[charles4allme]

Hello,

I have this new conduction equation and I was wondering how to insert it into OpenFOAM

pcdT/dt = d/dx(kdT/dx) with k = keff if x< du or k = k if x> du

I have also attached the equation with the diagram of the problem. I do not know how to create the condition in my pyrolysis model with the new thermal conductivity.

I appreciate the assistance.

[SHUBHAM9595]

The Equation can be written as follow in a new file TEqn.H....This file can be created in solver directory using touch TEqn.H

	fvScalarMatrix TEqn
    (
        fvm::ddt(T) == fvm::laplacian(alphat, T)
     );

TEqn.solve();

But before this we have to define alphat as

tmp <volScalarField> alphat = K/(rho*cp);

Now as k is dependent on vertical length, we need to access that coordinate using

const fvMesh& mesh = U.mesh();
volScalarField Ycord = mesh.C().component(vector::Y);// assuming Y is the vertical

	 forAll(K,celli)
{
		if (Ycord[celli] <= DU.value())
	
		{
			K[celli] = Keff.value()/(rho.value()*cp.value());
		}
		else
		{
			K[celli] = K2.value()/(rho.value()*cp.value());;
		}

}

And finally we have to intialise all the additional variables in createFields.H as

    // Density
    dimensionedScalar rho(transportProperties.lookup("rho"));
    
    // sPECIFIC HEAT
    dimensionedScalar cp(transportProperties.lookup("cp"));

    // Threshold vertical length 
    dimensionedScalar DU(transportProperties.lookup("DU"));
    
      // Keff
    dimensionedScalar Keff(transportProperties.lookup("Keff"));
    
      // K2
    dimensionedScalar K2(transportProperties.lookup("K2"));

 Info<< "Reading field Thermal Conductivity \n" << endl;
volScalarField K
(
    IOobject
    (
        "K",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

Finally, include "TEqn.H" in your "customFoam.C" file within runtime loop

[charles4allme]

Hi SHUBHAM9595,

Thanks a lot for your reply. It has truly been helpful