有关calculatedFvPatchField

李东岳

某同学来信的错误代码如下：

Starting time loop

Courant Number mean: 0 max: 0
Time = 0.01

time:0.01 curMotionVel_:(0.001 0 0) curLeft:0.099 curRight:0.1
No topology change
Executing mesh motion
GAMG:  Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
PIMPLE: iteration 1
DILUPBiCGStab:  Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCGStab:  Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0


--> FOAM FATAL ERROR: 
cannot be called for a calculatedFvPatchField
    on patch bottom of field p in file "/home/sh/OpenFOAM/sh-5.0/run/171109DyM/HH/0/p"
    You are probably trying to solve for a field with a default boundary condition.

    From function Foam::tmp<Foam::Field<Type> > Foam::calculatedFvPatchField<Type>::gradientInternalCoeffs() const [with Type = double]
    in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 187.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::calculatedFvPatchField<double>::gradientInternalCoeffs() const at ??:?
#3  Foam::fv::gaussLaplacianScheme<double, Foam::SymmTensor<double> >::fvmLaplacianUncorrected(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#4  Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#5  Foam::fv::laplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#6  Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::laplacian<double, double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::word const&) at ??:?
#7  Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::laplacian<double, double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#8  ? at ??:?
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  ? at ??:?
已放弃 (核心已转储)

原因在于你在求解p压力场，因此你不能给定calculatedFvPatchField边界条件。

北山木鱼

东岳老师您好：
上述问题您能再展开说一下嘛？我再求解rho1时遇到了相同的问题。

李东岳

@北山木鱼如果存在变量的Eqn需要solve，就不能调用calculated边界条件。不好意思刚看到

马乔

valueInternalCoeffs, valueBoundaryCoeffs, gradientInternalCoeffs, gradientBoundaryCoeffs are all key coeffs for boundary correct.

In calculatedFvPatchField, those are all:

tmp<Field<Type> > calculatedFvPatchField<Type>::valueInternalCoeffs
(
    const tmp<scalarField>&
) const
{
    FatalErrorIn
    (
        "calculatedFvPatchField<Type>::"
        "valueInternalCoeffs(const tmp<scalarField>&) const"
    )   << "\n    "
...

when construct convection tern

fvm.internalCoeffs()[patchI] = patchFlux*psf.valueInternalCoeffs(pw);
fvm.boundaryCoeffs()[patchI] = -patchFlux*psf.valueBoundaryCoeffs(pw);

and laplacian term

fvm.internalCoeffs()[patchI] = patchGamma*psf.gradientInternalCoeffs();
fvm.boundaryCoeffs()[patchI] = -patchGamma*psf.gradientBoundaryCoeffs();

so...

李东岳

Thanks for sharing

北山木鱼

@东岳好的东岳老师，谢谢东岳老师，实在不好意思，上次断网没发出去刚发现。

CFD中文网

有关calculatedFvPatchField