[hari154]

At very beginning of the simulation, where is phi calculated /initialised?

I am aware that phi is calculated according to,
phi = (fvc::interpolate(U) & mesh.Sf())
+ fvc::ddtPhiCorr(rUA, U, phi);
But at the very beginning of the simulation we have to form Ueqn using phi, unfortunately we don't have rUA at the beginning of simulation.

So I am curious to know how phi is initialised?

[mAlletto]

https://www.openfoam.com/documentati...8H_source.html

[superkelle]

Originally Posted by hari154

At very beginning of the simulation, where is phi calculated /initialised?

I am aware that phi is calculated according to,
phi = (fvc::interpolate(U) & mesh.Sf())
+ fvc::ddtPhiCorr(rUA, U, phi);
But at the very beginning of the simulation we have to form Ueqn using phi, unfortunately we don't have rUA at the beginning of simulation.

So I am curious to know how phi is initialised?

I think this question occures very often and has been answered several times. Just use the search function. Never the less I give you some additional advice, look into createField files of the solver source code for example in icoFoam: /applications/solvers/incompressible/icoFoam

Info<< "Reading field U\n" << endl;
volVectorField U
(
    IOobject
    (
        "U",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);


#include "createPhi.H"

Then search for this file, it is located in a different location. For simplicity just use the search in your OF directory. You will find createFields.H for example in /src/finiteVolume/cfdTools/incompressible , that have following code:

Global
    createPhi

Description
    Creates and initialises the relative face-flux field phi.

\*---------------------------------------------------------------------------*/

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Info<< "Reading/calculating face flux field phi\n" << endl;

surfaceScalarField phi
(
    IOobject
    (
        "phi",
        runTime.timeName(),
        mesh,
        IOobject::READ_IF_PRESENT,
        IOobject::AUTO_WRITE
    ),
    fvc::flux(U)
);


// ************************************************************************* //

You will also find some additional "links" that are also called createFields.H but don't mind that ( for example in /src/finiteVolume/lnInclude ).



On the other hand there are also solvers that have no:

#include "createPhi.H"

like potentialFoam, there it is "hard coded" into createFields. Do not ask me why.

U = dimensionedVector(U.dimensions(), Zero);

surfaceScalarField phi
(
    IOobject
    (
        "phi",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    fvc::flux(U)
);

What I does not know myself is whether there is a difference in the ways to write the flux:

fvc::flux(U)

vs.

phi = (fvc::interpolate(U) & mesh.Sf())

Maybe someone else could bring light into this dark. I suspect that there is maybe the same math involved but, with some additional conditions/restrictions for the fvc::flux() function, since the second version is very strait forward.


I have also seen versions where the "fvc::" is not put in front like in "createPhiv.H" . I also don't know why that is.(and where/what phiv is used for)

surfaceScalarField phiv
(
    IOobject
    (
        "phiv",
        runTime.timeName(),
        mesh,
        IOobject::READ_IF_PRESENT,
        IOobject::AUTO_WRITE
    ),
    flux(U)
);