)-scalar(0.629963)*runTime.value()+scalar(0.00898332)*sqr(runTime.value()))
	    );

	
    return
        nuInf_tmdep
      + (nu0_tmdep - nuInf_tmdep)
       *pow(scalar(1) + sqr(k_*strainRate()), (n_ - 1.0)/2.0);
}

In compilation, I am getting these errors:
ModifiedBirdCarreau/ModifiedBirdCarreau.C: In member function ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::viscosityModels::ModifiedBirdCarreau::calcNu () const’:
ModifiedBirdCarreau/ModifiedBirdCarreau.C:55:54: error: ‘runTime’ was not declared in this scope
ModifiedBirdCarreau/ModifiedBirdCarreau.C: In constructor ‘Foam::viscosityModels::ModifiedBirdCarreau::Modif iedBirdCarreau(const Foam::word&, const Foam::dictionary&, const volVectorField&, const surfaceScalarField&)’:
ModifiedBirdCarreau/ModifiedBirdCarreau.C:104:5: error: no matching function for call to ‘Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField()’

I would be really thankful if someone can give me some pieces of advice and I must say I am kind of new in OpenFOAM territory, so I might have done something pretty silly!
Cheers!

[alexeym]

Hi,

you can try

U_.time().timeOutputValue()

if you'd like to access runTime (which usually is available in solvers and is created in createTime.H include file).

[Sun]

Hi Alexey,
Thanks a lot for your help.
Now I've got access to the runTime. But it's still complaining about:

In member function ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::viscosityModels::ModifiedBirdCarreau::calcNu () const’:
ModifiedBirdCarreau/ModifiedBirdCarreau.C:59:6: error: no matching function for call to ‘Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricField(double)’

I am not really sure, where it is coming from! any suggestions would be appreciated.

Cheers!

[alexeym]

Hi,

it's just trying to say that it can't construct volScalarField from double. Why would you like to use volScalarField for nu0_tmdep instead of dimensionedScalar? I can see that this value depends on time, but I don't see the dependence of coordinate. So I think this

volScalarField nu0_tmdep 
	    (
	     scalar(84.455311)/(scalar(1)-scalar(0.0309746)*runTime.value()+scalar(0.00024088)*sqr(runTime.value()))
	    );

should be

dimensionedScalar nu0_tmdep("nu0", <dimensions of nu0_tmdep>, scalar(84.455311)/(scalar(1) -scalar(0.0309746)*runTime.value() + scalar(0.00024088)*sqr(runTime.value())))

Or you can create this dimensionedScalar in constructor of the class and then just update it value in calcNu method.

[Sun]

Thank you so much Alexey for the speedy answer. I created it as a dimensionedScalar in the constructor and no compilation error.
You've just made my day!
cheers!

[deve]

Hey,

I didn't want to open a new thread since I think that my problem has a lot to do with the problem of the thread opener's.

i'm trying to modify a viscosity model (newtonian, but i guess it doesn't matter). What I want to do is, make the viscosity time dependent.
So I wrote a simple equation which describes this relation:
Viscosity = nu * ( 1 + nu / 700 * Time )
and implemented it in the following source code (see green lines!)
(Voelkl is the Name of my ViscosityModel)

#include "Voelkl.H"
#include "addToRunTimeSelectionTable.H"
#include "surfaceFields.H"
//extern Foam::Time runTime;
 
// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
 
namespace Foam
{
namespace viscosityModels
{
    defineTypeNameAndDebug(Voelkl, 0);
    addToRunTimeSelectionTable(viscosityModel,Voelkl,dictionary);
}
}
 
 
// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
Foam::viscosityModels::Voelkl::Voelkl
(
    const word& name,
    const dictionary& viscosityProperties,
    const volVectorField& U,
    const surfaceScalarField& phi
)
:
    viscosityModel(name, viscosityProperties, U, phi),
    nu0_("nu", dimensionSet(0, 2, -1, 0, 0), viscosityProperties_.lookup("nu")),
    nu_
    (
        IOobject
        (
            name,
            U_.time().timeName(),
            U_.db(),
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        U_.mesh(),
       nu0_* ( 1 + nu0_ / 700 * runTime.value() )
  //   nu0_* ( 1 + nu0_ / 700 * U_.time()timeOutputValue() )
    )
{}
 
 
// * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * * //
 
bool Foam::viscosityModels::Voelkl::read
(
    const dictionary& viscosityProperties
)
{
    viscosityModel::read(viscosityProperties);
 
    viscosityProperties_.lookup("nu") >> nu0_;
    nu_ = nu0_;
 
    return true;
}
 
 
// ************************************************************************* //

The Problem is that neither of the two variants are working. I tried a lot of things but had no success yet.
Among these tries were adding

#include "createTime.H"

which resulted in the following Problem:

deve@deve:~/OpenFOAM/deve-2.3.1/applications/viscosityModels/Voelkl$ wmake
wmakeLnInclude: linking include files to ./lnInclude
Making dependency list for source file Voelkl.C
SOURCE=Voelkl.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam231/src/transportModels/incompressible/lnInclude/ -I/opt/openfoam231/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/Voelkl.o
In file included from Voelkl.C:29:0:
/opt/openfoam231/src/OpenFOAM/lnInclude/createTime.H:5:5: error: ‘Info’ in namespace ‘Foam’ does not name a type
     Foam::Info<< "Create time\n" << Foam::endl;
     ^
/opt/openfoam231/src/OpenFOAM/lnInclude/createTime.H:7:53: error: ‘args’ was not declared in this scope
     Foam::Time runTime(Foam::Time::controlDictName, args);
                                                     ^
make: *** [Make/linux64GccDPOpt/Voelkl.o] Fehler 1

I noticed that the "createTime.H" file is not what i expected.

//
// createTime.H
// ~~~~~~~~~~~~
 
    Foam::Info<< "Create time\n" << Foam::endl;
 
    Foam::Time runTime(Foam::Time::controlDictName, args);

Does anyone have a clue what the problem is?
Thanks in advance
Deve

Edit: I was able to find a solution to my problem; send PM for further information

[jasouza1974]

Hi deve,

I'm having the same problem. I can not access runTime() variable from my viscosity model.

How did you solve the problem?

Thanks.