[sharonyue]

Hello guys

I was trying to figure out this function:

tmp<fvMatrix<Type> > Foam::correction	(	const fvMatrix< Type > & 		)	
Return the correction form of the given matrix.
by subtracting the matrix multiplied by the current field

I checked out the code in fvMatrix.H. its:

template<class Type>
Foam::tmp<Foam::fvMatrix<Type> > Foam::correction
(
    const fvMatrix<Type>& A
)
{
    tmp<Foam::fvMatrix<Type> > tAcorr = A - (A & A.psi());

    if
    (
        (A.hasUpper() || A.hasLower())
     && A.psi().mesh().fluxRequired(A.psi().name())
    )
    {
        tAcorr().faceFluxCorrectionPtr() = (-A.flux()).ptr();
    }

    return tAcorr;
}

But I did grasp its meaning. Is it substantial derivative?

Thanks

[sharonyue]

Yeah, from mathematical equations. it should be substantial derivative, but it does not look like.

[sharonyue]

Okay, I figured it out finally,

correction(fvm::ddt(p)) means d(p)/d(t) - d(pold)/d(t)

/handshake

[kaifu]

Originally Posted by sharonyue

correction(fvm::ddt(p)) means d(p)/d(t) - d(pold)/d(t)

What does pold here refer to? A temporary value during iteration or the solution from previous time step (usually in the transient solver)? In case of former circumstance, the correction term should disappear when the equation is converged. I'd rather treat this term in favor of mathematics than physics.

[CorbinMG]

Dear FOAMers,

I have been struggling to understand the correction() function as well. Particularly as it is implemented in the compressibleInterFoam pEqn.H. I don't have a perfect answer, but I at least wanted to put in the information I have found here. It would be nice if an OpenFOAM expert could tell us once and for all the meaning and purpose of correction().

First, the definition of the correction() function is found in fvMatrix.C. For OpenFOAM v2112, this looks like:

template<class Type>
Foam::tmp<Foam::fvMatrix<Type>> Foam::correction
(
    const fvMatrix<Type>& A
)
{
    tmp<Foam::fvMatrix<Type>> tAcorr = A - (A & A.psi());
 
    // Delete the faceFluxCorrection from the correction matrix
    // as it does not have a clear meaning or purpose
    deleteDemandDrivenData(tAcorr.ref().faceFluxCorrectionPtr());
 
    return tAcorr;
}
 
 
template<class Type>
Foam::tmp<Foam::fvMatrix<Type>> Foam::correction
(
    const tmp<fvMatrix<Type>>& tA
)
{
    tmp<Foam::fvMatrix<Type>> tAcorr = tA - (tA() & tA().psi());
 
    // Delete the faceFluxCorrection from the correction matrix
    // as it does not have a clear meaning or purpose
    deleteDemandDrivenData(tAcorr.ref().faceFluxCorrectionPtr());
 
    return tAcorr;
}

Then the question is what does the A.psi() mean? Well, from the CFD Direct book Chapter 3.5, OpenFOAM constructs the matrix for each equation as: . So I guess psi refers to the solved field variable.

What does correction() actually do? Well, as mentioned at the beginning of this post, "Return the correction form of the given matrix by subtracting the matrix multiplied by the current field".

Henry gave us another hint here: https://bugs.openfoam.org/view.php?id=1772
"The correction(fvm::ddt(p_rgh)) term is a correction to fvc::ddt(rho) due to changes in pressure and the converged result will be the same irrespective of how this correction is formulated, i.e. the correction will converge to 0 and the results will be fvc::ddt(rho)."

So I guess the correction term goes to 0 at convergence and it is meant for improving solver robustness?

More insights into the functionality of the correction() function are welcomed.

Best regards,
Corbin

Edit: this thread also contains come interesting ideas on what correction() might do: Understanding Terms in Compressible pEqn

Edit2: this wiki has some good info on OpenFOAM matrices which may also help: https://openfoamwiki.net/index.php/O...es_in_OpenFOAM