[sahm]

Hello Everyone, What's the plan?
I wish you had a good thanksgibing.
recently I'm trying to run a case with reactingFoam using LES turbulence model. I set up my case, changing the Turbulence model to LES and changing some of fields ( like alphaSGS and muSGS) but when I run the case I get this error in the first place:

--> FOAM FATAL ERROR: 

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

19
(
psi
N2
C3H8
kappa
rho
CO2
k
O2
psi_0
delta
alpha
p
T
alphaSgs
H2O
geometricDelta
mu
hs
muSgs
)


    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/nini/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 139.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::error::abort() in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#2  Foam::Ostream& Foam::operator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/reactingFoam"
#3  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#4  Foam::compressible::LESModels::alphaSgsJayatillekeWallFunctionFvPatchScalarField::evaluate(Foam::Pstream::commsTypes) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#5  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/reactingFoam"
#6  Foam::compressible::LESModels::oneEqEddy::updateSubGridScaleFields() in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#7  Foam::compressible::LESModels::oneEqEddy::oneEqEddy(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#8  Foam::compressible::LESModel::adddictionaryConstructorToTable<Foam::compressible::LESModels::oneEqEddy>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#9  Foam::compressible::LESModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#10  Foam::compressible::turbulenceModel::addturbulenceModelConstructorToTable<Foam::compressible::LESModel>::NewturbulenceModel(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#11  Foam::compressible::turbulenceModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleTurbulenceModel.so"
#12  main in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/reactingFoam"
#13  __libc_start_main in "/lib64/libc.so.6"
#14  Foam::regIOobject::writeObject(Foam::IOstream::streamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/reactingFoam"

I think the problem is due to my thermophysical model. I think the reactingFoam is looking for a field like h ( total enthalpy ) but It should be looking for hs. At this point I don't know where I should change this option to look for hs, or add this model as an option to compressible LES. Any body can help me with this?

[tuominen]

Originally Posted by sahm

Hello Everyone, What's the plan?
I wish you had a good thanksgibing.
recently I'm trying to run a case with reactingFoam using LES turbulence model. I set up my case, changing the Turbulence model to LES and changing some of fields ( like alphaSGS and muSGS) but when I run the case I get this error in the first place:

--> FOAM FATAL ERROR: 

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

19
(
psi
N2
C3H8
kappa
rho
CO2
k
O2
psi_0
delta
alpha
p
T
alphaSgs
H2O
geometricDelta
mu
hs
muSgs
)


    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/nini/OpenFOAM/OpenFOAM-1.7.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 139.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::error::abort() in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libOpenFOAM.so"
#2  Foam::Ostream& Foam::operator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/reactingFoam"
#3  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#4  Foam::compressible::LESModels::alphaSgsJayatillekeWallFunctionFvPatchScalarField::evaluate(Foam::Pstream::commsTypes) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#5  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/reactingFoam"
#6  Foam::compressible::LESModels::oneEqEddy::updateSubGridScaleFields() in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#7  Foam::compressible::LESModels::oneEqEddy::oneEqEddy(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#8  Foam::compressible::LESModel::adddictionaryConstructorToTable<Foam::compressible::LESModels::oneEqEddy>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#9  Foam::compressible::LESModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#10  Foam::compressible::turbulenceModel::addturbulenceModelConstructorToTable<Foam::compressible::LESModel>::NewturbulenceModel(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleLESModels.so"
#11  Foam::compressible::turbulenceModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&) in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/lib/linux64GccDPOpt/libcompressibleTurbulenceModel.so"
#12  main in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/reactingFoam"
#13  __libc_start_main in "/lib64/libc.so.6"
#14  Foam::regIOobject::writeObject(Foam::IOstream::streamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/home/sahm/OpenFOAM/OpenFOAM-1.7.0/applications/bin/linux64GccDPOpt/reactingFoam"

I think the problem is due to my thermophysical model. I think the reactingFoam is looking for a field like h ( total enthalpy ) but It should be looking for hs. At this point I don't know where I should change this option to look for hs, or add this model as an option to compressible LES. Any body can help me with this?

I had the same problem some time ago in OF 1.7.1.
I changed in file "OpenFOAM-1.7.x/src/turbulenceModels/compressible/LES/derivedFvPatchFields/wallFunctions/alphaSgsWallFunctions/alphaSgsJayatillekeWallFunction/alphaSgsJayatillekeWallFunctionFvPatchScalarField. C" line 212 to
patch().lookupPatchField<volScalarField, scalar>("hs");

And after that compiled OF again.

[yashar.afarin]

Originally Posted by sahm

recently I'm trying to run a case with reactingFoam using LES turbulence model. I set up my case, changing the Turbulence model to LES and changing some of fields ( like alphaSGS and muSGS) but when I run the case I get this error in the first place:

Hi Ali,

I really need to run my case with reactingFoam using LES. could you please describe me which filed I should change? did you have any tutorial about using reactingFoam with LES?

[ni-openfoam-user]

Hi Yashar,

Did you ever solve this problem? I am currently trying to switch from RAS to LES using reactingFoam and am getting the following error message:

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

I guess it's something to do with the setup of the 0 folder.

What files do you need to change when switching from RAS to LES?

I look forward to hearing from you.

James

[babakflame]

Greetings James

As I know yashar is no longer working on O.F.

However, for your case you need to have muSgs and alphaSgs files instead of mut and alphat. Also k in LES is completely different with RAS.

For setting the abovementioned files, just take a look at firefoam and pisoFoam and rhoPimpleFoam tutorials.

Hope this helps you

Regards
Bobi

[reza_65]

if somebody else face the same problem, here is the solution:

You need to change your alphaSgs file, e.g:

boundaryField
{
wall
{
// type alphaSgsJayatillekeWallFunction;
type alphaSgsWallFunction;
hs h;
value uniform 0;
}

................

Good luck.
Reza