[Kummi]

Hello Foamers,
I was working with older version of OpenFOAM 2.1.1. Currently, I shifted to version v2106 for some reason. While working with pyrolysis in OFv2106, the energy equation looks like,

fvScalarMatrix hEqn
(
fvm::ddt(rho_, h_)
- fvm::laplacian(alpha, h_)
+ fvc::laplacian(alpha, h_)
- fvc::laplacian(kappa(), T())
==
chemistryQdot_
+ solidChemistry_->RRsHs()
);

In my case, I want to use temperature directly in Energy equation as follows,

fvScalarMatrix TEqn
(
fvm::ddt(rhoCp, T_)
- fvm::laplacian(K_, T_)
==
chemistryQdot_
);

In older version OF 2.1.1, the temperature implementation is so direct in the equation but not in the case of OFv2106. So, I did little research on how to make this happen.
In basicThermo.C,

// Temperature returns a non-const value
Foam::volScalarField& Foam::basicThermo::T()
{
return T_;
}

So, I initialized T_ as part of constructor in my source file as,

T_
(
IOobject
(
* * "T",
* * * regionMesh().time().timeName(),
* * * regionMesh(),
* * * IOobject::MUST_READ,
* * * IOobject::AUTO_WRITE
),
* * * //regionMesh(),
* * * solidThermo_->T()
* * )

There is no problem with compilation. Before running the case, I fixed a print statement under the energy equation to check the variation of temperature.
Info << "T_from Energy equ:" << T_ << endl;

I can find the variation in temperature in the log file as,

T_from Energy equ:dimensions [0 0 0 1 0 0 0];

internalField nonuniform List<scalar>
14
(
931.685
877.421
824.294
773.017
724.259
678.639
636.723
599.013
565.938
537.856
515.058
497.77
486.156
480.322
)
;

However, the output changes are nil. NO changes in fuel compositions, temperature and other variables. If I'm not wrong, the energy equation which I've adopted based on temperature is not solved. Can someone share their ideas to sort out this ?
Another question:
What are differences in implementing T or h in Energy equation and their advantages and disadvantages in OpenFOAM ?
Thank you

[Kummi]

auto& T1_ = solidThermo_->T();
forAll(T1_, celli)
{
T1_[celli] = T_[celli];
}

I have tried fixing this above the energy equation, but that doesn't helped. Any ideas from someone ?
Thank you

[mAlletto]

What you are solving for in fluid dynamics is the energy equation. For this reason solving for h does make sense. If you want to solve for T you already make an assumption about your thermodynamic model:





This model is fairly ok if the temperature range is not too high or for ideal gases. If you want to apply other thermodynamic models (see https://cfd.direct/openfoam/user-gui...hermophysical/) or be as flexible as possible in selecting your desired thermodynamic model at run time, you have to solve for h. If you want then to retrieve the temperature from your equation of state, you have to solve a non-linear equation. See https://caefn.com/openfoam/temperature-calculation for an explanation.

[Kummi]

Hello Michael Alletto,
Thanks for your points.
In my case, the boundary condition is given in the form of temperature not heat and that's the reason why my energy equation is in temperature form. Correct me if I'm wrong please.
So the temperature variable calculates heat transferred into the domain.



Hereby in my governing equation, the source terms are dependent on temperature changes too.
Thank you

[Kummi]

In higher versions of OpenFOAM, the temperature is calculated from enthalpy. In the file heSolidThermo.C, the function THE calculates temperature from enthalpy, where enthalpy is declared in the parent class heThermo.

In any case, if we require the energy equation in temperature form (as quoted below), that's not gonna work, as there will no change in temperature at the end result.

fvScalarMatrix TEqn
(
fvm::ddt(rhoCp, T_)
- fvm::laplacian(K_, T_)
==
chemistryQdot_
);

In order to solve TEqn, comment out updateT() return variable TOwner in basicThermo.H.

//- Should T be updated
Switch updateT() const
{
//return TOwner_;
}

In basicThermo.C, T_ returns temperature value. updateT() updates T_ based on enthalpy. If updateT() is dead, then T_ will be calculated from the TEqn matrix.

T_(lookupOrConstruct(mesh, phasePropertyName("T"), TOwner_)),
TOwner_(getOrDefault<Switch>("updateT", TOwner_)),

Hope it helps someone.
Thank you