[jose_rodrig]

Originally Posted by jose_rodrig

Hi Again everyone!
I managed to compile Novaresio's library and the modifiedReactingFoam solver.
Now I want to set up a new simulation with Smooke's chemistry scheme but the library needs addtional info in the transportDictionary, namely the collision diameter and the characteristic Lennard-Jones energy of each involving species, to compute the binary diffusion coefficient.

I found in Novaresio's paper the some of these data is tabulated in "Hirshfelder et al., Molecular Theory of Gases and Liquids". However, neither the values he has in example case (supplied with the library) correspond to the ones in the former reference (despeite units), nor I am able to find data for all the species, namely, OH, H2O2, H, O, HCO, etc.

Does anybody have any idea where can I find this data?
Novaresio, could you enlighten me on this? Where did you get your data?

Regards everyone!

Hi!
I found a data file with all this info. For those interested, you can find it here:

http://diesel.me.berkeley.edu/~gri_m...12/text12.html

It has all the data necessary for methane combustion, using the grimech chemical mechanism. It is used for the sandia flame code.

Cheers
Jose

[jose_rodrig]

Originally Posted by jose_rodrig

Hi Again

I am getting a strange error with modifiedReactingFoam solver:

If I try to use a Chemkin file as input for chemical scheme I get this error:



I wonder what this is...
You can replicate this (i guess) by simply replacing the chemkin file (chem.inp) used in the dieselFoam tutorial distributed with OF by the chemistry used in the modifiedReactingFoam test case. Everything else is untouched.

Cheers

Ok.. I was able to track down this bug and came up with a simple fix.

So, I found out the code was crashing as it ran lines 65 and 66 in file Wilke.C:

const scalar& W1 = molecularWeights[name1];
const scalar& W2 = molecularWeights[name2];

I guess the problem is with function "molecularWeights" and so I replaced those lines with the following to avoid the fatal error I was getting so far.

const scalar& W1 = readScalar(dic.subDict("molarWeight").lookup(name1 ));

const scalar& W2 = readScalar(dic.subDict("molarWeight").lookup(name2));

This will look for the molecular weights of each species in a subdictionary in the constant/transportProperties file.

molarWeight
{
	C7H16	100;
	O2		36;
	CO2		48;
	H2O		18;
	N2		38;
}

This worked for me. If you're using other Binary diffusivity model than Wilke, you should do the same procedure in the respective .C file (i. e. ChapmanEnskog.C or Fuller.C).

I haven't look inside the molecularWeights.C file, where I think the prob is, to find out what is wrong with it and fix it. However, I will had this task to my todo list and, whenever I´ll have the time, I will try to have a look on it.

Hope I could help.

Cheers

Jose

[mturcios777]

It seems a shame to have to specify the molecular weights in a dictionary when we should already have the data available through the thermo model. Can we (in general) call

 thermo.composition.W(specI)

, where specI is the label of the specie in questions (we'll have to do a search for it every time). I've tried to compile this but I'm told that composition (which is a basic) has no member W, when it does:

http://foam.sourceforge.net/docs/cpp...87805d01d0cc28

I'm sure I'm missing something about pointers and casting, but I'm not seeing it. Anyone have ideas?

[wyldckat]

Greetings to all!

Originally Posted by mturcios777

It seems a shame to have to specify the molecular weights in a dictionary when we should already have the data available through the thermo model. Can we (in general) call

 thermo.composition.W(specI)

, where specI is the label of the specie in questions (we'll have to do a search for it every time). I've tried to compile this but I'm told that composition (which is a basic) has no member W, when it does:

http://foam.sourceforge.net/docs/cpp...87805d01d0cc28

I'm sure I'm missing something about pointers and casting, but I'm not seeing it. Anyone have ideas?

From the link, it says it's a pure virtual method. This means that if the method is not reimplemented, then it's as good as non-existent!

Now, I haven't checked/looked at the code, but I'm assuming you can't simply use the basic thermo dictionary and will have to use the complex one, namely one of those long ones with the various characteristics for the fluid/gas...

Best regards,
Bruno

[mturcios777]

Ah, so I need to go deeper in the templatization. Following the inheritance diagram, multiComponentMixture<thermoType> implements the W() function. In createFields for the modified reactingFoam, which I think would be the general purpose type. The modifiedReactingFoam test case uses the thermo model.

hsPsiMixtureThermo<reactingMixture<gasThermoPhysics>>

Is there any way to explicitly to call the version of the function we want, maybe calling it straight from the psiChemistry object?

[wyldckat]

Perhaps something similar to:

hsPsiMixtureThermo<reactingMixture<gasThermoPhysics>>().composition.W(specI)

Not very pretty, but it's the most direct thing I can think of, although this might not work exactly this way...

Additionally, the instantiated class might not like the dictionary file if said dictionary is using any other terms from the ones above

[mturcios777]

Bummer. So there isn't a way to call the implemented version of a pure virtual function of a template class without knowing what the implementation will be?

[wyldckat]

Originally Posted by mturcios777

Bummer. So there isn't a way to call the implemented version of a pure virtual function of a template class without knowing what the implementation will be?

It shouldn't be necessary to bother with the details in the solver itself. Other solvers should show that it's as simple as using the correct thermo dictionary options for what you need to solve. What might happen is that some thermo options disregard completely molecular weight and such

[wyldckat]

For example, buoyantSimpleFoam:

Info<< "Reading thermophysical properties\n" << endl;

    autoPtr<basicPsiThermo> pThermo
    (
        basicPsiThermo::New(mesh)
    );
    basicPsiThermo& thermo = pThermo();

//.....

    volScalarField& p = thermo.p();
    volScalarField& h = thermo.h();
    const volScalarField& psi = thermo.psi();

Seems simple enough here....

Tutorial "heatTransfer/buoyantSimpleFoam/hotRoom":

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType      hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>;

pRef            100000;

mixture
{
    specie
    {
        nMoles          1;
        molWeight       28.9;
    }
    thermodynamics
    {
        Cp              1000;
        Hf              0;
    }
    transport
    {
        mu              1.8e-05;
        Pr              0.7;
    }
}

Weight should be easily accessible in this case. But it needs one big template hierarchy in there for it to work out of the box.

[mturcios777]

Thank you for the explanation. It just seems a bit off to me that a class named basicMultiComponentMixture would have an access function for the molecular weight and not be able to use it.

Doing a quick comparison between versions (as I'm switching between 1.6-ext and 2.1.x until the polyTopoChange/polyTopoChanger mechanisms are fixed), it seems that the function is available in 2.1.x (to accomodate the SLGThermo class I'll bet) but not in 1.6.ext.

So if you are using this with 2.1.x, you can get the molecular weights using

 composition.W(specI)

. I've compiled the code and it seems to work as desired. as previously mentioned. In 1.6-ext it appears we are stuck with the dictionary.

[mhsn]

Originally Posted by mturcios777

I've been monitoring this thread and am quite interested in experimenting with it. Jose, other than Niklas' comment about the inert species, were there any other fixes required to get it running in 2.1.x? From your earlier comments it appears you were gunning for that.

Thanks!

Originally Posted by novyno

Dear Anton,

I will follow your suggestion soon.

Many thanks

Valerio

Originally Posted by mturcios777

I've done work with both versions and have some experience adapting between the two, so maybe I'll also tackle it if I find the time (been working on polyTopoChangers in 21x and that's been taking a LOT of time).

Cheers

Hi, I'm interested in using this model for OpenFoam2.1.1. Did you guys happen to make it compatible with this version?
I tried to compile it using OF2.1.1 but got this error:
diffusivityModel/diffusivityModel.C:104:69: error: ‘const class Foam:orousZone’ has no member named ‘zoneId’
It might be because the zoneId is named something else in Of2.1.1! Does anybody have any clue?

Thanks

[mhsn]

After looking at the file porousZone.H, I guess I should change "zoneId" to "zoneIds" which I did and now I get the below error:

diffusivityModel/diffusivityModel.C:104:76: error: no match for ‘operator[]’ in ‘(&(& T)->Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::<anonymous>.Foam:imensionedField <Type, GeoMesh>::mesh [with Type = double, GeoMesh = Foam::volMesh, typename GeoMesh::Mesh = Foam::fvMesh]())->Foam::fvMesh::<anonymous>.Foam:olyMesh::cellZon es()[(& pZones)->Foam::PorousZones<Foam:orousZone>::<anonymous>. Foam::IOPtrList<Foam:orousZone>::<anonymous>.Foa m::PtrList<T>:perator[] [with T = Foam:orousZone, Foam::label = int](zoneI).Foam:orousZone::zoneIds]’


The error refers to the part of the code which looks like this:

forAll(pZones, zoneI)
{
const scalar& porosity = pZones[zoneI].porosity();
const labelList& cells = T.mesh().cellZones()[pZones[zoneI].zoneIds()];
forAll(cells, cellI)
{
eps_[cells[cellI]] = porosity;
}
}

Can anybody help how I can resolve this error?
Thanks

[tetraeder]

Hi mhsn,

you have do add a loop over all porosity Zones.

forAll(pZones, zoneI)
{
const labelList& cellZoneIds = pZones[zoneI].zoneIds();
const scalar& porosity = pZones[zoneI].porosity();
forAll(cellZoneIds, zoneJ)
{
const labelList& cells = T.mesh().cellZones()[cellZoneIds[zoneJ]];
forAll(cells, cellI)
{
eps_[cells[cellI]] = porosity;
}
}
}

BR

[mhsn]

Originally Posted by tetraeder

Hi mhsn,

you have do add a loop over all porosity Zones.

forAll(pZones, zoneI)
{
const labelList& cellZoneIds = pZones[zoneI].zoneIds();
const scalar& porosity = pZones[zoneI].porosity();
forAll(cellZoneIds, zoneJ)
{
const labelList& cells = T.mesh().cellZones()[cellZoneIds[zoneJ]];
forAll(cells, cellI)
{
eps_[cells[cellI]] = porosity;
}
}
}

BR

Thanks, it compiled Now I should check what error I will see when compiling the other library "multiSpeciesTransportModels".

[mhsn]

Well, now I'm trying to compile "multiSpeciesTransportModels" and after resolving some errors regarding universal gas constant "R", I see some errors when it tries to read submodels.
Here is what I get:
lnInclude/Fick.C:149:19: error: ‘const class Foam::fvMesh’ has no member named ‘relax’
lnInclude/Fick.C:167:19: error: ‘const class Foam::fvMesh’ has no member named ‘relax’
lnInclude/Fick.C:169:28: error: ‘const class Foam::fvMesh’ has no member named ‘relaxationFactor’

and here is what the code looks like at those lines:

iline149:
f (mesh_.relax("Yi"))
{
yi.storePrevIter();
}


line167:
if (mesh_.relax("Yi"))
{
yi.relax(mesh_.relaxationFactor("Yi"));
}


I guess from of1.6 to of2.1.1 that relax may be defined differently! IS that right? anyone knows how this can be resolved?
Tetraeder, can you help?

[tetraeder]

Hi mhsn,

with


if (mesh_.relaxField("Yi"))
{
yi.storePrevIter();
}

.....

if (mesh_.relaxField("Yi"))
{
yi.relax(mesh_.fieldRelaxationFactor("Yi"));
}

it should compile in OF 2.1.x

BR

[mhsn]

Originally Posted by tetraeder

Hi mhsn,

with


if (mesh_.relaxField("Yi"))
{
yi.storePrevIter();
}

.....

if (mesh_.relaxField("Yi"))
{
yi.relax(mesh_.fieldRelaxationFactor("Yi"));
}

it should compile in OF 2.1.x

BR

Yes, it compiled. Thanks a lot

Just to learn more for future, how did you find the equivalent member functions in of2.1? I looked into everything and couldn't find them and it was because I didn't know where and what to look for!

Another problem, now that I have both libraries compiled, I went to to $FOAM_RUN/../applications and typed wmake modifiedReactingFoam and got this error:
modifiedReactingFoam.C:41:40: fatal error: multiSpeciesTransportModel.H: No such file or directory

Why can't it find the .H file although I have the my Make/options looks like it addresses that. Here is my Make/options:
EXE_INC = \
-I$(LIB_SRC)/turbulenceModels/compressible/turbulenceModel \
-I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/reactionThermo/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/chemistryModel/lnInclude \
-I$(LIB_SRC)/ODE/lnInclude \
-I$(LIB_SRC)/finiteVolume/lnInclude \
-I$(FOAM_USER_LIBBIN)/../diffusivityModels/lnInclude \
-I$(FOAM_USER_LIBBIN)/../multiSpeciesTransportModels/lnInclude


EXE_LIBS = \
-lcompressibleTurbulenceModel \
-lcompressibleRASModels \
-lcompressibleLESModels \
-lreactionThermophysicalModels \
-lbasicThermophysicalModels \
-lchemistryModel \
-lODE \
-lfiniteVolume \
-llduSolvers \
-L$(FOAM_USER_LIBBIN) \
-lmultiSpeciesTransportModels

Will be appreciated if you give me a hint on that too!
Thanks again

[mhsn]

Originally Posted by mhsn

Yes, it compiled. Thanks a lot

Just to learn more for future, how did you find the equivalent member functions in of2.1? I looked into everything and couldn't find them and it was because I didn't know where and what to look for!

Another problem, now that I have both libraries compiled, I went to to $FOAM_RUN/../applications and typed wmake modifiedReactingFoam and got this error:
modifiedReactingFoam.C:41:40: fatal error: multiSpeciesTransportModel.H: No such file or directory

Why can't it find the .H file although I have the my Make/options looks like it addresses that. Here is my Make/options:
EXE_INC = \
-I$(LIB_SRC)/turbulenceModels/compressible/turbulenceModel \
-I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/reactionThermo/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
-I$(LIB_SRC)/thermophysicalModels/chemistryModel/lnInclude \
-I$(LIB_SRC)/ODE/lnInclude \
-I$(LIB_SRC)/finiteVolume/lnInclude \
-I$(FOAM_USER_LIBBIN)/../diffusivityModels/lnInclude \
-I$(FOAM_USER_LIBBIN)/../multiSpeciesTransportModels/lnInclude


EXE_LIBS = \
-lcompressibleTurbulenceModel \
-lcompressibleRASModels \
-lcompressibleLESModels \
-lreactionThermophysicalModels \
-lbasicThermophysicalModels \
-lchemistryModel \
-lODE \
-lfiniteVolume \
-llduSolvers \
-L$(FOAM_USER_LIBBIN) \
-lmultiSpeciesTransportModels

Will be appreciated if you give me a hint on that too!
Thanks again

I had to change two the below lines:
-I$(FOAM_USER_LIBBIN)/../diffusivityModels/lnInclude \
-I$(FOAM_USER_LIBBIN)/../multiSpeciesTransportModels/lnInclude

to:
-I$(FOAM_RUN)l/../lib/diffusivityModels/lnInclude \
-I$(FOAM_RUN)/../lib/multiSpeciesTransportModels/lnInclude

I had to add some more lines as well, so the error resolved.
Now I face this error which I don't understand what it is about:

/usr/bin/ld: cannot find -llduSolvers

Do you know what it relates to? let me know if you needed more information.

Thanks

[mhsn]

Hey guys, thanks to your help, I could make modifiedReactingFoam work with openFoam2.1.1.
you may have to change some parts to be adapted to your openFoam especially in modifiedReactingFoam/Make/options and modifiedReactingFoam/Make/files

let me know if you needed that. I couldn't upload them regarding the maximum limit for the file size.

[openfoamstudents]

Dear novyno, dear community,


Great work and thanks for this library!

In your publication in Computer Physics Communications, you mention a generic boundary condition for species mass flux, called fixedFlux.
Could you please post it here? I would like to use it for part of my bachelor thesis on silicium wafer processing.

I am trying to implement a simple surface reaction boundary with a sticking coefficient 0..1 (only valid for Ficks law, similar to the boundary fixedGradient):

// Get Species name
const word specie_(dimensionedInternalField().name());

// Get p, T, rho, moleFrac, massFrac, Alpha,diffAlpha, molarWeight
const fvPatchField<scalar>& p = patch().lookupPatchField<volScalarField, scalar>("p");
const fvPatchField<scalar>& T = patch().lookupPatchField<volScalarField, scalar>("T");
const fvPatchField<scalar>& rho = patch().lookupPatchField<volScalarField, scalar>("rho");
// const fvPatchField<scalar>& massFrac = patch().lookupPatchField<volScalarField, scalar>(specie_); // Mass fraction
const fvPatchField<scalar>& moleFrac = patch().lookupPatchField<volScalarField, scalar>("x_"+specie_); // Mole fraction
const fvPatchField<scalar>& diffAlpha = patch().lookupPatchField<volScalarField, scalar>("D_"+specie_); // Diffusion constant
const scalar molarWeight(molecularWeights[specie_]); // kg/mol

// Constants
const scalar R(8.3144621); // J/(K*mol) = kg^2*m^2*s^-2*kgmol^-1
const scalar twoPi(6.283185307179586);

gradient() = -stickingCoeff_*p*moleFrac / (sqrt(twoPi*molarWeight*R*T) * (rho*diffAlpha));

Unfortunately, in every second iteration, this formula produces a gradient only containing zeros "gradient() 25{-0}" which probably means, moleFrac is exactly zero (unphysical I think).
Can somebody help me out please?

Thanks a lot,
OpenFoamStudent