Code of the Week #18: phi -= pEqn.flux()

在 icoFoam.C 中,有这么一段

                pEqn.solve();

                if (nonOrth == nNonOrthCorr)
                {
                    phi -= pEqn.flux();
                }

对不可压缩流体连续性方程进行离散,

\nabla\cdot U = \sum_f U\cdot S_f = \sum \phi_f

式中, \phi_f 为面通量。
将此式代入

\begin{equation} \mathbf U_\mathrm{P}^{n+1} = \mathbf{U}^{*,n+1} - \frac{1}{A_\mathrm{P}}\nabla p^{n+1} \end{equation} \tag{5}

此式来自 Code of the Week #4: solve(UEqn == -fvc::grad( p))。有

\phi_f = \mathbf S_f\cdot U^{*,n+1} - \frac{1}{A_p} \mathbf S_f \cdot \nabla p

上式中的 \dfrac{1}{A_p} S_f \cdot \nabla p 出现在了压力泊松方程的离散过程中 (Code of the Week #4: solve(UEqn == -fvc::grad( p)) 式 (9) ),有

\frac{1}{A_p} \mathbf S_f \cdot \nabla p = \frac{1}{A_p} \frac{\mathbf S_f}{|\mathbf d|}( p_N - p_P) = a_N^P(p_N - p_P)

式中, \mathbf d 为相邻网格中心点距离。因为, \mathbf S = \mathbf\Delta +\mathbf k
over-relaxed
所以

\frac{1}{A_p} \mathbf S_f \cdot \nabla p = \frac{1}{A_p} \frac{\mathbf \Delta}{|\mathbf d|}( p_N - p_P) + \frac{1}{A_p} \mathbf k\cdot\nabla p

上式就是 flux() 表达式。要使通量完全守恒,必须与组成压力方程的形式一致 (使用非正交修正)。

flux() 在 fvMatrix.C 中的定义为:

template<class Type>
Foam::tmp<Foam::GeometricField<Type, Foam::fvsPatchField, Foam::surfaceMesh> >
Foam::fvMatrix<Type>::
flux() const
{
    if (!psi_.mesh().schemesDict().fluxRequired(psi_.name()))
    {
        FatalErrorIn("fvMatrix<Type>::flux()")
            << "flux requested but " << psi_.name()
            << " not specified in the fluxRequired sub-dictionary"
               " of fvSchemes."
            << abort(FatalError);
    }

    // construct GeometricField<Type, fvsPatchField, surfaceMesh>
    tmp<GeometricField<Type, fvsPatchField, surfaceMesh> > tfieldFlux
    (
        new GeometricField<Type, fvsPatchField, surfaceMesh>
        (
            IOobject
            (
                "flux("+psi_.name()+')',
                psi_.instance(),
                psi_.mesh(),
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
            psi_.mesh(),
            dimensions()
        )
    );
    GeometricField<Type, fvsPatchField, surfaceMesh>& fieldFlux = tfieldFlux();

    for (direction cmpt=0; cmpt<pTraits<Type>::nComponents; cmpt++)
    {
        fieldFlux.internalField().replace
        (
            cmpt,
            lduMatrix::faceH(psi_.internalField().component(cmpt))
        );
    }

    // This needs to go into virtual functions for all coupled patches
    // in order to simplify handling of overset meshes
    // HJ, 29/May/2013
    forAll (psi_.boundaryField(), patchI)
    {
        psi_.boundaryField()[patchI].patchFlux
        (
            fieldFlux,
            *this
        );
    }

    if (faceFluxCorrectionPtr_)
    {
        fieldFlux += *faceFluxCorrectionPtr_;
    }

    return tfieldFlux;
}

faceHlduMatrixTemplates.C 中定义

template<class Type>
Foam::tmp<Foam::Field<Type> >
Foam::lduMatrix::faceH(const Field<Type>& psi) const
{
    tmp<Field<Type> > tfaceHpsi
    (
        new Field<Type> (lduAddr().lowerAddr().size())
    );
    Field<Type>& faceHpsi = tfaceHpsi();

    if (lowerPtr_ || upperPtr_)
    {
        const scalarField& Lower = const_cast<const lduMatrix&>(*this).lower();
        const scalarField& Upper = const_cast<const lduMatrix&>(*this).upper();

        const unallocLabelList& l = lduAddr().lowerAddr();
        const unallocLabelList& u = lduAddr().upperAddr();

        for (register label face=0; face<l.size(); face++)
        {
            faceHpsi[face] = Upper[face]*psi[u[face]]
                - Lower[face]*psi[l[face]];
        }
    }
    else
    {
        // No off-diagonal.  Bug fix for conjugate matrices.  HJ, 27/Nov/2008
        faceHpsi = pTraits<Type>::zero;
    }
    
    return tfaceHpsi;
}

Hrv 在 cfd-online.com 上提到:

If your pressure laplacian has a minus sign (-), then it’s

phi = phiHbyA + pEqn().flux()

This is the case in compressible solvers.

For incompressible solvers, the pressure laplacian has a positive sign and it’s

phi = phiHbyA - pEqn().flux()

参考文献

  1. Description of flux() method. https://www.cfd-online.com/Forums/openfoam/114933-description-flux-method.html
  2. https://www.cfd-online.com/Forums/openfoam-programming-development/83638-phi-peqn-flux-vs-linearinterpolate-u-mesh-sf.html
  3. http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2010/implementApplication.pdf
  4. Jasak, H. Error Analysis and Estimation for the Finite Volume Method with Applications to Fluid Flows. PhD thesis. Imperial College London, 1996