[Sk Hossen Ali]

Dear Foamers,

I am trying to validate the capability of reaction part of reactingTwoPhaseEulerFoam solver.

Although the solver is multiphase, I am interested to solve only one phase currently i.e., gas phase.

I am trying to simulate flow reaction of H2/O2 gases considering detailed kinetics.

From one end H2 and O2 gas will enter with a composition (say 0.5 mass fraction each) at an initial temperature of 800K (high temperature, so that reaction happens quickly)

Error File Output :

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create mesh for time = 0
PIMPLE: no residual control data found. Calculations will employ 3 corrector loops

Reading g

Reading hRef
Creating phaseSystem

Selecting twoPhaseSystem thermalPhaseChangeTwoPhaseSystem
Selecting phaseModel for H2O2Gas: reactingPhaseModel
Selecting diameterModel for phase H2O2Gas: constant
Selecting thermodynamics package 
{
    type            heRhoThermo;
    mixture         reactingMixture;
    transport       sutherland;
    thermo          janaf;
    energy          sensibleInternalEnergy;
    equationOfState perfectGas;
    specie          specie;
}

Selecting chemistryReader foamChemistryReader
Calculating face flux field phi.H2O2Gas
Selecting turbulence model type laminar
Selecting laminar stress model Stokes
Selecting combustion model laminar
Selecting chemistry solver 
{
    solver          ode;
    method          standard;
}

StandardChemistryModel: Number of species = 10 and reactions = 27
Selecting ODE solver seulex
    using integrated reaction rate
Selecting phaseModel for H2O2Liq: purePhaseModel
Selecting diameterModel for phase H2O2Liq: constant
Selecting thermodynamics package 
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          eConst;
    equationOfState perfectFluid;
    specie          specie;
    energy          sensibleInternalEnergy;
}

Calculating face flux field phi.H2O2Liq
Selecting turbulence model type laminar
Selecting laminar stress model Stokes
No MRF models present

Selecting default blending method: none
Selecting saturationModel: constant
Calculating field g.h

Reading field p_rgh

Courant Number mean: 0 max: 0

Starting time loop

fieldAverage fieldAverage1:
    Restarting averaging for fields:
        U.H2O2Gas: starting averaging at time 0
        U.H2O2Liq: starting averaging at time 0
        alpha.H2O2Gas: starting averaging at time 0
        p: starting averaging at time 0

Courant Number mean: 0 max: 0
Max Ur Courant Number = 0
Time = 1e-07

PIMPLE: iteration 1
MULES: Solving for alpha.H2O2Gas
MULES: Solving for alpha.H2O2Gas
alpha.H2O2Gas volume fraction = 1  Min(alpha1) = 1  Max(alpha1) = 1
smoothSolver:  Solving for H2.H2O2Gas, Initial residual = 0.998572, Final residual = 0.0309635, No Iterations 1000
smoothSolver:  Solving for H.H2O2Gas, Initial residual = 0, Final residual = 0, No Iterations 1
smoothSolver:  Solving for O2.H2O2Gas, Initial residual = 0.998572, Final residual = 0.0309635, No Iterations 1000
smoothSolver:  Solving for O.H2O2Gas, Initial residual = 0, Final residual = 0, No Iterations 1
smoothSolver:  Solving for OH.H2O2Gas, Initial residual = 0, Final residual = 0, No Iterations 1
smoothSolver:  Solving for HO2.H2O2Gas, Initial residual = 0, Final residual = 0, No Iterations 1
smoothSolver:  Solving for H2O2.H2O2Gas, Initial residual = 0, Final residual = 0, No Iterations 1
smoothSolver:  Solving for H2O.H2O2Gas, Initial residual = 0, Final residual = 0, No Iterations 1
smoothSolver:  Solving for AR.H2O2Gas, Initial residual = 0, Final residual = 0, No Iterations 1
Constructing momentum equations
smoothSolver:  Solving for e.H2O2Gas, Initial residual = 0.0390438, Final residual = 0.0231076, No Iterations 1000
smoothSolver:  Solving for e.H2O2Liq, Initial residual = 0.00341936, Final residual = 0.00281149, No Iterations 1000
Fluid1 min/max(T) = 800, 800
Fluid1 min/max(T) = 800, 800


--> FOAM FATAL ERROR: (openfoam-2106)

    request for volVectorField U from objectRegistry region0 failed
    available objects of type volVectorField are
8(HbyA.H2O2Liq U.H2O2Liq_0 HbyA.H2O2Gas HbyA.H2O2Liq_0 U.H2O2Gas HbyA.H2O2Gas_0 U.H2O2Liq U.H2O2Gas_0)

    From const Type& Foam::objectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>]
    in file /home/ali/OpenFOAM/ali-v2106/OpenFOAM-v2106/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 463.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::exitOrAbort(int, bool) at ??:?
#2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&, bool) const at ??:?
#3  Foam::totalPressureFvPatchScalarField::updateCoeffs() at ??:?
#4  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) in ~/OpenFOAM/ali-v2106/OpenFOAM-v2106/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam
#5  Foam::fv::EulerDdtScheme<double>::fvmDdt(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#6  Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::ddt<double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in ~/OpenFOAM/ali-v2106/OpenFOAM-v2106/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam
#7  ? in ~/OpenFOAM/ali-v2106/OpenFOAM-v2106/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam
#8  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#9  ? in ~/OpenFOAM/ali-v2106/OpenFOAM-v2106/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam
Aborted (core dumped)

From the above it is obvious what is the phaseProperties files composed of.

I believe there is some problem with pressure and velocity boundary conditions.
BC for me is simple inlet with specified composition and velocity and the outlet is open.

The p_rgh file:

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

internalField       uniform 5e5;

boundaryField
{
    inlet
    {
        type            zeroGradient;
        // type            fixedFluxPressure;
        // value           $internalField;
    }

    outlet
    {
        // type            zeroGradient;
        type            totalPressure;
        p0              uniform 5e5;
    }

    frontBackTopBottom
    {
        type            empty;
    }
}

The p file :

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

internalField       uniform 5e5;

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

    outlet
    {
        type               calculated;
        value              $internalField;
    }

    frontBackTopBottom
    {
        type               empty;
    }
}

The U.H2O2Gas file is :

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

internalField   uniform (0 0 0);

boundaryField
{
    inlet
    {
        type               fixedValue;
        value              uniform (0 0.025 0);
    }

    outlet
    {
        type               fixedValue;
        value              uniform (0 0 0);
    }

    frontBackTopBottom
    {
        type               empty;
    }
}

The U.H2O2Liq file is :

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

internalField   uniform (0 0 0);

boundaryField
{
    inlet
    {
        type               fixedValue;
        value              uniform (0 0 0);
    }

    outlet
    {
        type               fixedValue;
        value              uniform (0 0 0);
    }

    frontBackTopBottom
    {
        type               empty;
    }
}

Earlier also I was getting the same error and I got away from it by manipulating in the U or p BC which I don't remember now.

Any help would be highly appreciated.

Thanks in advance.

[fripa]

The problem is that totalPressure uses the velocity field to calculate the total pressure. As default it looks up "U" as the velocity field. You can however specify which phase you intend to use for the velocity field by adding the following line to the outlet pressure BC:

    
outlet
    {
        // type            zeroGradient;
        type            totalPressure;
        U                U.gas;
        p0              uniform 5e5;
    }