[balkrishna]

In the buoyantBousinessqSimpleFoam solver i want to vary my Cp with temperature . How should i write the program for this ?

[balkrishna]

As a start , lets say i want to vary Cp in the following manner :
Cp = C*tanh(mT) ;

I write the program in the following manner :

Info<<" Reading field Cp "<<endl ;
    volScalarField Cp
    (
        IOobject
        (
            "Cp",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    );

Info<<" Reading field C "<<endl ;
    volScalarField C
    (
        IOobject
        (
            "C",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    );

and in readTransportProperties.H

dimensionedScalar m (laminarTransport.lookup("m"));

m will have dimensions of [ 0 0 0 -1 0 0 0]
In TEqn.H i have the added a source term . and hence need Cp . I add it in the following manner .

Cp = C*tanh(mT);
followed by the temperature equation .

This compiles fine but when i run the program i get the following error :

--> FOAM FATAL ERROR: 
Argument of trancendental function not dimensionless

    From function trans(const dimensionSet& ds)
    in file dimensionSet/dimensionSet.C at line 370.

Does any1 have a clue to solve this ???

[chandramurthy]

i think, this is something to do with dimensional consistency for LHS and RHS. From the error message it may said that the term "C*tanh(mT)" should have the units of cp.

An alternative way is use JANAF tables.

[nimasam]

1) you can use thermodynamic table which is implemented in open foam
2) but whats the dimension of c and cp, does they have the same dimensions?
if yes,
try it
forAll (C,celli)
{cp[celli]=c[celli]*tanh(m*T[celli])
}
or
define m as dimless and use T.value() to get just the value of it

[balkrishna]

@chandramurthy : C has the dimensions of Cp and m*T is dimensionless. .... m has dimensions of [ 0 0 0 -1 0 0 0 ] while T has that of [0 0 0 1 0 0 0].... The error says that m*T is not dimensionless .... which is not very clear to me ...

[balkrishna]

@nimasam : C and Cp have the same dimensions . regarding the loop you have suggested when i declare C and Cp as volScalarFields and simply do Cp = C*tanh(m*T) shouldnt it be executed on all cells ?

[nimasam]

u are right, every thing seems correct! but those two suggested methods were to insure that variable are dimensionless

[balkrishna]

@nimasam I get the following error for the first one :
error: ‘struct Foam::volScalarField’ has no member named ‘value’

for the second one :
error: cannot convert ‘Foam::dimensioned<double>’ to ‘double’ in assignment

[alberto]

Hi,

value() is a method for scalars, not for volScalarFields. You have to loop over cells to use it.

Did you check mT is actually dimensionless (you did not say how you define it in the code).

Best,

[balkrishna]

@alberto i define m in transportProperties in the following manner :

m                 m [0 0 0 -1 0 0 0] 0.2;

to read m i define it in readTransportProperties.H
as

dimensionedScalar m (laminarTransport.lookup("m"));

and T is temperature i.e. [0 0 0 1 0 0 0] . I loop over cells in the above mentioned manner and i got the following error :

error: cannot convert ‘Foam::dimensioned<double>’ to ‘double’ in assignment

basically that means i cant declare m in readTransportProperties.H . Then what is the workaround ?

[alberto]

Use

m.value()

However it should really work with fields without looping.

Best,

[karthik1414]

Originally Posted by chandramurthy

i think, this is something to do with dimensional consistency for LHS and RHS. From the error message it may said that the term "C*tanh(mT)" should have the units of cp.

An alternative way is use JANAF tables.

hello,
i am very new to openfoam, is it possible to use janafthermo.H while using the interfoam solver?? basically i want to vary Cp and density with temperature and pressure in a 2 phase incompressible vof problem.
Please help me out in this matter.
regards,
karthik

[balkrishna]

that gives the following error :

error: call of overloaded ‘tanh(double)’ is ambiguous

[balkrishna]

problem solved . Thanks everyone . I was including the variation in a header file . Once this was removed and added it in TEqn.H ... it worked ... thanks a lot for your help .

[nimasam]

Originally Posted by balkrishna

that gives the following error :

error: call of overloaded ‘tanh(double)’ is ambiguous

i know ur problem get solve but for who to seek answer for this problem:

use Foam::tanh(....) instead of tanh() , it will cure the pain

[balkrishna]

In case of varying Cp with temperature , i wish to vary it conditionally .
What i mean is :
for T < Tvalue
Cp = f(T) ;
for T >= Tvalue
Cp = g(T) ;

in such a case i am not able to use the standard operators like >= or > or <
My code is as follows:

forAll(T,celli)
      {
        if ( T[celli] >= Tleft && T[celli] <= Tmid)
          {
            Cp[celli] = 1000*41.2/50.0 * (T[celli] - Tleft) +   cpConstant;
          }
        else if ( T[celli] > Tmid && T[celli] <= Tright )
          {
            Cp[celli] = -1000*41.2/50 * ( T[celli] - Tright ) + cpConstant;
          }
      }

I get the following error :

TEqn.H: In function ‘int main(int, char**)’:
TEqn.H:23: error: no match for ‘operator>=’ in ‘T.Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::<anonymous>.Foam::DimensionedField<double, Foam::volMesh>::<anonymous>.Foam::Field<double>::<anonymous>.Foam::List<double>::<anonymous>.Foam::UList<T>::operator[] [with T = double](celli) >= Tleft’
TEqn.H:23: error: no match for ‘operator<=’ in ‘T.Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::<anonymous>.Foam::DimensionedField<double, Foam::volMesh>::<anonymous>.Foam::Field<double>::<anonymous>.Foam::List<double>::<anonymous>.Foam::UList<T>::operator[] [with T = double](celli) <= Tmid’
TEqn.H:25: error: cannot convert ‘Foam::dimensioned<double>’ to ‘double’ in assignment
TEqn.H:27: error: no match for ‘operator>’ in ‘T.Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::<anonymous>.Foam::DimensionedField<double, Foam::volMesh>::<anonymous>.Foam::Field<double>::<anonymous>.Foam::List<double>::<anonymous>.Foam::UList<T>::operator[] [with T = double](celli) > Tmid’
TEqn.H:27: error: no match for ‘operator<=’ in ‘T.Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::<anonymous>.Foam::DimensionedField<double, Foam::volMesh>::<anonymous>.Foam::Field<double>::<anonymous>.Foam::List<double>::<anonymous>.Foam::UList<T>::operator[] [with T = double](celli) <= Tright’
TEqn.H:29: error: cannot convert ‘Foam::dimensioned<double>’ to ‘double’ in assignment
/home/ifmg/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/readSIMPLEControls.H:9: warning: unused variable ‘transonic’
make: *** [Make/linux64GccDPOpt/buoyantBoussinesqSimpleFoam.o] Error 1

In the above case , Tmid , Tleft , Tright are dimensionedScalars defined in the following manner :

In readTransportProperties.H
dimensionedScalar  Tleft (laminarTransport.lookup("Tleft"));
dimensionedScalar   Tright (laminarTransport.lookup("Tright"));
dimensionedScalar   Tmid (laminarTransport.lookup("Tmid"));

How should i use the conditional operators in this case ?

[nimasam]

dear friend you can not assign a dimension Scalar to a scalar so use value()

Tleft.value() and so on

[balkrishna]

thanks ,

that was a lesson learnt ....

[balkrishna]

I am solving a heat transfer problem with water as fluid . So far I am using the buoyantBousinessqSimpleFoam solver . This solver however has the temperature formulation instead of the enthalpy formulation for the energy equation . That is correct considering that Cp and rho are assumed to be constant . I wish to formulate the energy equation using enthalpy . Can any of the already available solvers do this ? I went through the tutorials of solvers which are present in OF170 , what i found was that all of them used the working substance as air , assuming it as a perfectGas . This was declared in constant/thermophysicalProperties as :

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

mixture         air 1 28.96 1004.4 0 1.831e-05 0.705;

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

How do i use solvers like buoyantPimpleFoam for water ?

[balkrishna]

When i rewrite the enthalpy equation as :

fvScalarMatrix hEqn
          (
           fvm::ddt(rho, h)
           + fvm::div(phi, h)
           ==
            fvm::laplacian(k,T)
           + DpDt + heatSource
           );
//In the above , k is thermal conductivity , T is temperature , h is enthalpy .

I get the following error :

incompatible fields for operation 
    [h] == [T]

    From function checkMethod(const fvMatrix<Type>&, const fvMatrix<Type>&)
    in file /home/ifmg/OpenFOAM/OpenFOAM-1.7.0/src/finiteVolume/lnInclude/fvMatrix.C at line 1181.

How to overcome it ?