[JChristopher]

Hello,

I am trying to run a simulation with dynamic meshing using dynamicRefineFvMesh. I am using the EHD solver from https://github.com/iroghair/openFoamEHD but upgraded it to work on OpenFOAM 8. This issue also exists in OpenFOAM 2.3 and the original unmodified version of the EHD solver. I noticed a pair of warnings in my output:

--> FOAM Warning :
From function Foam::autoPtr<Foam::mapPolyMesh> Foam::dynamicRefineFvMesh::refine(const labelList&)
in file dynamicRefineFvMesh/dynamicRefineFvMesh.C at line 308
Cannot find surfaceScalarField ((interpolate(eps)*magSf)*snGradCorr(Ue)) in user-provided flux mapping table
12
(
rhoPhi none
phi none
nHatf none
alphaPhi0.phase1 none
alphaPhiUn none
rhoEFlux none
rho*phi none
Ue none
ghf none
phiAbs none
rhoE none
alphaPhi none
)
The flux mapping table is used to recreate the flux on newly created faces.
Either add the entry if it is a flux or use (((interpolate(eps)*magSf)*snGradCorr(Ue)) none) to suppress this warning.
--> FOAM Warning :
From function Foam::autoPtr<Foam::mapPolyMesh> Foam::dynamicRefineFvMesh::refine(const labelList&)
in file dynamicRefineFvMesh/dynamicRefineFvMesh.C at line 308
Cannot find surfaceScalarField ((-interpolate(sgm)*magSf)*snGrad(Ue)) in user-provided flux mapping table
12
(
rhoPhi none
phi none
nHatf none
alphaPhi0.phase1 none
alphaPhiUn none
rhoEFlux none
rho*phi none
Ue none
ghf none
phiAbs none
rhoE none
alphaPhi none
)
The flux mapping table is used to recreate the flux on newly created faces.
Either add the entry if it is a flux or use (((-interpolate(sgm)*magSf)*snGrad(Ue)) none) to suppress this warning.

I added the suggested suppression to dynamicMeshDict/correctFluxes:

  correctFluxes
    (
     (phi none)
     (rhoPhi none)
     (ghf none)
     (alphaPhi none)
     (alphaPhiUn none)
     (alphaPhi0.phase1 none)
     (Ue none)
     (rhoE none)
     (nHatf none)
     (rho*phi none)
     (phiAbs none)
     (rhoEFlux none)
     (((-interpolate(sgm)*magSf)*snGrad(Ue)) none)
     );

However this gives the error:

[3] --> FOAM FATAL IO ERROR:
[3] wrong token type - expected word, found on line 0 the punctuation token '('
[3]
[3] file: IOstream/dynamicRefineFvMeshCoeffs/correctFluxes at line 0.
[3]
[3] From function Foam::Istream& Foam::operator>>(Foam::Istream&, Foam::word&)

The code where this expressions is used is:

             surfaceScalarField rhoEFlux = -fvc::interpolate(sgm)*mesh.magSf()*fvc::snGrad(Ue);
             fvScalarMatrix rhoEEqn
             (
                 fvm::ddt(rhoE)
               + fvm::div(phi, rhoE)
               + fvc::div(rhoEFlux)
             );
              rhoEEqn.solve();

This issue is essentially identical to this thread:

dynamic Mesh, correct fluxes, surfaceScalarFields

However, that thread was not resolved and the suggestions in that thread did not help me. As you can see in the correctFluxes above, I also tried putting (rhoEFlux none) into correctFluxes.


Does anyone have any suggestions on how to correctly add that surfaceScalarField with parenthesis into correctFluxes?


Thank you,
Joshua

[JChristopher]

Hello everyone,

I was able to resolve the warning by making the following changes to the solver:

1. In createFields.H, create the surfaceScalarField for rhoEFlux:

surfaceScalarField rhoEFlux
(
    IOobject
    (
        "rhoEFlux",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::NO_WRITE
    ),
    -fvc::interpolate(sgm)*mesh.magSf()*fvc::snGrad(Ue)
 );

2. In the solver instead of creating a temporary surfaceScalarField at each time step, I just compute the update to the rhoEFlux that is now in createFields.H:

rhoEFlux = -fvc::interpolate(sgm)*mesh.magSf()*fvc::snGrad(Ue);

This seems to be sufficient for OpenFOAM to detect the flux by the name RhoEFlux.


3. In dynamicMeshDict my correctFluxes looks like:

  correctFluxes
    (
     (phi none)
     (rhoPhi none)
     (ghf none)
     (alphaPhi none)
     (alphaPhiUn none)
     (alphaPhi0.phase1 none)
     (Ue none)
     (rhoE none)
     (nHatf none)
     (rho*phi none)
     (phiAbs none)
     (rhoEFlux none)
     );

to perform no flux corrections of rhoEFlux.


In my original post you notice there are two warnings, one for the positive and one for the negative sign on rhoEFlux. I had to duplicate this process and swap the sign to get the second warning to go away.

I don't know if this is a workaround or the correct method of resolving this, but the warning is gone so presumably I can now correct the rhoEFlux by velocity.


Thanks,
Joshua