[massive_turbulence]

Hello all,

I would love an explanation as to why this isn't functioning. I've looked over the theory of why this solver runs and I still cannot imagine why I'd get a negative temperature for the initial case.

Here's the output of the error running the hotRoom tutorial with buoyantPimpleFoam

Courant Number mean: -6.65662e-05 max: 4.57604e-07
Time = 3e-07

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCGStab:  Solving for Ux, Initial residual = 0.00268968, Final residual = 4.59223e-15, No Iterations 1
DILUPBiCGStab:  Solving for Uy, Initial residual = 0.00269014, Final residual = 4.60139e-15, No Iterations 1
DILUPBiCGStab:  Solving for Uz, Initial residual = 0.00268968, Final residual = 4.59223e-15, No Iterations 1

DILUPBiCGStab:  Solving for h, Initial residual = 0.19232, Final residual = 1.63083e-12, No Iterations 1

--> FOAM FATAL ERROR: 
Negative initial temperature T0: -91630.1

    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::perfectGas<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>]
    in file /mnt/external/OpenFOAM/OpenFOAM-v1806/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 54.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<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::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:?
#4  ? in /mnt/external/OpenFOAM/OpenFOAM-v1806/platforms/linux64GccDPInt32Opt/bin/buoyantPimpleFoam
#5  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#6  ? in /mnt/external/OpenFOAM/OpenFOAM-v1806/platforms/linux64GccDPInt32Opt/bin/buoyantPimpleFoam

Basically I setup the case with
blockMesh
setFields
foamJob -s buoyantPimpleFoam

The machines file is obviously my machine so you may need to change that to run it. I attached the entire case as a zip hotRoom.zip


I only made changes to the pressure files, here's p

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1806                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 1e2;

boundaryField
{
    floor
    {
        type            calculated;
        value           $internalField;
    }

    ceiling
    {
        type            calculated;
        value           $internalField;
    }

    fixedWalls
    {
        type            calculated;
        value           $internalField;
    }
}

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

p_rgh file

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1806                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 1e2;

boundaryField
{
    floor
    {
        type            fixedFluxPressure;
        value           $internalField;
    }

    ceiling
    {
        type            fixedFluxPressure;
        value           $internalField;
    }

    fixedWalls
    {
        type            fixedFluxPressure;
        value           $internalField;
    }
}

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

I tried using smaller time steps as well from .01 to .0000001; to no luck?

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1806                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     buoyantPimpleFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         2000;

deltaT          .0000001;

writeControl    timeStep;

writeInterval   100;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

adjustTimeStep  no;

maxCo           0.5;

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

[pete20r2]

Do you want to know why this is happening or just how to fix it? I can suggest utilising the limitTemperature function in fvOptions with some reasonable limits. Your issue is likely that the initial conditions are either bad or non-physical, although I have heard of parallel sometimes affecting convergence, although I think that was a bug and not normal behaviour.
https://www.openfoam.com/documentati...mperature.html

Or try initialising with a steady-state solver.

(Sorry for the long link, I'm on my phone)

[massive_turbulence]

Originally Posted by pete20r2

Do you want to know why this is happening or just how to fix it? I can suggest utilising the limitTemperature function in fvOptions with some reasonable limits. Your issue is likely that the initial conditions are either bad or non-physical, although I have heard of parallel sometimes affecting convergence, although I think that was a bug and not normal behaviour.
https://www.openfoam.com/documentati...mperature.html

Or try initialising with a steady-state solver.

(Sorry for the long link, I'm on my phone)

It's actually the fvSolution file that needs a minor tweak. In the section for PIMPLE that looks like

PIMPLE
{
    momentumPredictor yes;
    nOuterCorrectors 1;
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       1e2;
}

I changed the pRefValue from 1e5 to the one shown above and then in object p_rgh I changed to this internalField uniform 1e1; and also in object p to internalField uniform 1e2; and the timestep is deltaT .0000001;. These changes made it work.

Not positive if this is the best fix; ran it for a while but at small timesteps, not sure if running it at 1/1000th would still work but that would be ideal.

If you want to explain the theory why the solver got negative temperature that would be fine. I would like to read your explanation. Thanks!