[Lexe]

Hello,


i desperately seek help for a problem i have with chtMultiRegionSimpleFoam. I try to simlulate a testcase for my thesis. The geometry is a simple cube (SOLIDWURFEL) with a straight, cylindrical oil channel (FLUIDROHR) through it. The oil is supposed to heat the cube.


The problem is, whenever i try to simluate the process, i get one of two error messages:


1) Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux : 291125.4
Specified mass inflow : 7442.71
Specified mass outflow : 0
Adjustable mass outflow : 0


From function bool Foam::adjustPhi(Foam::surfaceScalarField&, const volVectorField&,volScalarField&)
in file cfdTools/general/adjustPhi/adjustPhi.C at line 107.


2) Negative initial temperature T0: -0.6823983

From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hConstThermo<Foam::rhoConst<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::rho Const<Foam::specie> >, Foam::sensibleEnthalpy>]
in file /home/pawan/OpenFOAM/OpenFOAM-v1712/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 54.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam::constTransport<Foam::speci es::thermo<Foam::hConstThermo<Foam::rhoConst<Foam: :specie> >, Foam::sensibleEnthalpy> > > >::calculate(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, bool) at ??:?
#3 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam::constTransport<Foam::speci es::thermo<Foam::hConstThermo<Foam::rhoConst<Foam: :specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:?
#4 ? at ??:?
#5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6 ? at ??:?
Abgebrochen (Speicherabzug geschrieben)


The system folder, the 0 folder and a picture of the geometry are attached. "WURFEL" is the surface of the cube, "ROHRAUSEN" is the shared face of the oil channel and the cube.



I don't have any clue where the problem is and i hope somebody can help me, please. Thanks in advance.

[TomasDenk]

Hi Lexe,


I faced the same problem and I wasn't able to resolve it yet. I also posted question in this forum several weeks ago, but received no answer, so far.


I think, you should also attach constant directory, because I assume you have temperature dependent density of the oil in your case. That turned out to be the major proble maker in my case. With constant density, everything works just fine.


I suspect there is an error in continuity check classes. I use flowRateInletVelocity on the inlet and flowRateOutletVelocity on the outlet boundary conditions for U, both set massFlowRate to 1. I suspect that at some point durig the check, massFlowRate is mixed up with volumetricFlowRate and changing density leads to the error.


I hope someone competent will reply to this thread and post fix or at least workaround.

[Lexe]

I tried to upload the constant folder, but it is simply to big, even if i split it up.

[TomasDenk]

It is probably too big because of mesh. You can remove the mesh and leave only properties. Such .zip file will be small enough.

[Bloerb]

Continuity error cannot be removed by adjusting the outflow

This is due to improper boundary conditions.

Negative initial temperature T0

Most likely as well. It is nevertheless a good idea to add an fvOption to limit the temperature between E.g:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.0                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

    limitT
    {
        type            limitTemperature;
        active          yes;
        limitTemperatureCoeffs
        {
            selectionMode   all;
            min             338;
            max             500;
            Tmin            338; // syntax depends on the of version
            Tmax            500;            
        }
    }

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

I'd like you to test the following

checkMesh -region SOLIDWURFEL -allTopology -allGeometry
checkMesh -region FLUIDROHR -allTopology -allGeometry

Just saw the files you uploaded. The p_rgh outlet condition should be fixedValue. p should be calculated on all boundaries. U at the inlet should be fixedvalue and the outlet should be inletoutlet or zeroGradient.

This solver uses p_rgh to calculate everything. p = p_rgh + rho*g*h is just the absolute pressure which is calculated for your convenience. Hence all boundaries are calculated. You should also check rhoMin and rhoMax in your fvSolution file. Those do not seem appropriate.

[TomasDenk]

Hello Bloerb,


Could you, by any chance, take a look at my case. It uses different setup (BCs), but I experience the same problem with "Continuity error cannot be removed..."
My question in this blog is here


Thanks,
Tomas

[Lexe]

Thank you very much Bloerb.


The simulation is still a bit odd, but at least the errors are gone.

I've added the "corrected" folders, maybe someone finds something to improve the simulation.