[kaber]

Dear Foamers,

I try to modify the laplacianFoam solver to account for a variable thermal diffusivity.

I found the following three threads:

LaplacianFoam with non-constant Diffusion Coefficient

Non-constant Diffusion Coefficient

Thermal conductivity as function of temperature

which deal with this modification. However, I'm not able to implement them.

I added the following code to the createFields.H

volScalarField Diff
(
    IOobject
    (
        "Diff",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::NO_WRITE
    ),
    mesh,
    dimensionedScalar("Diff",dimensionSet(0,2,-1,0,0),0.0)
  );

and added a (simplified linear) equation to the mylaplacianFoamVarDT.C

while (runTime.loop())
     {
     Diff = 430-0.0785*T;

    fvScalarMatrix TEqn(-fvm::laplacian(Diff, T));
 
    TEqn.solve();

     }

The code compiles without any error, but mylaplacianFoamVarDT complains that the dimensions of

Diff = 430-0.0785*T;

are not correct

--> FOAM FATAL ERROR:
LHS and RHS of '-' have different dimensions
     dimensions : [0 0 0 0 0 0 0] - [0 0 0 1 0 0 0]

Sure, "430" is dimensionless and the "linear equation" part is of dimension K.
Since I'm not yet very familiar with openFOAM, I tried a work around by changing the dimension of Diff (to avoid a similar dimension problem) to K and get rid of the constant "430" first.

volScalarField Diff
(
    IOobject
    (
        "Diff",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::NO_WRITE
    ),
    mesh,
    dimensionedScalar("Diff",dimensionSet(0,0,0,1,0),0.0)
);

while (runTime.loop())
    {
    Diff = -0.0785*T;

    fvScalarMatrix TEqn(-fvm::laplacian(Diff, T));

    TEqn.solve();

    }

Again, wmake complies, but mylaplacianFoamVarDT shows the following error:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v1812 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : v1812 OPENFOAM=1812
Arch : "LSB;label=32;scalar=64"
Exec : mylaplacianFoamVarDT
Date : Nov 17 2019
Time : 13:26:07
Host : kabaer
PID : 13163
I/O : uncollated
Case : /home/XXX/OpenFOAM/XXX-v1812/run/GettingStarted/1DRod-Dirichlet-VariableDT
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


SIMPLE: no convergence criteria found. Calculations will run for 1 steps.

Reading field T

Creating variable Diffusivity

Reading transportProperties

Reading diffusivity k

No finite volume options present

Calculating temperature distribution

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in /lib/x86_64-linux-gnu/libc.so.6
#3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) at ??:?
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foamerator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#5 Foam::harmonic::interpolate(Foam::GeometricField<d ouble, Foam::fvPatchField, Foam::volMesh> const&) const at ??:?
#6 Foam::fv::laplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#7 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::laplacian<double, double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in ~/OpenFOAM/XXX-v1812/platforms/linux64GccDPInt32Opt/bin/mylaplacianFoamVarDT
#8 ? in ~/OpenFOAM/XXX-v1812/platforms/linux64GccDPInt32Opt/bin/mylaplacianFoamVarDT
#9 __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#10 ? in ~/OpenFOAM/XXX-v1812/platforms/linux64GccDPInt32Opt/bin/mylaplacianFoamVarDT

I'm grateful for any help....

[ahmmedshakil]

Hi Chris,
If you look at the error message printed by the OpenFOAM, you may figure out why the error is coming. The error in the first line is showing is a "printStack" type, which means that something is calculating wrong, Please check the parameters as well as the boundary conditions you're using for simulations. Then, check the laplacian scheme you used, as the diffusion term is non-linear, you may use the harmonic interpolation, which may help you to simulate.

-S

[kaber]

Dear Mohammed,
thanks for the hint ! I found the problem.
The initial temperature distribution within my domain was set to "zero",

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v1812 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 1 0 0 0];

internalField uniform 0;

so the equation

Diff=-0.0785*T

results in Diff = 0, which obviously leads to a zero matrix. However, I wonder why this is not leading to the same error with original laplacianFoam and constant conductivity....

In addition, I checked both, "linear" as well as "harmonic" interpolation scheme for "Diff" and also the solver "Conjugate Gradient" as well as "GaussSeidel". All of them give the same result.

But I got another question. In order to get the dimensions of "Diff" right (not the work around with dimension "K" - see above) I would like to know how I can assign the right dimension to the terms within the equation.

Diff = 430 - 0.0785*T;

Best regards!

[jd87]

You can name new scalar variables, give them proper dimensions in the transportproperties file, so that Diff has a dimension of thermal diffusivity. This will work well. Or else you have to put dimensionSet to 0 so that OpenFOAM does not check dimensional consistency before running the simulations.

[Bloerb]

Define 430 as a variable with a unit (this is a dimensionedScalar). Something like this with maybe a slightly different syntax.

 dimensionedScalar Tvalue = ("Tvalue", [0 2 -1 0 0 0 0], 430);