[adhiraj]

Hi all,
I am new to OpenFOAM. I was looking at where OpenFOAM does the h to T (or hs top T) conversion, and I noted that they use a Newton iteration mthod. But when I try to trace the sepcific heat they use in this equation, they seem to use Cp=Cp(T) and not Cp=Cp(T,Yi). This is the file I am talking about:-
$FOAM/src/thermophysicalModels/specie/thermo/janaf
Can anyone confirm/explain this?
Thanks in advance.

[Farshad_Noravesh]

Hi,

I have exactly the same question.

Thanks

Farshad

[adhiraj]

I have dug deep since this post, and have the answers. When they go for the h->T conversion they hold the composition fixed, and define a new 'gas' with the composition averaged thermal properties. It is the Cp of this mixture gas that is (rightly) used to compute T.

[isabel]

Hi all,

I am looking for the extract of the code where the conversion from h to T is done but I do not find it. Can anybody tell me where it is?

[adhiraj]

Check under

$FOAM_SRC/thermophysicalModels/specie/thermo/specieThermo

[isabel]

Thank you very much. I found the iteration in these lines:


// return the temperature corresponding to the value of the
// thermodynamic property f, given the function f = F(T) and dF(T)/dT
template<class thermo>
inline scalar specieThermo<thermo>::T
(
scalar f,
scalar T0,
scalar (specieThermo<thermo>::*F)(const scalar) const,
scalar (specieThermo<thermo>::*dFdT)(const scalar) const
) const
{
scalar Test = T0;
scalar Tnew = T0;
scalar Ttol = T0*tol_;
int iter = 0;

do
{
Test = Tnew;
Tnew = Test - ((this->*F)(Test) - f)/(this->*dFdT)(Test);

if (iter++ > maxIter_)
{
FatalErrorIn
(
"specieThermo<thermo>::T(scalar f, scalar T0, "
"scalar (specieThermo<thermo>::*F)(const scalar) const, "
"scalar (specieThermo<thermo>::*dFdT)(const scalar) const"
") const"
) << "Maximum number of iterations exceeded"
<< abort(FatalError);
}

} while (mag(Tnew - Test) > Ttol);

return Tnew;
}


There is something I do not understhand. What does “this->” means?

[megacrout]

I might be wrong but I don´t think this is an OF-specific function.
Ecosia (instead of googling it) "this pointer" or "this pointer c++" or such.
Tibo

[adhiraj]

It is a C++ keyword. "this" acts like a pointer to the object whose member function is under consideration.

[isabel]

Dear friends,

I have another doubt about these files. Where are defined the functions F and dFdT?

[adhiraj]

They are the function and its derivative.
The Newton iteration in this case calculates T, given F(T) and dF/dT(T).
The function gets pointers to the functions F and dF/dt.

If the energy variable is enthalpy h, then F=h(T) and dF/dt=Cp(T).
If it is internal energy e, then F=e and dF/dT=Cv(T).

The code resolves these at runtime, and sends the appropriate pointers to the Newton iteration routine.

[isabel]

Dear friends,

Thank you very much for your help. I need to simulate melting of a solid. In that case, the enthalpy is given by the following equation:




where L is the latent heat and alpha_l the mass fraction of the liquid phase.

How do I implement the term alpha_l*L in the functions F and dFdT?

[adhiraj]

Hi,
I would use

    F=H
    dFdT=Cp

This is because, H=H(T) is the relationship you are trying to invert.
And, at that point you will typically hold the composition fixed, so that \alpha, L and H_{ref} are fixed. So, dFdT=Cp.
This of course assumes that L is not a function of T.

[lfgmarc]

Hi, I have a little question,

I understand that if i.e, the energy variable is enthalpy F=h(T) and dF/dT=Cp(T), my question is in where it is defined in the code that F and dF/dt take these variables as arguments.

Thanks in advance.

[ahmmedshakil]

Hi isabel ,
Will you please guide me how you implemented the melting problem ?
thanks in advance.

Originally Posted by isabel

Dear friends,

Thank you very much for your help. I need to simulate melting of a solid. In that case, the enthalpy is given by the following equation:




where L is the latent heat and alpha_l the mass fraction of the liquid phase.

How do I implement the term alpha_l*L in the functions F and dFdT?

[Mhmnabil]

Hi All,

I just don't know where that "f" is coming from in OpenFOAM??? I know "F" and "dFdT", but I don't understand "f" in the Newton's routine!!

Originally Posted by adhiraj

They are the function and its derivative.
The Newton iteration in this case calculates T, given F(T) and dF/dT(T).
The function gets pointers to the functions F and dF/dt.

If the energy variable is enthalpy h, then F=h(T) and dF/dt=Cp(T).
If it is internal energy e, then F=e and dF/dT=Cv(T).

The code resolves these at runtime, and sends the appropriate pointers to the Newton iteration routine.

[Mhmnabil]

What is that "f" in the routine?! Where does it come from?

Originally Posted by isabel

Thank you very much. I found the iteration in these lines:


// return the temperature corresponding to the value of the
// thermodynamic property f, given the function f = F(T) and dF(T)/dT
template<class thermo>
inline scalar specieThermo<thermo>::T
(
scalar f,
scalar T0,
scalar (specieThermo<thermo>::*F)(const scalar) const,
scalar (specieThermo<thermo>::*dFdT)(const scalar) const
) const
{
scalar Test = T0;
scalar Tnew = T0;
scalar Ttol = T0*tol_;
int iter = 0;

do
{
Test = Tnew;
Tnew = Test - ((this->*F)(Test) - f)/(this->*dFdT)(Test);

if (iter++ > maxIter_)
{
FatalErrorIn
(
"specieThermo<thermo>::T(scalar f, scalar T0, "
"scalar (specieThermo<thermo>::*F)(const scalar) const, "
"scalar (specieThermo<thermo>::*dFdT)(const scalar) const"
") const"
) << "Maximum number of iterations exceeded"
<< abort(FatalError);
}

} while (mag(Tnew - Test) > Ttol);

return Tnew;
}


There is something I do not understhand. What does “this->” means?

[qjh888]

Could anybody help me to find where it is defined in the code that F and dF/dt take these variables as arguments??

Thanks!