[shenzhou1987]

Hi, everyone. I'm using OpenFOAM 2.3.0 to simulate the jet flow of a nozzle which contains two species, gas and air. I just want to study the process of jet gas mixing into the air without combustion and reaction. After reading the User Guide, I think reactingFoam could be a suitalbe solver for my case. And I have read some threads in the forum which mentioned this problem, some one said combustion and reaction model can be switched off in reactingFoam. But there is no details about how to switch off combustion and reaction in reactingFoam. I open the tutorial case "counterFlowFlame2D", in folder "constant" I copy file chemistryProperties, combustionProperties and thermophysicalProperties to my case folder and modify them. Then I execute "reactingFoam" command. Some errors are reported as blow and the relation files are attached. Can anybody tell me what's wrong with my case files? Thank you!

Error:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0
Exec   : reactingFoam
Date   : Jan 13 2015
Time   : 23:20:54
Host   : "localhost.localdomain"
PID    : 32121
Case   : /home/shenzhou1987/OpenFOAM/Jet/2D-axis
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create mesh for time = 0


Reading g
Creating reaction model

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



--> FOAM FATAL IO ERROR: 
Attempt to return dictionary entry as a primitive

file: /home/shenzhou1987/OpenFOAM/Jet/2D-axis/constant/thermophysicalProperties.species

    From function ITstream& primitiveEntry::stream() const
    in file db/dictionary/dictionaryEntry/dictionaryEntry.C at line 83.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::IOerror::abort() in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::dictionaryEntry::stream() const in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#3  Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::multiComponentMixture(Foam::dictionary const&, Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#4  Foam::SpecieMixture<Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::SpecieMixture(Foam::dictionary const&, Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#5  Foam::heThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::heThermo(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#6  Foam::hePsiThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::hePsiThermo(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#7  Foam::psiReactionThermo::addfvMeshConstructorToTable<Foam::hePsiThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > > >::New(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#8  Foam::autoPtr<Foam::psiReactionThermo> Foam::basicThermo::New<Foam::psiReactionThermo>(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#9  Foam::psiReactionThermo::New(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#10  Foam::combustionModels::psiThermoCombustion::psiThermoCombustion(Foam::word const&, Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcombustionModels.so"
#11  Foam::combustionModels::psiCombustionModel::adddictionaryConstructorToTable<Foam::combustionModels::noCombustion<Foam::combustionModels::psiThermoCombustion> >::New(Foam::word const&, Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcombustionModels.so"
#12  Foam::combustionModels::psiCombustionModel::New(Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcombustionModels.so"
#13  
 in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/reactingFoam"
#14  __libc_start_main in "/lib64/libc.so.6"
#15  
 in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/reactingFoam"
Aborted (core dumped)

thermophysicalProperties:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType
{
    type            hePsiThermo;
    mixture         multiComponentMixture;
    transport       sutherland;
    thermo          janaf;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

species
{
    GAS;
    AIR;
}

inertSpecies    AIR;

GAS
{
    specie
    {
        nMoles       1;
        molWeight    27.7133;
    }
    thermodynamics
    {
        Tlow         200;
        Thigh        5000;
        Tcommon      300;
        highCpCoeffs (6 0 0 0 0 0 0);
        lowCpCoeffs  (6 0 0 0 0 0 0);
    }
    transport
    {
        As           1.5e-6;
        Ts           120;
    }
}

AIR
{
    specie
    {
        nMoles      1;
        molWeight   28.9;
    }
    thermodynamics
    {
        Tlow         200;
        Thigh        5000;
        Tcommon      300;
        highCpCoeffs (3.49344 0 0 0 0 0 0);
        lowCpCoeffs  (3.49344 0 0 0 0 0 0);
    }
    transport
    {
        As          1.4792e-06;
        Ts          116;
    }
}


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

chemistryProperties:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      chemistryProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

/*chemistryType
{
    chemistrySolver   EulerImplicit;
    chemistryThermo   psi;
}*/

chemistry           off;

/*initialChemicalTimeStep 1e-07;

EulerImplicitCoeffs
{
    cTauChem        1;
    equilibriumRateLimiter off;
}

odeCoeffs
{
    solver          Rosenbrock43;
    absTol          1e-12;
    relTol          0.01;
}*/

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

combustionProperties:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      combustionProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

combustionModel  noCombustion<psiThermoCombustion>;

active  false;

noCombustionCoeffs
{
}


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

[Linse]

For the moment I cannot see any error concerning the reaction-switchoff. I would have chosen the same settings.

It seems the error is within your thermophysicalProperties-file, as the error message says. The only thing I see: Does it really have to be "inertSpecies"? In my files it is without the final "s", but then it is rhoReactingBuoyantFoam, which MIGHT be slightly different in the settings...

[shenzhou1987]

Originally Posted by Linse

For the moment I cannot see any error concerning the reaction-switchoff. I would have chosen the same settings.

It seems the error is within your thermophysicalProperties-file, as the error message says. The only thing I see: Does it really have to be "inertSpecies"? In my files it is without the final "s", but then it is rhoReactingBuoyantFoam, which MIGHT be slightly different in the settings...

Hi Linse, Thank you for your carefulness. I have corrected it. But sadly it still doesn't work. I'm thinking change multiComponentMixture to reactingMixture. I will try it later, and if there are some changes, I will post it.

[shenzhou1987]

I change multiComponentMixture to reactingMixture, modify file 'thermophysicalProperties' according to tutorial case 'counterFlowFlame2D', and add file 'reactions' and 'thermo.compressilbeGas'. Now the good news is it works and gives me some results, the bad news is after 5~10 time steps it falls to divergence. The error message "Floating point exception" is reported. A good gain takes long pain, right? Maybe the inital total pressure of the inlet boundary is too high(18Mpa). So I will set a lower value and use rhoReactingFoam, and try again~ Hope it works. If I success, I will upload my case in this thread.

[comingdaytime]

Originally Posted by shenzhou1987

I change multiComponentMixture to reactingMixture, modify file 'thermophysicalProperties' according to tutorial case 'counterFlowFlame2D', and add file 'reactions' and 'thermo.compressilbeGas'. Now the good news is it works and gives me some results, the bad news is after 5~10 time steps it falls to divergence. The error message "Floating point exception" is reported. A good gain takes long pain, right? Maybe the inital total pressure of the inlet boundary is too high(18Mpa). So I will set a lower value and use rhoReactingFoam, and try again~ Hope it works. If I success, I will upload my case in this thread.

Hey,
I have the similar problem with you. I don't need reactions in reactingFoam, just consider the density difference into consideration. I have propane and air. And I switched off the chemistry and combustion, turbulentreaction at the same time. But my simulation crashed after 400 time steps. The courant number increases to quite a high value. When I switch on the turbulentreaction, it is the same situation. Did you figure out what exactly happened with your case? Maybe it will also help with my case.

Best Regards

Litchy

[wayne14]

Hi,

Did you try a smaller time step like 1e-3 or 1e-4? With a small time step, I have succeeded in simulating a multi-species problem without reactions using reactingFoam.

Regards,
Yan

Originally Posted by comingdaytime

Hey,
I have the similar problem with you. I don't need reactions in reactingFoam, just consider the density difference into consideration. I have propane and air. And I switched off the chemistry and combustion, turbulentreaction at the same time. But my simulation crashed after 400 time steps. The courant number increases to quite a high value. When I switch on the turbulentreaction, it is the same situation. Did you figure out what exactly happened with your case? Maybe it will also help with my case.

Best Regards

Litchy

[liping_he]

[QUOTE=wayne14;577977]

Hi, Yan


I have the same problem. I hope you can help me. MY QQ number 274795506. THX very much if any help from you..

Regards,

liping_he

[adrieno]

Hi everyone,

I'm also trying to use reactingFoam without reaction.
I try to adapt my case from the counterFlowFlame2D example.

The thing is, I'm questioning on several points:

FIRST :
In the thermophysicalProperties the keyword used for mixture is reactingmixture. Do I have to change it ?

SECOND :
The turbulenceporperties file is set with the keyword laminar. I would like to simulate turbulence, can I change it to the kEpsilon ? (or reanctingFoam isn't able to handle it ?...)

[wayne14]

Originally Posted by adrieno

Hi everyone,

I'm also trying to use reactingFoam without reaction.
I try to adapt my case from the counterFlowFlame2D example.

The thing is, I'm questioning on several points:

FIRST :
In the thermophysicalProperties the keyword used for mixture is reactingmixture. Do I have to change it ?

SECOND :
The turbulenceporperties file is set with the keyword laminar. I would like to simulate turbulence, can I change it to the kEpsilon ? (or reanctingFoam isn't able to handle it ?...)

Hi,

From my experience, reactingmixture is ok.

The inheritance process is:
reactingMixture <- multiComponentMixture <- basicSpecieMixture <- basicMultiComponentMixture

reactingMixture should be able to do the things multiComponentMixture do.


If you want turbulence, use the following:
simulationType RAS;

RAS
{
RASModel kEpsilon;

turbulence on;
printCoeffs on;
}

Correct me if anything wrong.

Regards,
Yan

[adrieno]

Thanks for your answer wayne14.
I'll try to run reactingFoam with reactingMixture.

As everyone who's using reactingFoam without combustion I guess, I want to see the flow of some different gases. One of my gas is the air.

Here is other questions.

FIRST:
Are they other solutions to define air that the one consisting in defining the rate of N2 and O2 ?
I mean, is it possible to define instead a gaz "air" ? (and how if it's possible...)
// EDIT : ... I know that it should be possible with multicomponent as shenzhou1987 tried to do (on the beginning of this topic) but I don't know if it was a success or not finally... (That's why I was wondering about using multicomponentMixture instead of reactingMixture)

SECOND:
What are the files Ydefault and alphat corresponding to in the 0 folder ? I can't explain myself what is the physical correspondence...

[adrieno]

Hi all,

I've been able to run reactingFoam turning off combustion (and with kEpsilon model turbulence).

I join my files in case of it can help someone but remember that I have no experience in CFD and less in OpenFoam. So maybe that it's full of mistake...

All I guarantee is that the solver is running without fatal error, so help yourself and adapt it to your case properly.

For the beginner as I am, be brave, then, if you wanna try my case you will have to run successively:

1. blockMesh
2. topoSet
3. createPatch -overwrite
4. reactingFoam

Have a nice project,
Adrien

[BakedAlmonds]

Hi Adrien,

I was doing some reading about reactingFoam without the use of combustion nor reacting and came across this useful link.
I compared the settings I did to yours. Mainly, the only difference I see is in the combustionModel where you used PaSR, I used noCombustion (not sure what are this as I am also new to OF)

What are the difference between the two? Since we are dealing with no combustion, naturely i selected that.

But i got the error as below:

Selecting chemistryReader foamChemistryReader
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-v3.0+/pla
tforms/linux64Gcc48DPInt32Opt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/lin
ux64Gcc48DPInt32Opt/lib/libOpenFOAM.so"
#2  ? in "/lib64/libc.so.6"
#3  Foam::heThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMi
xture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::pe
rfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::he(Foam::Field<double
> const&, Foam::Field<double> const&, int) const in "/opt/OpenFOAM/OpenFOAM-v3.0
+/platforms/linux64Gcc48DPInt32Opt/lib/libreactionThermophysicalModels.so"
#4  Foam::heThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::reactingMi
xture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::pe
rfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::heThermo(Foam::fvMesh
 const&, Foam::word const&) in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gc
c48DPInt32Opt/lib/libreactionThermophysicalModels.so"
#5  Foam::psiReactionThermo::addfvMeshConstructorToTable<Foam::hePsiThermo<Foam:
:psiReactionThermo, Foam::SpecieMixture<Foam::reactingMixture<Foam::sutherlandTr
ansport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >
, Foam::sensibleEnthalpy> > > > > >::New(Foam::fvMesh const&, Foam::word const&)
 in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/lib/libreacti
onThermophysicalModels.so"
#6  Foam::autoPtr<Foam::psiReactionThermo> Foam::basicThermo::New<Foam::psiReact
ionThermo>(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM/OpenFOAM-v3
.0+/platforms/linux64Gcc48DPInt32Opt/lib/libreactionThermophysicalModels.so"
#7  Foam::psiReactionThermo::New(Foam::fvMesh const&, Foam::word const&) in "/op
t/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/lib/libreactionThermo
physicalModels.so"
#8  Foam::combustionModels::psiThermoCombustion::psiThermoCombustion(Foam::word
const&, Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM/OpenFOAM-v3.0+
/platforms/linux64Gcc48DPInt32Opt/lib/libcombustionModels.so"
#9  Foam::combustionModels::psiCombustionModel::adddictionaryConstructorToTable<
Foam::combustionModels::noCombustion<Foam::combustionModels::psiThermoCombustion
> >::New(Foam::word const&, Foam::fvMesh const&, Foam::word const&) in "/opt/Ope
nFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/lib/libcombustionModels.so
"
#10  Foam::combustionModels::psiCombustionModel::New(Foam::fvMesh const&, Foam::
word const&) in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/l
ib/libcombustionModels.so"
#11  ? in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/bin/rea
ctingFoam"
#12  __libc_start_main in "/lib64/libc.so.6"
#13  ? in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/bin/rea
ctingFoam"
Floating point exception

[adrieno]

Hi BakedAlmonds,
Unfortunately I don't know the difference between PaSR and noCombustion (placeholder or not ? in the extend that we turned off combustion...). Someone who is used to look into the source code would be better for answering you. Sorry, but if you succeed in running you're case with "noCombustion" let me know.
Best regards,
Adrien

[ab2484]

Hello everyone,

I'm encountering your same difficulties in the implementation my case. Basically I need to study a jet involving air and a different gas, without any reaction or combustion involved (OF 4.x).

I'm now working on the tutorial, trying to switch of reactions and turn on the turbulence, but I'm not sure of my results.

Did you manage to develop a good solver for this kind of simulation? Any help would be really useful, since I'm not experienced in OF and completely new to multi species problems.

Thanks
Anrdea

[kcjarvis56]

Originally Posted by ab2484

Hello everyone,

I'm encountering your same difficulties in the implementation my case. Basically I need to study a jet involving air and a different gas, without any reaction or combustion involved (OF 4.x).

I'm now working on the tutorial, trying to switch of reactions and turn on the turbulence, but I'm not sure of my results.

Did you manage to develop a good solver for this kind of simulation? Any help would be really useful, since I'm not experienced in OF and completely new to multi species problems.

Thanks
Anrdea

Did you manage to get the chemistry turned off?

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      chemistryProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

chemistryType
{
    chemistrySolver   EulerImplicit;
    chemistryThermo   psi;
}

chemistry           off;

initialChemicalTimeStep 1e-07;

EulerImplicitCoeffs
{
    cTauChem        1;
    equilibriumRateLimiter off;
}

odeCoeffs
{
    solver          Rosenbrock43;
    absTol          1e-12;
    relTol          0.01;
}

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

Then combustion has to be off also:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      combustionProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

combustionModel  noCombustion<rhoThermoCombustion>;


active false;

noCombustionCoeffs
{
}


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

Make sure the reaction file has the correct species that you are using with no reactions:

species
(
    O2    
    etoh
    H2O
    N2
);

reactions
{
    
}

For reference here is the thermophysicalProperties

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

inertSpecie N2;

chemistryReader foamChemistryReader;

foamChemistryFile "$FOAM_CASE/constant/reactions";

foamChemistryThermoFile "$FOAM_CASE/constant/thermo.compressibleGas";


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

This should be able to get the model running with no combustion or chemistry.

[ab2484]

Dear Kirk,

many thanks for your reply, I used a similar set up and it run (and the solution seems realistic).

I have another question, again related to the use of reactingFoam.

I want to run a low-mach simulation and making comparison with the standard one. Do you have any suggestions?
Initially I thought that using the incompressiblePerfectGas law as State equation was fine, but apparently I cannot use it with this setup for the thermophysicalProperties file:



/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType
{
type heRhoThermo;
mixture reactingMixture;
transport const;
thermo hConst;
energy sensibleEnthalpy;
equationOfState incompressiblePerfectGas;
specie specie;
}



On top of that, I read that other mods to the solver's code must be applied.

Do you have any advices to turn reactingFoam in a Low-Mach solver instead of running it compressible?


Thanks!
Andrea

[Richardk]

Originally Posted by shenzhou1987

Hi, everyone. I'm using OpenFOAM 2.3.0 to simulate the jet flow of a nozzle which contains two species, gas and air. I just want to study the process of jet gas mixing into the air without combustion and reaction. After reading the User Guide, I think reactingFoam could be a suitalbe solver for my case. And I have read some threads in the forum which mentioned this problem, some one said combustion and reaction model can be switched off in reactingFoam. But there is no details about how to switch off combustion and reaction in reactingFoam. I open the tutorial case "counterFlowFlame2D", in folder "constant" I copy file chemistryProperties, combustionProperties and thermophysicalProperties to my case folder and modify them. Then I execute "reactingFoam" command. Some errors are reported as blow and the relation files are attached. Can anybody tell me what's wrong with my case files? Thank you!

Error:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0
Exec   : reactingFoam
Date   : Jan 13 2015
Time   : 23:20:54
Host   : "localhost.localdomain"
PID    : 32121
Case   : /home/shenzhou1987/OpenFOAM/Jet/2D-axis
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create mesh for time = 0


Reading g
Creating reaction model

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



--> FOAM FATAL IO ERROR: 
Attempt to return dictionary entry as a primitive

file: /home/shenzhou1987/OpenFOAM/Jet/2D-axis/constant/thermophysicalProperties.species

    From function ITstream& primitiveEntry::stream() const
    in file db/dictionary/dictionaryEntry/dictionaryEntry.C at line 83.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::IOerror::abort() in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::dictionaryEntry::stream() const in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#3  Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >::multiComponentMixture(Foam::dictionary const&, Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#4  Foam::SpecieMixture<Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::SpecieMixture(Foam::dictionary const&, Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#5  Foam::heThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::heThermo(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#6  Foam::hePsiThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::hePsiThermo(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#7  Foam::psiReactionThermo::addfvMeshConstructorToTable<Foam::hePsiThermo<Foam::psiReactionThermo, Foam::SpecieMixture<Foam::multiComponentMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::janafThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > > >::New(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#8  Foam::autoPtr<Foam::psiReactionThermo> Foam::basicThermo::New<Foam::psiReactionThermo>(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#9  Foam::psiReactionThermo::New(Foam::fvMesh const&, Foam::word const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libreactionThermophysicalModels.so"
#10  Foam::combustionModels::psiThermoCombustion::psiThermoCombustion(Foam::word const&, Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcombustionModels.so"
#11  Foam::combustionModels::psiCombustionModel::adddictionaryConstructorToTable<Foam::combustionModels::noCombustion<Foam::combustionModels::psiThermoCombustion> >::New(Foam::word const&, Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcombustionModels.so"
#12  Foam::combustionModels::psiCombustionModel::New(Foam::fvMesh const&) in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcombustionModels.so"
#13  
 in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/reactingFoam"
#14  __libc_start_main in "/lib64/libc.so.6"
#15  
 in "/opt/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/bin/reactingFoam"
Aborted (core dumped)

thermophysicalProperties:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType
{
    type            hePsiThermo;
    mixture         multiComponentMixture;
    transport       sutherland;
    thermo          janaf;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

species
{
    GAS;
    AIR;
}

inertSpecies    AIR;

GAS
{
    specie
    {
        nMoles       1;
        molWeight    27.7133;
    }
    thermodynamics
    {
        Tlow         200;
        Thigh        5000;
        Tcommon      300;
        highCpCoeffs (6 0 0 0 0 0 0);
        lowCpCoeffs  (6 0 0 0 0 0 0);
    }
    transport
    {
        As           1.5e-6;
        Ts           120;
    }
}

AIR
{
    specie
    {
        nMoles      1;
        molWeight   28.9;
    }
    thermodynamics
    {
        Tlow         200;
        Thigh        5000;
        Tcommon      300;
        highCpCoeffs (3.49344 0 0 0 0 0 0);
        lowCpCoeffs  (3.49344 0 0 0 0 0 0);
    }
    transport
    {
        As          1.4792e-06;
        Ts          116;
    }
}


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

chemistryProperties:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      chemistryProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

/*chemistryType
{
    chemistrySolver   EulerImplicit;
    chemistryThermo   psi;
}*/

chemistry           off;

/*initialChemicalTimeStep 1e-07;

EulerImplicitCoeffs
{
    cTauChem        1;
    equilibriumRateLimiter off;
}

odeCoeffs
{
    solver          Rosenbrock43;
    absTol          1e-12;
    relTol          0.01;
}*/

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

combustionProperties:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      combustionProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

combustionModel  noCombustion<psiThermoCombustion>;

active  false;

noCombustionCoeffs
{
}


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

Hi

for switching the chemistry off, additional to sellecting off for chemistry, you need to change the reaction mechanism. E.g. You should put zero for activation energy and B, also you should not consider chemical reactions in the mechanism which means that the reactants and products should be the same.


Regards,
Richard