[Dan1788]

Dear all,

I am using reactingFoam for simulating a 2d axisymmetric jet flame. The following in the default energy equation in reactingFoam:

{
volScalarField& he = thermo.he();

fvScalarMatrix EEqn
(
fvm::ddt(rho, he) + mvConvection->fvmDiv(phi, he)
+ fvc::ddt(rho, K) + fvc::div(phi, K)
+ (
he.name() == "e"
? fvc::div
(
fvc::absolute(phi/fvc::interpolate(rho), U),
p,
"div(phiv,p)"
)
: -dpdt
)
- fvm::laplacian(turbulence->alphaEff(), he)
// - fvm::laplacian(turbulence->muEff(), he) // unit lewis no.
==
reaction->Sh()
+ fvOptions(rho, he)
);

EEqn.relax();

fvOptions.constrain(EEqn);

EEqn.solve();

fvOptions.correct(he);

thermo.correct();

Info<< "min/max(T) = "
<< min(T).value() << ", " << max(T).value() << endl;
}

What does the term "fvc::ddt(rho, K) + fvc::div(phi, K)" signify in the above, specifically what is the variable K in this equation?

Also what does the term "fvOptions(rho, he)" mean?

I would be really glad if anyone could help me out. Thanks!

[Dan1788]

Foamers,

Anyone who can help? would really appreciate it

[dkxls]

Hi Daniel,

maybe at first a general advise: Please use the CODE tags, makes it much easier to read your post!
See also here: http://www.cfd-online.com/Forums/ope...tml#post424508

Originally Posted by Dan1788

What does the term "fvc::ddt(rho, K) + fvc::div(phi, K)" signify in the above, specifically what is the variable K in this equation?

K is the kinetic energy; see the files createFields.H and pEqn.H in

applications/solvers/combustion/reactingFoam/

This "new" formulation of the energy equation got introduced with version 2.1, see OpenFOAM 2.0 for an alternative formulation of the energy equation (or a good text book will also do ).

Originally Posted by Dan1788

Also what does the term "fvOptions(rho, he)" mean?

If you don't know what it is you can forget about it at this point. See here for a more detailed explanation:
http://www.openfoam.org/version2.2.0/fvOptions.php

[Dan1788]

Thanks Armin, this info certainly helped

I had another question regarding the momentum predictor statement in OpenFoam.

In the default version of reactingFoam (the solver I am using), the momentum predictor is turned off. Does this mean that the momentum equation is not solved ?? How is the velocity then computed ??

Please let me know if you have some knowledge about this. Thanks again!

[Cyp]

Hi Daniel,

When your momentum predictor is set to off, indeed the matrix UEqn is not solved. However, you will notice in the source code that the matrix in created and updated with the flux of the previous time step. The variable H and rAU depend on this updated matrix and they are used to solve p.

U is then evaluated during the corrector step, at the end of pEqn file.

Best,
Cyprien

[Dan1788]

Thanks Cyprien,

Can you suggest me some references or books where I can read about the pressure velocity coupling and the nomenclature that OpenFoam uses?

[Cyp]

Sure,

The reference for me remains the book of Patankar "Numerical Heat Transfer And Fluid Flow"

Another good reference, Ferziger and Peric "Computational Method for Fluid Dynamics"

The original paper of PISO is also instersting: Issa "Solution of the implicitly discretised fluid flow equations by operator-splitting"

More specific to OpenFOAM, there is the PhD dissertation of Hrvoje Jasak one of the main contributor to OpenFOAM "Error Analysis and Estimation for the Finite Volume Method with Application to Fluid Flows".

And a personal contribution: http://www.scribd.com/doc/181588911/...ion-of-icoFoam.

Cheers,
Cyprien