[open]

New OpenFoam (2.4) user!

As per the title... I wish to use a temperature dependent viscosity model. I've seen various posts and papers on this so I've followed the example modifying the power law - that compiles ok.

My next step was to take the BirdCarreau and modify to suit Carreau-Yasuda:

u=u0 * alpha * [lambda * alpha * strainrate + 1]^((n-1)/2)
alpha = exp[beta * (1/T - 1/Tref)]

TempCarreauYasuda.C (header also modified)

Foam::tmp<Foam::volScalarField>
Foam::viscosityModels::TempCarreauYasuda::calcNu() const
{
    const volScalarField& T= U_.mesh().lookupObject<volScalarField>("T"); 

    return max
    (
    nuInf_,

        nu0_ * Foam::exp(beta_ * (1.0/T - 1.0/Tref_) )
    *pow(lambda_ * Foam::exp(beta_ * (1.0/T - 1.0/Tref_) ) * strainRate() + scalar(1), (n_ - 1.0)/a_)

    );
}

transportProperties

TempCarreauYasudaCoeffs
{
    nu0             nu0 [ 0 2 -1 0 0 0 0 ] 7.191; // 5645/rho
    nuInf           nuInf [ 0 2 -1 0 0 0 0 ] 1.2739e-03; // 1/rho
    lambda          lambda [ 0 0 -1 0 0 0 0 ] 0.28;
    n               n [ 0 0 0 0 0 0 0 ] 0.61;
    beta            beta [ 0 0 0 1 0 0 0 ] 6330.0;
    Tref            Tref [ 0 0 0 1 0 0 0 ] 473.15;
    a               a [ 0 0 0 0 0 0 0 ] 2.0; // can omit as will default to 2
}

Question 1: how can I define

Foam::exp(beta_ * (1.0/T - 1.0/Tref_) )

as a variable to avoid repetition?

Question 2: The code compiles without error. Why is the following error occurring:

Selecting incompressible transport model TempCarreauYasuda


--> FOAM FATAL ERROR: 
LHS and RHS of + have different dimensions
     dimensions : [0 0 -2 0 0 0 0] + [0 0 0 0 0 0 0]


    From function operator+(const dimensionSet&, const dimensionSet&)
    in file dimensionSet/dimensionSet.C at line 478.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::operator+(Foam::dimensionSet const&, Foam::dimensionSet const&) at ??:?
#3  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator+<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::dimensioned<double> const&) at ??:?
#4  Foam::viscosityModels::TempCarreauYasuda::calcNu() const at ??:?
#5  Foam::viscosityModels::TempCarreauYasuda::TempCarreauYasuda(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) at ??:?
#6  Foam::viscosityModel::adddictionaryConstructorToTable<Foam::viscosityModels::TempCarreauYasuda>::New(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) at ??:?
#7  Foam::viscosityModel::New(Foam::word const&, Foam::dictionary const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) at ??:?
#8  Foam::singlePhaseTransportModel::singlePhaseTransportModel(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) at ??:?
#9  ? at ??:?
#10  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11  ? at ??:?

It looks like a dimension problem but I'm not sure why.

[open]

Question 2 is resolved... I notice that I specified incorrect units in the transportProperties.

The full source code is attached (no guarantees) to help other beginners.

Still looking for guidance with the first question.

[TobM]

Do you mean something like that?

Foam::tmp<Foam::volScalarField> 
Foam::viscosityModels::TempCarreauYasuda::calcNu() const 
{
    const volScalarField& T= U_.mesh().lookupObject<volScalarField>("T");
    volScalarField test = Foam::exp(beta_ * (1.0/T - 1.0/Tref_) );      
    return max
    (
        nuInf_, 
        nu0_ * Foam::exp(beta_ * (1.0/T - 1.0/Tref_) )
      * pow(lambda_ * test * strainRate() + scalar(1), (n_ - 1.0)/a_)      
    );
 }

I hope it works...

[open]

Originally Posted by TobM

I hope it works...

Forgot to post back; yes works, and thank you for your help.