[Archana V]

Hi,

I am trying to add pyrolysis model in chtMultiRegionFoam (version-6). I am able to compile the new solver. But when I run my case, following error has been obtained.


archanav@pc421-195:~/OpenFOAM/archanav-6/run/surfaceReaction1$ myChtMultiRegionFoam
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 6
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
Build : 6
Exec : myChtMultiRegionFoam
Date : May 07 2019
Time : 11:01:23
Host : "pc421-195"
PID : 8019
I/O : uncollated
Case : /home/archanav/OpenFOAM/archanav-6/run/surfaceReaction1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

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

Create fluid mesh for region region2 for time = 0

Create solid mesh for region region1 for time = 0

Create solid mesh for region region3 for time = 0

*** Reading fluid mesh thermophysical properties for region region2

Adding to thermoFluid

Selecting thermodynamics package
{
type hePsiThermo;
mixture reactingMixture;
transport sutherland;
thermo janaf;
equationOfState perfectGas;
specie specie;
energy sensibleEnthalpy;
}

Selecting chemistryReader foamChemistryReader
elements not defined in "/home/archanav/OpenFOAM/archanav-6/run/surfaceReaction1/constant/region2/reactions"
Adding to rhoFluid

Adding to UFluid

Adding to phiFluid

Adding to gFluid

Adding to hRefFluid

Adding to ghFluid

Adding to ghfFluid

Adding to turbulenceFluid

Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon
RAS
{
RASModel kEpsilon;
turbulence on;
printCoeffs on;
Cmu 0.09;
C1 1.44;
C2 1.92;
C3 0;
sigmak 1;
sigmaEps 1.3;
}

Adding to reactionFluid

Selecting combustion model PaSR
Selecting chemistry solver
{
solver EulerImplicit;
method standard;
}

StandardChemistryModel: Number of species = 3 and reactions = 0
using integrated reaction rate
Adding to radiationFluid

Selecting radiationModel none
Adding to KFluid

Adding to dpdtFluid

Adding to fieldsFluid

Adding to QdotFluid

Adding MRF

No MRF models present

Adding fvOptions

*** Reading solid mesh thermophysical properties for region region1

Adding to thermos

Selecting thermodynamics package
{
type heSolidThermo;
mixture reactingMixture;
transport constIso;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}

Selecting chemistryReader foamChemistryReader
elements not defined in "/home/archanav/OpenFOAM/archanav-6/run/surfaceReaction1/constant/region1/reactions"
Adding to radiations

Selecting radiationModel opaqueSolid
Selecting absorptionEmissionModel constantAbsorptionEmission
Selecting scatterModel none
Selecting sootModel none
Adding fvOptions

Creating finite volume options from "system/fvOptions"

Selecting finite volume options model type scalarSemiImplicitSource
Source: HeatSource
- selecting all cells
- selected 3595 cell(s) with volume 0.00068306205
Adding Pyrolysis model

*** Reading solid mesh thermophysical properties for region region3

Adding to thermos

Selecting thermodynamics package
{
type heSolidThermo;
mixture reactingMixture;
transport constIso;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}

Selecting chemistryReader foamChemistryReader
elements not defined in "/home/archanav/OpenFOAM/archanav-6/run/surfaceReaction1/constant/region1/reactions"
Adding to radiations

Selecting radiationModel opaqueSolid
Selecting absorptionEmissionModel constantAbsorptionEmission
Selecting scatterModel none
Selecting sootModel none
Adding fvOptions

Adding Pyrolysis model

Selecting pyrolysisModel reactingOneDim
Selecting region model functions
none


--> FOAM FATAL ERROR:
index -1 out of range 0 ... 8216

From function void Foam::UList<T>::checkIndex(Foam::label) const [with T = int; Foam::label = int]
in file /home/archanav/Documents/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/UListI.H at line 106.

FOAM aborting

#0 Foam:: error:: printStack(Foam:: Ostream&) at ~/Documents/OpenFOAM/OpenFOAM-6/src/OSspecific/POSIX/printStack.C:218
#1 Foam:: error:: abort() at ~/Documents/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/error.C:249
#2 Foam:: Ostream& Foam:: operator<< <Foam:: error>(Foam:: Ostream&, Foam:: errorManip<Foam:: error>) at ~/Documents/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/errorManip.H:85 (discriminator 4)
#3 Foam:: UList<int>:: checkIndex(int) const at ~/Documents/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/UListI.H:106
#4 Foam:: UList<int>:: operator[](int) const at ~/Documents/OpenFOAM/OpenFOAM-6/src/OpenFOAM/lnInclude/UListI.H:201
#5 Foam:: regionModels:: regionModel1D:: initialise() at ~/Documents/OpenFOAM/OpenFOAM-6/src/regionModels/regionModel/regionModel1D/regionModel1D.C:90 (discriminator 2)
#6 Foam:: regionModels:: regionModel1D:: regionModel1D(Foam:: fvMesh const&, Foam:: word const&, Foam:: word const&, Foam:: dictionary const&, bool) at ~/Documents/OpenFOAM/OpenFOAM-6/src/regionModels/regionModel/regionModel1D/regionModel1D.C:350
#7 Foam:: regionModels:: pyrolysisModels:: pyrolysisModel:: pyrolysisModel(Foam:: word const&, Foam:: fvMesh const&, Foam:: dictionary const&, Foam:: word const&) at ~/Documents/OpenFOAM/OpenFOAM-6/src/regionModels/pyrolysisModels/pyrolysisModel/pyrolysisModel.C:109
#8 Foam:: regionModels:: pyrolysisModels:: reactingOneDim:: reactingOneDim(Foam:: word const&, Foam:: fvMesh const&, Foam:: dictionary const&, Foam:: word const&) at ~/Documents/OpenFOAM/OpenFOAM-6/src/regionModels/pyrolysisModels/reactingOneDim/reactingOneDim.C:569
#9 Foam:: regionModels:: pyrolysisModels:: pyrolysisModel:: adddictionaryConstructorToTable<Foam:: regionModels:: pyrolysisModels:: reactingOneDim>:: New(Foam:: word const&, Foam:: fvMesh const&, Foam:: dictionary const&, Foam:: word const&) at ~/Documents/OpenFOAM/OpenFOAM-6/src/regionModels/pyrolysisModels/lnInclude/pyrolysisModel.H:114 (discriminator 2)
#10 Foam:: regionModels:: pyrolysisModels:: pyrolysisModel:: New(Foam:: fvMesh const&, Foam:: dictionary const&, Foam:: word const&) at ~/Documents/OpenFOAM/OpenFOAM-6/src/regionModels/pyrolysisModels/pyrolysisModel/pyrolysisModelNew.C:115
#11 Foam:: regionModels:: pyrolysisModels:: pyrolysisModelCollection:: pyrolysisModelCollection(Foam:: fvMesh const&) at ~/Documents/OpenFOAM/OpenFOAM-6/src/regionModels/pyrolysisModels/pyrolysisModel/pyrolysisModelCollection.C:85
#12 ? at ~/OpenFOAM/archanav-6/applications/solvers/heatTransfer/myChtMultiRegionFoam/createFields.H:14
#13 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#14 ? at ??:?
Aborted (core dumped)


I am simulating an annulus flow in which region 1 is a horizontal solid rod (solid reaction happens here with the fluid), region 2 is the fluid flowing in the annulus and region 3 is the outside pipe.

These modifications are done in the code

/*------------- createSolidFields.H-------------------*\

PtrList<regionModels:: pyrolysisModels:: pyrolysisModel>tpyrolysis(solidRegions.size());

forAll(solidRegions, i)
{

Info<< " Adding Pyrolysis model\n" << endl;


tpyrolysis.set
(
i,
regionModels:: pyrolysisModels:: pyrolysisModel:: New(solidRegions[i])
);

IOdictionary additionalControlsDict
(
IOobject
(
"additionalControls",
runTime.constant(),
solidRegions[i],
IOobject:: MUST_READ_IF_MODIFIED,
IOobject:: NO_WRITE
)
);
volScalarField Qdot
(
IOobject
(
"Qdot",
runTime.constant(),
solidRegions[i],
IOobject:: READ_IF_MODIFIED,
IOobject:: AUTO_WRITE
)
solidRegions[i],
dimensionedScalar("Qdot", dimEnergy/dimVolume/dimTime,0.0)
);

Switch solvePyrolysisRegion
(
additionalControlsDict.lookupOrDefault<bool>("solv ePyrolysisRegion",true)
);
}
/*----------------------------------------------------------------------*\

/*------------- setSolidFields.H-------------------*\


regionModels:: pyrolysisModels:: pyrolysisModelCollection& pyrolysis = tpyrolysis[i];

/*----------------------------------------------------------------------*\

in main code pyrolysis.evolve(); is added


I don't know how to tackle this problem as I am new to OpenFOAM and C++language. I would be grateful, If anyone could help me to solve this problem. Looking forward for reply.

Regards

Archana

[Archana V]

I solved above problem.

[Paulo SPS]

Hi there,
I am new to openfoam and I'm trying to do something similar.
Did you manage to read the reactions into the solid region from the "reactions" dictionary or you went another route?
I managed to read a composition into the solid region using "solidReactionThermo.H" but I can't for the life of me figure out how to read the reactions, not to mention the actual reaction rates to put into an Y equation for the solid region.


Cheers

[Kummi]

Hello Paulo,
Hereby some hints for you to follow on.
Take a look at this blog:
http://sourceflux.de/blog/howto-writ...n-in-openfoam/

Here you can find - significant note in comment section:

Once you have figured out the dendency structure of both solvers, you should make sure that the solution algorithms used for the model implemented by both solvers fit together. For example, if fireFoam is based on a PISO/PIMPLE loop and executes bunch of models in the in-between steps of such a segregated algorithm, it would not be straightforward to couple the functionality of fireFoam with another solver that relies on fully implicit equation coupling with block matrices.
At this point you should chose the source and the target for the new combined solver. Obviously, if fireFoam is more complicated in the sense of library dependencies as well as the overall solution algorithm, then you should port the chtMultiRegionFoam into fireFoam.

Later, you can manage your pyrolysis solver in different blocks using "compressible::turbulentTemperatureCoupledBaffleMi xed" condition

[Zhiheng Wang]

Hi how did you add pyrolysis to chtMultiRegion Foam and how did the problem was solved can you reply ??
By the way why did not you Used fireFoam ???

[Zhiheng Wang]

How did you solved and what part you have modified ???

[atulkjoy]

Where was the problem ??? I have tried the same thing, This sort of problem can also be tried using fireFOAM and reactingParcelFilmFoam. Did you tried so

[Kummi]

In my case, I developed a solver for pyrolysis based on fireFOAM. For simulating two regions, I implemented "compressible::turbulentTemperatureCoupledBaffleMix ed" condition as stated below:

boundaryField
{
hotSide
{
type fixedValue;
value uniform 1323;
}

right
{
type symmetryPlane;
value uniform 0;
}

sides
{
type empty;
}

furnace_to_oven
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
value uniform 293;
neighbourFieldName T;
K solidThermo;
KName none;
}
}

Keep both pyrolysis zones active.

pyrolysis
{
active true;
pyrolysisModel reactingOneDim;
regionName furnace;
reactingOneDimCoeffs
{
filmCoupled false;
radFluxName Qr;
minimumDelta 1e-8;
reactionDeltaMin 1e-8;
moveMesh false;
}
infoOutput true;
}

However, switch off the chemistry for regions where pyrolysis is not necessary.

solidChemistryModel ODECoalHeterogeneousChemistryModel<constSolidTherm oPhysics>;
gasThermoModel gasThermoPhysics;
chemistry off; //on - region2
chemistrySolver ode;
initialChemicalTimeStep 1e-07;
odeCoeffs
{
solver SIBS;
eps 0.05;
}

In addition, use topoSet command to explicitly create two zones followed by splitMeshRegions.
If above steps are followed, one can implement the multiple regions (chtMultiRegionFoam) in pyrolysis solver.

Hope it helps. Thank you ^^

[Saeng Kinley]

There will be a difference in solution if you create Two Regions by splitMesh and if Your create Region by extrudetoRegionMesh.

[Kummi]

In my case, there are 2 regions "furnace" and "oven".
"Furnace" treated with heat equation only. And the "oven" involves pyrolysis. The resultant heat outflow from the furnace is introduced inside "oven" using coupled boundary condition. And for this reason to split 2 zones, I implemented "splitMeshRegions" command. Is there any other command to be used promptly?

There will be a difference in solution if you create Two Regions by splitMesh and if Your create Region by extrudetoRegionMesh.

Could you please explain me the difference in solution using both commands?

Thank you

[ArminAlavi]

hello Archana
I am struggling with a problem same to yours. I want to implement the fireFoam pyrolysis model in chtMultiRegionFoam. May I ask how did you manage to do so?
Thank you in advance
Armin

[Kummi]

Hello Armin,
Kindly choose the source and the target for the new combined solver. FireFoam is more complicated in the sense of library dependencies as well as the overall solution algorithm, then you should port the chtMultiRegionFoam into fireFoam.

Above comments may clearly give you some idea. Did you got It?
Thank you ^^

[ArminAlavi]

hello Kummi
First of all thank you for your reply. Yes I get the general idea, but I have one more question if you will. you are right about library dependencies and complexity of the fireFoam solver. the below code is a part of fireFoam.C that solves the solid fuel part:

if(solvePyrolysisRegion)
{
pyrolysis.evolve();
}

Am I right? the rest is similar to what chtMultiRegionFoam solves for fluid part. In your opinion is it right to just add the pyrolysis region solver(libraries and needed classes included) to the chtMultiRegion Solver?

[ArminAlavi]

I am sorry to trouble you, but I have one more question. The pyrolysis model which OpenFOAM provides only interacts with surface films, If I am right, that is why you have to define your solid region by extrudeMesh. I want to have a volume of solid. Is there a way to make this model work on 3d arbitrary mesh?
Thank you
Armin

[Kummi]

Hello Armin,

Yes you are right. FireFOAM solver rely on pyrolysis based on the keyword pyrolysis.evolve(). It was resolved based on regionModel (based on coupled Boundary condition - using extrudetoRegionMesh) under the source file reactingOneDim. Its dependent libraries for thermo, transport and other properties are declared in thermophysicalproperties under the file names like solidChemistryModel, basicSolidThermo and so on [kindly follow the keyword "solid" and header files accordingly to understand]

Am I right? the rest is similar to what chtMultiRegionFoam solves for fluid part. In your opinion is it right to just add the pyrolysis region solver(libraries and needed classes included) to the chtMultiRegion Solver?

Yes, you are right. In chtMultiRegionFoam solver, if I'm not wrong, solid model is resolved only with diffusion equation fvm::laplacian(kappa, T). Inclusion of source term like solid (wood, coal) heat absorption (endothermic) and exothermic heat release was found in pyrolysis solver under FireFOAM. If you look deep into the code, pyrolysis is solved based on regionModelling, whereas chtMultiRegionFoam was constructed based on fully implicit equation coupling with block matrices [solid, fluid]. So my request is, before trying to merge both solvers, be clear with the algorithms and physics of both solvers. You also need to be quite confident with OpenFOAM technics. Nothing is impossible. I haven't done it either, since its not part of my plan now. In my other work, I have partially achieved by coupling boundary condition as explained above.

The pyrolysis model which OpenFOAM provides only interacts with surface films, If I am right, that is why you have to define your solid region by extrudeMesh.

Big NO. Not only interacts with surface film. You can disable/remove the surface film option as per your need. If you implement the extrudeMesh command, the solver doesn't consider the extruded part as separate body/domain because, its just extruded [like Pad option in CATIA]. To be more clear, when you do extrudeMesh command, you cant define the boundary condition for the extruded domain. Instead, if you try the command splitMeshRegions -cellZones -overwrite, you will get 2/more zones, where you can apply conditions as per your need.

I want to have a volume of solid. Is there a way to make this model work on 3d arbitrary mesh?

Try with splitMeshRegions command if you have more than 1region, you will find a way.

fvScalarMatrix TEqn
(
fvm::ddt(rhoCp, T_)
- fvm::laplacian(K_, T_)
==
chemistrySh_ //RRs*hf (hf - heat of formation) // explicit - Endothermic reaction
);

Here is the pyrolysis governing equation mentioned above. It serves perfectly for 3d arbitrary mesh.

In OpenFOAM as per my knowledge, pyrolysis model is depicted with the tag "1D", due to the energy transfer from pyrolysis to combustion model normal through the surface (in one direction, so called 1D). So, the tag "1D" doesn't mean that the pyrolysis can be solved only with 1D.

Feel free to ask any query.

Thank you

[ArminAlavi]

Hello Kummi,
Thank you very much for your precise advice. I will look into it. Although another thing started to interest me. Do you suggest that , if I use the fireFoam solver without any changes in the code with splitMeshRegions utility it would work just fine with suitable boundary conditions implemented. If that statement is right then I have no need to merge two solvers.

Thank you very much
Armin

[Kummi]

Hello Armin,
You are welcome.

Do you suggest that , if I use the fireFoam solver without any changes in the code with splitMeshRegions utility it would work just fine with suitable boundary conditions implemented.

It depends on your work. In my work, 2 regions are solid, in one region I need to solve only diffusion equ, whereas the other region solves pyrolysis. By switching the chemistry properties ON/OFF, I control my code.

But if its fluid/solid blocks, then no other go, you need to merge. May I know, WHat kind of problem you are gonna approach ?
Thank you

[ArminAlavi]

Hello Kummi,
To be more specific, my simulation consists of two regions, a solid polymer and a fluid flow. The fluid is a hot molten metal that interacts with the polymer causing it to pyrolise. In this interaction, polymer degrades into residual gases, the residual gases are diffused into the fluid region, meanwhile the molten metal eats it's way through the polymer by pyrolysing it. From what you said about fluid/solid interaction, I think the solution is to merge the two solvers, Am I right?

Thank you
Armin

[Kummi]

Hello Armin,
The energy in the form of heat is supplied by hot molten metal in fluid state. This source of energy from fluid causes the solid polymer to pyrolise. Its perfect fluid/solid interaction as you say.

So, its not about 2 regions (like chtmultiregionFOAM).. Its all about multiphase problem with fluid/solid interaction. Did I got it right ?

[ArminAlavi]

Hello again
Yes you got it right about the multiphase problem + fluid/solid interaction but yet I don't understand how isn't it a 2 region problem. Is it because fields inside the solid part do not need to be solved? and the fluid/solid surface interactions are only important?