
[Sponsors] 
June 30, 2009, 09:53 
cellMixture: multicomponent mixture

#1 
New Member
Maria
Join Date: Apr 2009
Posts: 12
Rep Power: 13 
Hi !
I think I have found a bug in the "calculate()" function of a multicomponent mixture. Let me go step by step: 1. For multiComponentMixtures OpenFOAM calculates the cellMixture as: cellMixture = ForAll (i) { cellMixture += Y[i] / species[i].W() * speciesData[i] }; 2. Enthalpy in hCombustionThermo is massbased defined, meanwhile in specieThermo h is molarbased and H is massbased. 3. In hMixtureThermo::h (massbased) h = ForAll(i) { += Y[i] / species[i].W() * speciesData[i].H() }; where, as far as I understand, this H[i] is the massbased enthalpy calculated in specieThermo. 4. Having a look at the units of the hMixtureThermo::h => [m^2 s^(2)] != [][Kmol_i Kg_i^(1)]*[m^2 s^(2)] Which IS DIMENSIONALLY INCORRECT!! ... It does the same for calculating alpha/mu of the mixture, which are defined also in a MASS basis. So: I guess it should be fixed replacing the current cellMixturedefinition of multiComponentMixture by: cellMixture = ForAll (i) { cellMixture += Y[i] * speciesData[i] }; Is there really a bug..or I am missing something?? Regards! Last edited by mgc; July 1, 2009 at 04:14. 

June 30, 2009, 12:18 

#2  
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 694
Rep Power: 25 
Quote:
Quote:
This is an inconsistency in the naming convention. Quote:
I cannot find it anywhere. It looks like you have replaced speciesData in Q1 with H, which is incorrect. All I can find in there that is fairly similar is this (which is correct): Code:
136 template<class MixtureType> 137 Foam::tmp<Foam::scalarField> Foam::hMixtureThermo<MixtureType>::h 138 ( 139 const scalarField& T, 140 const labelList& cells 141 ) const 142 { 143 tmp<scalarField> th(new scalarField(T.size())); 144 scalarField& h = th(); 145 146 forAll(T, celli) 147 { 148 h[celli] = this>cellMixture(cells[celli]).H(T[celli]); 149 } 150 151 return th; 152 } Quote:
but all the code is correct. I get the feeling you have started in the wrong end. Looking at how nasa polynomials are defined, which is the speciesData. (or it could just as well be janaf) http://www.me.berkeley.edu/gri_mech/data/nasa_plnm.html H/RT = a1 + a2 T /2 + a3 T^2 /3 + a4 T^3 /4 + a5 T^4 /5 + a6/T unit for R is J/mol*K and the right hand side is dimensionless. so H is in J/mol. and if you want to calculate the enthalpy for the mixture you just add these coefficients together on a molar fraction basis. Thus the a1 coefficient for the mixture is sum of all its components = sum (X_i*a1_i) That is what the forloop does in Q1. I hope all is clearer now 

June 30, 2009, 13:38 

#3 
New Member
Maria
Join Date: Apr 2009
Posts: 12
Rep Power: 13 
Finally, I got it.
For those who could have the same doubt, I copy the keypoint (in my opinion) to understand how the "cellMixture" works: // template<class ThermoType> const ThermoType& multiComponentMixture<ThermoType>::cellMixture ( const label celli ) const { mixture_ = Y_[0][celli]/speciesData_[0].W()*speciesData_[0]; for (label n=1; n<Y_.size(); n++) { mixture_ *+=* Y_[n][celli]/speciesData_[n].W()*speciesData_[n]; } return mixture_; } // template<class equationOfState> inline void janafThermo<equationOfState>::*operator+=* ( const janafThermo<equationOfState>& jt ) { scalar molr1 = this>nMoles(); equationOfState:: operator+=(jt); molr1 /= this>nMoles(); scalar molr2 = jt.nMoles()/this>nMoles(); Tlow_ = max(Tlow_, jt.Tlow_); Thigh_ = min(Thigh_, jt.Thigh_); Tcommon_ = molr1*Tcommon_ + molr2*jt.Tcommon_; for ( register label coefLabel=0; coefLabel<janafThermo<equationOfState>::nCoeffs_; coefLabel++ ) { highCpCoeffs_[coefLabel] = molr1*highCpCoeffs_[coefLabel] + molr2*jt.highCpCoeffs_[coefLabel]; lowCpCoeffs_[coefLabel] = molr1*lowCpCoeffs_[coefLabel] + molr2*jt.lowCpCoeffs_[coefLabel]; } } Regards! María Last edited by mgc; July 15, 2009 at 05:57. 

May 12, 2013, 23:06 

#4 
New Member
何刚
Join Date: Jan 2011
Posts: 25
Rep Power: 11 
So, we could only set janafThermo? And what about the hconstThermo?


April 27, 2017, 11:18 

#5 
New Member
Join Date: Dec 2013
Posts: 11
Rep Power: 8 
Dear Maria and Niklas,
sorry for reviving this old thread but I am currently looking into the same issue and haven't fully understood how the mixtures are calculated in OpenFOAM, yet. I work with release 2.3.x and am looking at the equation given below: forAll (i) { cellMixture += Y[i] / species[i].W() * speciesData[i] } As I understand, speciesData[i] and cellMixture may for example be the coefficients of the JANAF polynomials: speciesData[i] for component i and cellMixture for the mixture. However, I feel like the molar mass of the mixture is missing in the equation. As it is now, the value of the coefficient related to the mixture should be scaled by the molar mass of the mixture or do I forget something? Moreover, the dimensions of "speciesData" and "cellMixture" should be different. Is this corrected at a later stage within the mixture property calculation? I hope you can help me find my error in reasoning! Thanks already! 

August 9, 2018, 17:59 
Understanding cellMixture: OpenFOAM incorrect density calculation in rhoReactingTherm

#6  
Member
Raunak Bardia
Join Date: Jan 2015
Posts: 32
Rep Power: 7 
Hi everyone,
LONG POST, PLEASE READ! At present, I am working with rhoReactingFoam in OpenFOAM v 5.0. On doing some digging into the solver, I was confused about the cellMixture calculations. Here are my observations, and I would request the senior members to please take some time and help the new Foamers understand this method. Disclaimer: The calculations seem to have been modified from previous versions of OpenFOAM so I will be posting everything afresh. 1) Where does rhoReactingFoam update thermophysical properties? The only viable candidate was in EEqn.H Code:
{ ... EEqn.relax(); fvOptions.constrain(EEqn); EEqn.solve(); fvOptions.correct(he); thermo.correct(); // properties are probably calculated in this Info<< "min/max(T) = " << min(T).value() << ", " << max(T).value() << endl; } rhoReactionThermo.H Code:
class rhoReactionThermo : public rhoThermo { ... (attached with this post) of my case in the constant directory, I use the heRhoThermo ($FOAM_SRC/thermophysicalModels/basic/rhoThermo/heRhoThermo.*) type of rhoThermo. The correct function has been defined in this class. It simply calls another function in this class called calculate(), which is shown below: heRhoThermo.C Code:
template<class BasicPsiThermo, class MixtureType> void Foam::heRhoThermo<BasicPsiThermo, MixtureType>::calculate() { const scalarField& hCells = this>he(); const scalarField& pCells = this>p_; scalarField& TCells = this>T_.primitiveFieldRef(); scalarField& psiCells = this>psi_.primitiveFieldRef(); scalarField& rhoCells = this>rho_.primitiveFieldRef(); scalarField& muCells = this>mu_.primitiveFieldRef(); scalarField& alphaCells = this>alpha_.primitiveFieldRef(); forAll(TCells, celli) { const typename MixtureType::thermoType& mixture_ = this>cellMixture(celli); TCells[celli] = mixture_.THE ( hCells[celli], pCells[celli], TCells[celli] ); psiCells[celli] = mixture_.psi(pCells[celli], TCells[celli]); rhoCells[celli] = mixture_.rho(pCells[celli], TCells[celli]); muCells[celli] = mixture_.mu(pCells[celli], TCells[celli]); alphaCells[celli] = mixture_.alphah(pCells[celli], TCells[celli]); } ..... Handle Boundary Patches This class does not implement the cellMixture function but instead inherits it from the multiComponentMixture. Code:
template<class ThermoType> class reactingMixture : public speciesTable, public autoPtr<chemistryReader<ThermoType>>, public multiComponentMixture<ThermoType>, public PtrList<Reaction<ThermoType>> { ... multiComponentMixture.C Code:
template<class ThermoType> const ThermoType& Foam::multiComponentMixture<ThermoType>::cellMixture ( const label celli ) const { mixture_ = Y_[0][celli]*speciesData_[0]; /* mixture is of datatype ThermoType and is initialized with speciesdata of 1st specie multiplied by its mass fraction*/ for (label n=1; n<Y_.size(); n++) { mixture_ += Y_[n][celli]*speciesData_[n]; /* All the weighted species data of remaining species is added to the mixture variable. Now, any property needed for the mixture can directly be accessed from the mixture itself. */ } return mixture_; } a = 1; b = 2; a += b; => a = 3; But, in OpenFOAM, they have redefined the way this and other operators behave for the thermoType class (mixture is a thermoType variable). 6) In my case again, thermophysicalProperties defines thermoType thermo as hPolynomial. So, I go to $FOAM_SRC/thermophysicalModels/specie/thermo/hPolynomial/hPolynomialThermoI.H, where this operator has been defined. hPolynomialThermoI.H Code:
template<class EquationOfState, int PolySize> inline void Foam::hPolynomialThermo<EquationOfState, PolySize>::operator+= ( const hPolynomialThermo<EquationOfState, PolySize>& pt ) { scalar Y1 = this>Y(); EquationOfState::operator+=(pt); if (mag(this>Y()) > SMALL) { Y1 /= this>Y(); const scalar Y2 = pt.Y()/this>Y(); Hf_ = Y1*Hf_ + Y2*pt.Hf_; Sf_ = Y1*Sf_ + Y2*pt.Sf_; CpCoeffs_ = Y1*CpCoeffs_ + Y2*pt.CpCoeffs_; hCoeffs_ = Y1*hCoeffs_ + Y2*pt.hCoeffs_; sCoeffs_ = Y1*sCoeffs_ + Y2*pt.sCoeffs_; } } 7) The bold part calls another operator for equationofstate (in my case icoPolyomial) $FOAM_SRC/thermophysicalModels/specie/equationOfState/icoPolynomial/icoPolynomialI.H Code:
template<class Specie, int PolySize> inline void Foam::icoPolynomial<Specie, PolySize>::operator+= ( const icoPolynomial<Specie, PolySize>& ip ) { scalar Y1 = this>Y(); Specie::operator+=(ip); if (mag(this>Y()) > SMALL) { Y1 /= this>Y(); const scalar Y2 = ip.Y()/this>Y(); rhoCoeffs_ = Y1*rhoCoeffs_ + Y2*ip.rhoCoeffs_; } } Code:
inline void specie::operator+=(const specie& st) { const scalar sumY = Y_ + st.Y_; if (mag(sumY) > SMALL) { molWeight_ = sumY/(Y_/molWeight_ + st.Y_/st.molWeight_); } Y_ = sumY; } Single Cell: Details: Specie 1: Molecular Weight = 36.46, Mass Fraction = 0.025, Density = (458.6 0 0 0 0 0 0 0) // icoPolynomial definition Specie 2: Molecular Weight = 112.56, Mass Fraction = 0.60, Density = 969.8 Specie 3: Molecular Weight = 98.92, Mass Fraction = 0.375, Density = 1089.4 Quick density calculation: Quote:
where Yi is mass fraction of each specie, and rhoi is density of each specie. For our example it comes out to be 982.874 But OpenFOAM calculates it to be 1001.87 (Output Log attached with this post). This number matches exactly if we calculate, Quote:
Interestingly, multiComponentMixture class has another function cellVolMixture, which seems to calculate the density correctly. But this is not the function called to define the mixture type in rhoReactionFoam. Code:
template<class ThermoType> const ThermoType& Foam::multiComponentMixture<ThermoType>::cellVolMixture ( const scalar p, const scalar T, const label celli ) const { scalar rhoInv = 0.0; forAll(speciesData_, i) { rhoInv += Y_[i][celli]/speciesData_[i].rho(p, T); } mixtureVol_ = Y_[0][celli]/speciesData_[0].rho(p, T)/rhoInv*speciesData_[0]; for (label n=1; n<Y_.size(); n++) { mixtureVol_ += Y_[n][celli]/speciesData_[n].rho(p, T)/rhoInv*speciesData_[n]; } return mixtureVol_; } ## THE END ## 

August 12, 2018, 22:28 

#7 
Senior Member
Yan Zhang
Join Date: May 2014
Posts: 108
Rep Power: 8 
Hi Raunak,
Actually, the operator += in the calculation of mixture_ is defined in the class sutherlandTransport (or other transport class). You can have a look at this post: https://openfoam.top/en/thermodynamicLIB/. Sorry its in Chinese, but I think the UML will help. As you can see in the UML, multiComponentMixture<ThermoType> needs a template, it can be gasHThermoPhysics, i.e. Code:
sutherlandTransport<species::thermo<janafThermo<perfectGas<specie>>,sensibleEnthalpy>> Code:
polynomialTransport<species::thermo<hPolynomialThermo<icoPolynomial<specie, 8>,8>,sensibleEnthalpy>,8>
__________________
https://openfoam.top/en 

July 12, 2019, 17:28 

#8 
New Member
Join Date: Jul 2012
Posts: 7
Rep Power: 10 
Hi Raunak,
can you share the code you used to probe the density calculation in a singlecell? I think I'm noticing the same issue, and would like to doublecheck Thank you very much 

July 12, 2019, 17:51 

#9 
Member
Raunak Bardia
Join Date: Jan 2015
Posts: 32
Rep Power: 7 
Hey,
I dealt with this issue about a year ago and can't really recall the exact solution I found for this. It was proprietary work so I don't even have my code to go back and look. If I recall, I played around a bit with this for a while but then skipped trying to understand the existing thermophysics model and defined one for my own case. Added it as another run time selectable model and used it in my simulations. Sorry, I am not much help on this one. Hope you will figure it out. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
cellMixture: multicomponent mixture  mgc  OpenFOAM  2  July 15, 2009 05:59 
Improvement to the update of T_ et al in hMixtureThermoC and hhuMixtureThermoC  richpaj  OpenFOAM Bugs  2  October 9, 2008 22:14 
multi component  ranap  Main CFD Forum  1  October 8, 2008 03:00 
multi component diffusivity  mahut  FLUENT  0  October 10, 2007 04:05 
doubt about background fluid in multico mixture...  Giosuč  Siemens  0  June 11, 2004 05:18 