[Jabo]

Hi guys,

My first post here.

I'm modifying the existing aachenBomb tutorial, to simulate the experiments done by Mayer et. al. - "Raman Measurements of Cryogenic Injection at Supercritical Pressure"

I need to be able to use the PengRobinsonGas equation of state. I've built OF 2.3.x from the GitHub source today.

I modified my thermophysicalProperties as such:

thermoType
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       sutherland;
    thermo          hConst;
    energy          sensibleEnthalpy;
    equationOfState PengRobinsonGas;
    specie          specie;
}

and my combustionProperties as such:

combustionModel noCombustion<psiThermoCombustion>;
active    false;

I made those modifications as that's what's details in the psiThermos source, https://github.com/OpenFOAM/OpenFOAM...o/psiThermos.C

chemistryProperties is set as such:

chemistryType
{
    chemistrySolver   noChemistrySolver;
    chemistryThermo   psi;
}

chemistry       off;

This produces an 'Unknown psiReactionThermo type' error and the valid types listed does not contain PengRobinsonGas under the equationOfState. Only perfectGas.

So how do I go about making this work or is it a bug?

[Jabo]

So I realised I had to build a new psiReactionThermo:

makeReactionThermo
(
    psiThermo,
    psiReactionThermo,
    hePsiThermo,
    reactingMixture,
    sutherlandTransport,
    sensibleEnthalpy,
    janafThermo,
    PengRobinsonGas,
    specie
);

I compiled the psiReactionThermo without error but attempting to compile sprayFoam gave this error:

/home/james/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so: undefined reference to `Foam::chemistryReader<Foam::sutherlandTransport<F oam::species::thermo<Foam::janafThermo<Foam::PengR obinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::dictionaryConstructorTablePtr_'
collect2: error: ld returned 1 exit status
make: *** [/home/james/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/bin/sprayFoam] Error 1


I've tried cleaning and making the model and the solver.

Please help!

[Jabo]

I think I'm not rebuilding everything that I should be or I'm just missing a step. I edited the thermo model, rebuilt it and rebuilt the solver.

What have I missed?

[Jabo]

Ok, here's what I missed.

To run my simulations with:

thermoType
{
    type            hePsiThermo;
    mixture         reactingMixture;
    transport       sutherland;
    thermo          janaf;
    energy          sensibleEnthalpy;
    equationOfState PengRobinsonGas;
    specie          specie;
}

I had to create:

typedef
    sutherlandTransport
    <
        species::thermo
        <
            janafThermo
            <
                PengRobinsonGas<specie>
            >,
            sensibleEnthalpy
        >
    > PengRobinsonGasPhysics;

in thermophysicalModels/species/include/thermoPhysicsTypes.H

and,

 typedef Reaction<PengRobinsonGasPhysics> PengRobinsonGasReaction;

in reactionTypes.H in that folder,

and,

makeReactionMixtureThermo
(
    psiThermo,
    psiReactionThermo,
    hePsiThermo,
    reactingMixture,
    PengRobinsonGasPhysics
);

in psiReactionThermos.C, and

makeChemistryReader(PengRobinsonGasPhysics);
makeChemistryReaderType(foamChemistryReader, PengRobinsonGasPhysics);

in reactionThermo/chemistryReaders/chemistryReader/makeChemistryReaders.C, and

makeReactions(PengRobinsonGasPhysics, PengRobinsonGasReaction)

in specie/reaction/reactions/makeReactions.C

I believe that's it. Allwmake the thermophysicalModels and the sprayFoam solver.

Figured that all out by myself

[arashfluid]

Did you fix undefined reference error?

[Jabo]

Yeah, my modifications fixed that error.

[arashfluid]

Which of the above code you added recently?
I have added variable and source term equation to icoflow.H and icoflow.C files.Should I add something else?

[Jabo]

I don't know about that one. My solution is to add new equations of state to the existing psiReactionThermo model. I think ours problems are unrelated.

[PeterBishop]

Hi Jabo,
I'm trying to modify the source code according to your suggestions but with no succes!

Could you please share your files to let me understand where I'm wrong, thank you!

[john myce]

Hi everyone,

I am working on the same subject, did you succeed to set up the sprayFoam solver to visualise LN2 with the Janaf table ? Because the initial range of temperature is from 200 K to 6000 K.

Cheers

[john myce]

By the way the method written by James works for me.
I have attached my files in case someone has an error.

Make for specie directory:

atomicWeights/atomicWeights.C
specie/specie.C
reaction/reactions/makeReactions.C
reaction/reactions/makeLangmuirHinshelwoodReactions.C

LIB = $(FOAM_USER_LIBBIN)/libspecie

Make for reactionthermo directory:

chemistryReaders/chemkinReader/chemkinReader.C
chemistryReaders/chemkinReader/chemkinLexer.L
chemistryReaders/chemistryReader/makeChemistryReaders.C

mixtures/basicMultiComponentMixture/basicMultiComponentMixture.C
mixtures/basicSpecieMixture/basicSpecieMixture.C
mixtures/basicCombustionMixture/basicCombustionMixture.C

psiReactionThermo/psiReactionThermo.C
psiReactionThermo/psiReactionThermos.C

psiuReactionThermo/psiuReactionThermo.C
psiuReactionThermo/psiuReactionThermos.C

rhoReactionThermo/rhoReactionThermo.C
rhoReactionThermo/rhoReactionThermos.C

derivedFvPatchFields/fixedUnburntEnthalpy/fixedUnburntEnthalpyFvPatchScalarField.C
derivedFvPatchFields/gradientUnburntEnthalpy/gradientUnburntEnthalpyFvPatchScalarField.C
derivedFvPatchFields/mixedUnburntEnthalpy/mixedUnburntEnthalpyFvPatchScalarField.C

functionObjects/moleFractions/moleFractionsFunctionObjects.C

LIB = $(FOAM_USER_LIBBIN)/libreactionThermophysicalModels

EXE_INC = \
    -I$(LIB_SRC)/transportModels/compressible/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
    -I$(WM_PROJECT_USER_DIR)/src/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/solidSpecie/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude

LIB_LIBS = \
    -lcompressibleTransportModels \
    -lfluidThermophysicalModels \
    -L$(FOAM_USER_LIBBIN)/lspecie \
    -lsolidSpecie \
    -lfiniteVolume

[mickbatti]

Hi John

I am trying to use your files, based on the method described by James. I compiled my thermophysicalModels library and also compiled a new reactingFoam with this library.
Now, if I test the solver using PengRobinsonGas on the tutorial case counterFlowFlame2D, deactivating the combustion as above, I get stuck. The code does not give me errors, but it stops after "foamChemistryReader"

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 3.0.1-d8a290b55d28
Exec   : myReactingFoam
Date   : Oct 24 2018
Time   : 00:28:40
PID    : 4838
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


PIMPLE: Operating solver in PISO mode


Reading g
Creating reaction model

Selecting combustion model noCombustion<psiThermoCombustion>
Selecting thermodynamics package
{
    type            hePsiThermo;
    mixture         reactingMixture;
    transport       sutherland;
    thermo          janaf;
    energy          sensibleEnthalpy;
    equationOfState PengRobinsonGas;
    specie          specie;
}

Selecting chemistryReader foamChemistryReader

Any ideas why?
I think the foamChemistryReader needs some modifications to work with PengRobinsonGas, but can't figure it out

[john myce]

Hi,

Strange.. since we have added the pengrobinson physics to the foamChemistryReader I don t think it needs something else. Maybe try to run the simulation with the basic solver and add in the controlDict file the modified reactionthermo and the specie libraries.

Like:

libs
{
        "libname.so"
        "libname.so"
}

Another question: Did you just add the pengrobinsongas instead of perfectGas or you made some others modifications in the initial tutorial case.

[mickbatti]

I put PengRobinson in the thermoType and adapted the test case setup, turning off combustion and providing necessary information for PR for each species.
I’ve tried with including libs in the controlDict and using the base solver, but same problem.
I'm using of301.

Can you tell me if you have tried with reactingFoam? Or just with sprayFoam?

[john myce]

Hello,

Just with sprayFoam.

[john myce]

Hi Mick


Did you solve your pb ?

[mickbatti]

Hi John

yes, I solved moving to openfoam 6. Not sure if this was the only possibility, but now I am able to compile a custom reactingFoam with a mixture of PR fluids.

[tmaffei]

Hi Mick,

I am trying to add PengRobinson EoS to reactingFoam in oF-6 following the tips provided by John.
I have adopted the case accordingly, adding equationOfState parameters for each species. My domain is a 2D planar system in which occurs a single step reaction A->B.

As happened to you, the simulation stops after "foamChemistryReader" with the following list of error:

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::Reaction<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::setThermo(Foam::HashPtrTable<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> >, Foam::word, Foam::string::hash> const&) at ??:?
#4  Foam::Reaction<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::Reaction(Foam::hashedWordList const&, Foam::HashPtrTable<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> >, Foam::word, Foam::string::hash> const&, Foam::dictionary const&) at ??:?
#5  Foam::Reaction<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::adddictionaryConstructorToTable<Foam::IrreversibleReaction<Foam::Reaction, Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> >, Foam::ArrheniusReactionRate> >::New(Foam::hashedWordList const&, Foam::HashPtrTable<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> >, Foam::word, Foam::string::hash> const&, Foam::dictionary const&) at ??:?
#6  Foam::Reaction<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::New(Foam::hashedWordList const&, Foam::HashPtrTable<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> >, Foam::word, Foam::string::hash> const&, Foam::dictionary const&) at ??:?
#7  Foam::ReactionList<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::readReactionDict() at ??:?
#8  Foam::foamChemistryReader<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::foamChemistryReader(Foam::dictionary const&, Foam::hashedWordList&) at ??:?
#9  Foam::chemistryReader<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::adddictionaryConstructorToTable<Foam::foamChemistryReader<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::New(Foam::dictionary const&, Foam::hashedWordList&) at ??:?
#10  Foam::chemistryReader<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::New(Foam::dictionary const&, Foam::hashedWordList&) at ??:?
#11  Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::reactingMixture(Foam::dictionary const&, Foam::fvMesh const&, Foam::word const&) at ??:?
#12  Foam::heThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::heThermo(Foam::fvMesh const&, Foam::word const&) at ??:?
#13  Foam::psiReactionThermo::addfvMeshConstructorToTable<Foam::hePsiThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::PengRobinsonGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > > >::New(Foam::fvMesh const&, Foam::word const&) at ??:?
#14  Foam::autoPtr<Foam::psiReactionThermo> Foam::basicThermo::New<Foam::psiReactionThermo>(Foam::fvMesh const&, Foam::word const&) at ??:?
#15  Foam::psiReactionThermo::New(Foam::fvMesh const&, Foam::word const&) at ??:?
#16  ? in "/opt/OpenFOAM/OpenFOAM-6/platforms/linux64GccDPInt64Opt/bin/reactingFoam"
#17  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#18  ? in "/opt/OpenFOAM/OpenFOAM-6/platforms/linux64GccDPInt64Opt/bin/reactingFoam"

Could you help me?

Thanks in advance

Tiziano

[mickbatti]

Hi Tiziano,
my problem was with of301, then moving to of6 and recompiling again I didn't get the foamChemistryReader error anymore.
My error was without messages, so somewhat different from yours. What type of thermoType are you using? Mine was:

thermoType
{
type hePsiThermo;
mixture reactingMixture;
transport sutherland;
thermo janaf;
energy sensibleEnthalpy;
equationOfState PengRobinsonGas;
specie specie;
}

[tmaffei]

Hi Mick,

thanks for your answer. At the end I have found the error and now I can able to use PengRobinsonGas Eos with reactingFoam.
Furthermore, I have modified the mixing rules applied to critical pressure, temperature and so on using molar fraction instead of mass fraction. In this way my results are more similar to ones obtained with other software like fluent or unisim.

Thanks for your availability

Tiziano