[Gary51075607]

hello, eveybody
i'm a new in learning OpenFoam and have problems in reading the EEqn.H in the solver of buyoantSimpleFoam.
what do the follwing secentences respect for?

he.name() == "e"
? fvc::div(phi, volScalarField("Ekp", 0.5*magSqr(U) + p/rho))
: fvc::div(phi, volScalarField("K", 0.5*magSqr(U)))

and i also doubt about the "fvOptions" followed.

[fabian_roesler]

Hi Gary

he.name() == "e"
? fvc::div(phi, volScalarField("Ekp", 0.5*magSqr(U) + p/rho))
: fvc::div(phi, volScalarField("K", 0.5*magSqr(U)))

is an if structure to decide whether to use
internal energy

fvc::div(phi, volScalarField("Ekp", 0.5*magSqr(U) + p/rho))

or enthalpy

fvc::div(phi, volScalarField("K", 0.5*magSqr(U)))

formulation, where 0.5*magSqr(U) is specific kinetic energy and p/rho should be a work term.

+ fvOptions(rho, he)

fvOptions is a kind of library where options like porous media, SRF/MRF and sources for all solvers are implemented. So if you choose to add a source term for a specific cell zone, this will be handled here.

Hope this helps a bit.

Cheers

Fabian

[Gary51075607]

Thank you very much, Febian. Now i can completely understand it

Regard,

Gary

[Gary51075607]

Originally Posted by fabian_roesler

fvOptions is a kind of library where options like porous media, SRF/MRF and sources for all solvers are implemented. So if you choose to add a source term for a specific cell zone, this will be handled here.

Hi, Fabian

Now i want to add a source term in the energy equation using the fvOptions. where can i get enough info about it?

Regards!

Gary

[fabian_roesler]

Browse the tutorials and you will find everthing you need:

 
energySource1
{
    type            scalarSemiImplicitSource;
    active          true;
    timeStart       0.2;
    duration        2.0;
    selectionMode   points;
    points
    (
        (2.75 0.5 0)
    );
    scalarSemiImplicitSourceCoeffs
    {
        volumeMode      absolute;
        injectionRateSuSp
        {
            h           (10 0);
        }
    }
}

 
source1
{
    type            fixedTemperatureConstraint;
    active          true;
    timeStart       0.1;
    duration        0.4;
    selectionMode   cellSet;
    cellSet         ignitionCells;
    fixedTemperatureConstraintCoeffs
    {
        mode            uniform;
        temperature     2000;
    }
}

[umeshisode]

Hello Everybody,

I am trying to understand a rhoPorousSimpleFoam solver but stuck in the file EEqn.h at solvers directory.

fvScalarMatrix EEqn
(
fvm::div(phi, he)
+ (
he.name() == "e"
? fvc::div(phi, volScalarField("Ekp", 0.5*magSqr(U) + p/rho))
: fvc::div(phi, volScalarField("K", 0.5*magSqr(U)))
)
- fvm::laplacian(turbulence->alphaEff(), he)
==
fvOptions(rho, he)
);


In above code what is "Ekp" and "K" stands for .

And one more question, how to get value in "fvOptions(rho, he)".

Thanks in advance. Waiting for your reply.