[hester]

Hello,

I'm simulating a bubble column after Denn [1]. My simulation setup is similar to this:
http://http://www.cfd-online.com/For...le-column.html.
I'm using OpenFoam 2.3.0.

I want to use turbulentMixingLengthDissipationRateInlet as the inlet BC instead of fixedValue for epsilon. It works fine for epsilon.air but for epsilon.water it gives me the following error message when the solver tries to solve for epsilon.water:

--> FOAM FATAL ERROR:

request for volScalarField k from objectRegistry region0 failed
available objects of type volScalarField are

47
(
div(phi.water)
k.water
K.air_0
e.air_0
yWall
kEpsilon:G
T.air
thermo:psi.water
K.air_0_0
dragModelCoeff
dpdt
thermo:psi.air
thermo:rho.water_0
p
K.air
p_0
thermo:mu.water
e.air
p_0_0
thermo:mu.air
dgdt
nut.water
thermo:alpha.air
epsilon.water
alpha.air_0
alpha.water_0
thermo:alpha.water
e.water_0
alpha.water_0_0
alpha.water
rho
T.water
e.air_0_0
thermo:rho.air_0_0
e.water_0_0
thermo:rho.air
thermo:rho.water
K.water
alpha.air
K.water_0
thermo:rho.water_0_0
alpha.air_0_0
thermo:rho.air_0
e.water
rAU.air
rAU.water
K.water_0_0
)


From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::Geometric Field<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3 Foam::turbulentMixingLengthDissipationRateInletFvP atchScalarField::updateCoeffs() at ??:?
#4 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::updateCoef fs() at ??:?
#5 Foam::RASModels::kEpsilon<Foam::PhaseIncompressibl eTurbulenceModel<Foam::phaseModel> >::correct() at ??:?
#6
at ??:?
#7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8
at ??:?

I'm not sure what this error message is saying. When I use fixedValue instead of turbulentMixingLengthDissipationRateInlet I get no error message and the simulation works fine. k at the inlet is calculated using turbulentIntensityKineticEnergyInlet for both phases.

Am I even supposed to used turbulentMixingLengthDissipationRateInlet for both phases? I used k-epsilon-model only for my continuous phase (water). My bubbles (air) are modeled as laminar. Might that be the problem?


hester


[1] N. G. Deen, T. Solberg, and B. H. Hjertager. Large eddy simulation of the gas-liquid flow in a square cross-sectioned bubble column. Chemical Engineering Science, 56:6341–6349, 2001.

[hester]

I figured it out myself. I just needed to specify the k field.

        type          turbulentMixingLengthDissipationRateInlet;
        mixingLength  1e-3;
        k             k.water;
        value         uniform 0;

Normally it is not required to specify k. The default value is just k but I needed k.water instead.

[GerhardHolzinger]

This behaviour is a consequence of the naming scheme. The BC expects a field k to be present. However, in the two-phase case, you have k.air and k.water but no k. Hence, OpenFOAM issued the error message you posted in your first post.