
[Sponsors] 
February 21, 2012, 10:52 
Total heat release rate  variation not expected

#1 
Member
Paulo Bufacchi
Join Date: Jun 2010
Posts: 50
Rep Power: 9 
Hi Foamers,
I ran into a variation in the total heat release rate when running two similar cases that were not expected to me. Let me explain what I did. I was running the case oppositeBurningPanels (fireFoam solver) with minor modifications as below: 1. the domain size in the Y direction was shortened from 4.2m to 2m; 2. the block resolution in the Y direction was lowered from 124 to 60; 3. the refinement block in the Y direction was shortened from 2.4m to 1m; 4. the panels height was shortened from 2.4m to 1m. Running the case as above, after time=3.00s I got a total heat release rate of 252 J/s. Then, for the second case I removed the right panel (in the original case there are two opposed panels). That's all I did. Running the second case with this single change, after time=3.00s I got a total heat release rate of 45 J/s. This value is 18% of the value in the first case. My expectation was the value to be 50% of the original one. Is there any reason for the total heat release rate to be so small in the second case? Thanks, Paulo 

September 12, 2012, 09:57 

#2 
New Member
Michael
Join Date: Dec 2011
Location: Geneva
Posts: 28
Rep Power: 8 
Hi Paulo,
unfortunaltey I cannot answer your questions. However, I realised, that the tutorial case smallPoolFire3D is also wrong in terms of set to calculated heat release rate. When you have a look at the speed of fuel at the inlet (Uy=0.0.1 m/s), multiplied with the area of the burner inlet (A=0.04m2), the density relating to set pressure and temperature (rho=0.65 kg/m3) and the heat of combustion estimated by the solver itself (∆Hv=5E7 J/kg) then you'll end up with 13 kW. Postprocessing the volume integral of the dQ scalar variable gives an average of 24 kW (55 saved time steps). I would not mind this, if the values would be below and above the set HRR due to the nature of an unsteady LES simulation. However, they are allmost all above the set power. I am using OpenFOAM 2.0.x build 931a91d59a3a currently, but I'll have a look at the behaviour of the newest version. Cheers, Michael 

September 12, 2012, 12:53 

#3 
Member
Paulo Bufacchi
Join Date: Jun 2010
Posts: 50
Rep Power: 9 
Hi Lithos,
Thanks for your time in addressing my issue. Unfortunately I had to move away from OpenFOAM due to difficulties I had to represent the scenario I am studying. Best regards, Paulo 

September 12, 2012, 13:58 

#4 
New Member
Michael
Join Date: Dec 2011
Location: Geneva
Posts: 28
Rep Power: 8 
Dear Paulo,
thanks for your reply. In fact it seems to be a problem of the diffusive mass flow in addition to the convective one. Please have a look here http://www.cfdonline.com/Forums/ope...chemistry.html just to have all entries concerning fireFoam and the problems linked. Cheers, Michael 

September 12, 2012, 14:47 

#5 
Member
Paulo Bufacchi
Join Date: Jun 2010
Posts: 50
Rep Power: 9 
Dear Lithos,
Thanks for the info. I checked the link you referenced, and it surprises me that mabinty didn't have a feedback on such an important issue. Regards, Paulo 

March 15, 2013, 08:56 
How to calculate the heat release rate HRR

#6 
New Member
Michael
Join Date: Dec 2011
Location: Geneva
Posts: 28
Rep Power: 8 
Dear all,
since I was asked how you could obtain the heat release rate: there are three ways I know currently: 1. you could calculate a volume integral of dQ (i.e. with Paraview) for your whole domain to obtain the overall heat release rate. This is not working if you have multiple sources of heat release and you want assess only one for sure. 2. you could put a monitor in you controlDict file before you carry out the calculation, i.e. Code:
functions ( volInts { type cellSource; functionObjectLibs ("libfieldFunctionObjects.so"); enabled true; outputControl timeStep; //outputTime; outputInterval 1; log true; //true; valueOutput false; source all; //cellZone; sourceName c0; operation volIntegrate; fields ( dQ ); } ); Hope this helps. Cheers, Michael 

July 24, 2014, 08:22 

#7  
Member
Ayhan Eses
Join Date: Mar 2009
Posts: 35
Rep Power: 10 
Quote:
I put the below code to logSummary.H and dieselEngineFoam.C Code:
scalar HRRate = fvc::domainIntegrate(chemistry.dQ()).value(); Info<< "HRRate = " << HRRate << " J/sW" << nl << endl; // Code:
foamCalcEx volIntegrate dQ Best regards. Code:
/**\  =========    \\ / F ield  foamextend: Open Source CFD   \\ / O peration  Version: 3.1   \\ / A nd  Web: http://www.extendproject.de   \\/ M anipulation   \**/ Build : 3.16c0c77dee21a Exec : dieselEngineFoamtemmuz2014tsu Date : Jul 24 2014 Time : 15:15:29 Host : ayhanvirtualmachine PID : 34548 CtrlDict : /opt/foam/foamextend3.1/etc/controlDict Case : /home/ayhan/foam/ayhan3.1/antorduzsilindirfoam31multiholeenj24swirlprofil40dereceTsurushimadQdeneme nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create engine time > FOAM Warning : From function entry::getKeyword(keyType&, Istream&) in file db/dictionary/entry/entryIO.C at line 77 Reading /home/ayhan/foam/ayhan3.1/antorduzsilindirfoam31multiholeenj24swirlprofil40dereceTsurushimadQdeneme/system/controlDict found on line 84 the punctuation token ')' expected either } or EOF > FOAM Warning : From function IOstream::compressionEnum(const word&) in file db/IOstreams/IOstreams/IOstream.C at line 74 bad compression specifier 'off', using 'uncompressed' Create mesh for time = 25 Selecting engineMesh layered deckHeight: 0.072 piston position: 0.0639363 Reading thermophysicalProperties Selecting psiChemistryModel ODEChemistryModel<gasThermoPhysics> Selecting thermodynamics package hsPsiMixtureThermo<reactingMixture<gasThermoPhysics>> Selecting chemistryReader chemkinReader Selecting chemistrySolver ode ODEChemistryModel: Number of species = 40 and reactions = 50 Reading field U Reading/calculating face flux field phi Creating turbulence model. Selecting turbulence model type RASModel Selecting RAS turbulence model kEpsilon kEpsilonCoeffs { Cmu 0.09; C1 1.44; C2 1.92; C3 0.33; sigmak 1; sigmaEps 1.3; Prt 1; } Creating field DpDt Creating field kinetic energy K Reading g Reading combustion properties Constructing Spray > FOAM Warning : From function Cloud<ParticleType>::initCloud(const bool checkClass) in file /opt/foam/foamextend3.1/src/lagrangian/basic/lnInclude/CloudIO.C at line 124 Cannot read particle positions file "/home/ayhan/foam/ayhan3.1/antorduzsilindirfoam31multiholeenj24swirlprofil40dereceTsurushimadQdeneme/25/lagrangian/defaultCloud" assuming the initial cloud contains 0 particles. Selecting injectorType multiHoleInjector injectionPressureProfile_.size() = 42, massFlowRateProfile_.size() = 42 end constructor. commonRail den alınan multihole Selecting atomizationModel off Selecting dragModel standardDragModel Selecting evaporationModel standardEvaporationModel Selecting heatTransferModel RanzMarshall Selecting wallModel reflect Selecting breakupModel ReitzKHRT Selecting collisionModel off Selecting dispersionModel off Selecting injectorModel hollowConeInjector Selecting pdfType RosinRammler Average Velocity for injector 0: 0.000127159 m/s, injection pressure = 19.7348 bar Constructing three dimensional spray injection. Courant Number mean: 8.6744e05 max: 0.000700434 velocity magnitude: 5.81392 ==startSummary.H yazdiriyor... Total cylinder mass: 0.387525 gram Starting time loop Courant Number mean: 8.6744e05 max: 0.000700434 velocity magnitude: 5.81392 > FOAM FATAL IO ERROR: all is not in enumeration 1 ( cellZone ) file: ::volInts::source at line 71. From function NamedEnum<Enum, nEnum>::read(Istream& is) const in file /home/dc/deb/foamextend3.1/src/foam/lnInclude/NamedEnum.C at line 74. FOAM exiting 

July 29, 2014, 05:43 

#8 
Member
Anthony Nitski
Join Date: Aug 2009
Location: Earth
Posts: 35
Rep Power: 10 
Dear all,
I have a question how to calculate total heat release (dQ integral over time) ?? In sprayEngineFoam solver i added the code: Info<< "Heat release [J]: " << fvc::domainIntegrate(dQ).value() * runTime.deltaTValue(). And when solver finishes i have to accumulate these values. Is it correct? Last edited by u22; July 30, 2014 at 05:28. 

August 1, 2014, 09:08 

#9 
Member
Ayhan Eses
Join Date: Mar 2009
Posts: 35
Rep Power: 10 
Dear all,
I put the below code dieselEngineFoam.C as u22 said Code:
Info<< "Heat release [J]: " << fvc::domainIntegrate(chemistry.dQ()).value() * runTime.deltaTValue() << nl << endl; // i use nheptan LHV= 44600 kJ/kg Added gas mass.................  7.96266 mg heat=fuelmass*LHV= 0.355134636 kJ (what i expected) i get 0,021976162 J from HRRate Is our calculation way of HRRate wrong? Please help what is wrong for this case? i put pressuretemp and HRRate and heat release graphics. I could not upload entire log file due to file size limit. Code:
/**\  =========    \\ / F ield  foamextend: Open Source CFD   \\ / O peration  Version: 3.1   \\ / A nd  Web: http://www.extendproject.de   \\/ M anipulation   \**/ Build : 3.16c0c77dee21a Exec : dieselEngineFoamtemmuz2014hrr Date : Aug 01 2014 Time : 12:55:15 Host : ayhanvirtualmachine PID : 17963 CtrlDict : /opt/foam/foamextend3.1/etc/controlDict Case : /mnt/hgfs/E/antorduzsilindirfoam31multiholeenj24swirlprofil40derecegrafikicinhrr nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create engine time > FOAM Warning : From function IOstream::compressionEnum(const word&) in file db/IOstreams/IOstreams/IOstream.C at line 74 bad compression specifier 'off', using 'uncompressed' Create mesh for time = 25 Selecting engineMesh layered deckHeight: 0.072 piston position: 0.0639363 Reading thermophysicalProperties Selecting psiChemistryModel ODEChemistryModel<gasThermoPhysics> Selecting thermodynamics package hsPsiMixtureThermo<reactingMixture<gasThermoPhysics>> Selecting chemistryReader chemkinReader Selecting chemistrySolver ode ODEChemistryModel: Number of species = 5 and reactions = 1 Reading field U Reading/calculating face flux field phi Creating turbulence model. Selecting turbulence model type RASModel Selecting RAS turbulence model kEpsilon kEpsilonCoeffs { Cmu 0.09; C1 1.44; C2 1.92; C3 0.33; sigmak 1; sigmaEps 1.3; Prt 1; } Creating field DpDt Creating field kinetic energy K Reading g Reading combustion properties Constructing Spray > FOAM Warning : From function Cloud<ParticleType>::initCloud(const bool checkClass) in file /opt/foam/foamextend3.1/src/lagrangian/basic/lnInclude/CloudIO.C at line 124 Cannot read particle positions file "/mnt/hgfs/E/antorduzsilindirfoam31multiholeenj24swirlprofil40derecegrafikicinhrr/25/lagrangian/defaultCloud" assuming the initial cloud contains 0 particles. Selecting injectorType multiHoleInjector injectionPressureProfile_.size() = 42, massFlowRateProfile_.size() = 42 end constructor. commonRail den alınan multihole Selecting atomizationModel off Selecting dragModel standardDragModel Selecting evaporationModel standardEvaporationModel Selecting heatTransferModel RanzMarshall Selecting wallModel reflect Selecting breakupModel ReitzKHRT Selecting collisionModel off Selecting dispersionModel off Selecting injectorModel hollowConeInjector Selecting pdfType RosinRammler Average Velocity for injector 0: 0.000127159 m/s, injection pressure = 19.7348 bar Constructing three dimensional spray injection. Courant Number mean: 0.000346976 max: 0.00280174 velocity magnitude: 5.81392 ==startSummary.H yazdiriyor... Total cylinder mass: 0.387525 gram Starting time loop Courant Number mean: 0.000346976 max: 0.00280174 velocity magnitude: 5.81392 Crank angle = 24.975 CAdeg deltaZ = 7.91565e06 clearance: 0.00805578 Piston speed = 4.17946 m/s Piston konumu (mm)= 63.9442 Piston yerdeğiştirme (mm)= 0.00791565 Piston hızı (m/s)= 4.17946 , T = 789.788, p = 1.95045e+06, C7H16 = 0 Solving chemistry diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 UEqn.H dosyası tamam DILUPBiCG: Solving for C7H16, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for O2, Initial residual = 0.0030041, Final residual = 3.23546e16, No Iterations 3 DILUPBiCG: Solving for CO2, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for H2O, Initial residual = 0, Final residual = 0, No Iterations 0 YEqn.H dosyası tamam DILUPBiCG: Solving for hs, Initial residual = 0.0086605, Final residual = 2.43842e07, No Iterations 1 EEqn.H dosyası tamam DICPCG: Solving for p, Initial residual = 0.965778, Final residual = 0.0184173, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.204614, Final residual = 0.00605899, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.00679623, Final residual = 0.000255068, No Iterations 1 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 2.56393e08, global = 9.25292e09, cumulative = 9.25292e09 pEqn.H dosyası tamam DICPCG: Solving for p, Initial residual = 0.000641585, Final residual = 1.83956e05, No Iterations 1 DICPCG: Solving for p, Initial residual = 1.8474e05, Final residual = 6.7099e07, No Iterations 1 DICPCG: Solving for p, Initial residual = 6.64488e07, Final residual = 6.64488e07, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 6.67414e11, global = 3.58652e11, cumulative = 9.28879e09 pEqn.H dosyası tamam DICPCG: Solving for p, Initial residual = 1.44558e05, Final residual = 3.33062e07, No Iterations 1 DICPCG: Solving for p, Initial residual = 3.32992e07, Final residual = 3.32992e07, No Iterations 0 DICPCG: Solving for p, Initial residual = 3.32992e07, Final residual = 3.32992e07, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 3.34456e11, global = 2.47535e12, cumulative = 9.29126e09 pEqn.H dosyası tamam DILUPBiCG: Solving for epsilon, Initial residual = 0.00150506, Final residual = 3.05437e08, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.000300666, Final residual = 8.07714e09, No Iterations 1 Mean pressure (pa): 1.95275e+06 Mean temperature (K): 815.163 Mean u'(m/s): 2.3296 Hacim (cmküp) 46.6023 Toplam silindir kütlesi (gram): 0.387525 Number of parcels in system....  0 Injected liquid mass...........  0 mg Liquid Mass in system..........  0 mg SMD, Dmax......................  0 mu, 0 mu Added gas mass.................  2.71051e13 mg Evaporation Continuity Error...  2.71051e13 mg enjekte edilmis kutle..........  0 mg Buharlasan kütle...............  0 mg liquidPenetration (1)..........  0 mm liquidPenetration (0.95).......  0 mm enjekte edilecek sivi kutle....  12.8189 mg enjekte edilmis entalpi........  0 J sivi entalpisi.................  0 J toplam sivi entalpisi..........  0 J sivi_fazin_kinetik_enerjisi....  0 J puskurtulen_sivi fazin kinetik enerjisi....  0 J HRRate = 0 J/sW Heat release [J]: 0 ExecutionTime = 0.22 s ClockTime = 1 s :::::::::::::::::::::::::::::::::bla bla bla::::::::::::::::::::::::::. Courant Number mean: 0.000268388 max: 0.00304259 velocity magnitude: 4.69281 Crank angle = 20 CAdeg deltaZ = 6.45075e06 clearance: 0.00662487 Piston speed = 3.40599 m/s Piston konumu (mm)= 65.3751 Piston yerdeğiştirme (mm)= 0.00645075 Piston hızı (m/s)= 3.40599 , T = 765.134, p = 2.68996e+06, C7H16 = 3.34728e15 Solving chemistry diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 UEqn.H dosyası tamam DILUPBiCG: Solving for C7H16, Initial residual = 8.21214e05, Final residual = 5.02072e16, No Iterations 2 DILUPBiCG: Solving for O2, Initial residual = 0.000106995, Final residual = 1.46664e15, No Iterations 2 DILUPBiCG: Solving for CO2, Initial residual = 0.000133814, Final residual = 1.48051e15, No Iterations 2 DILUPBiCG: Solving for H2O, Initial residual = 0.000133814, Final residual = 1.48051e15, No Iterations 2 YEqn.H dosyası tamam DILUPBiCG: Solving for hs, Initial residual = 0.000440409, Final residual = 1.69276e09, No Iterations 1 EEqn.H dosyası tamam DICPCG: Solving for p, Initial residual = 0.823998, Final residual = 0.02766, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.0743771, Final residual = 0.00428303, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.00428032, Final residual = 0.000245727, No Iterations 1 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 1.38177e07, global = 3.02512e08, cumulative = 3.58674e06 pEqn.H dosyası tamam DICPCG: Solving for p, Initial residual = 0.000265467, Final residual = 1.38747e05, No Iterations 1 DICPCG: Solving for p, Initial residual = 1.38875e05, Final residual = 9.78096e07, No Iterations 1 DICPCG: Solving for p, Initial residual = 9.74655e07, Final residual = 9.74655e07, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 5.48177e10, global = 3.28405e10, cumulative = 3.58707e06 pEqn.H dosyası tamam DICPCG: Solving for p, Initial residual = 1.12561e06, Final residual = 8.69588e08, No Iterations 1 DICPCG: Solving for p, Initial residual = 8.70896e08, Final residual = 8.70896e08, No Iterations 0 DICPCG: Solving for p, Initial residual = 8.70896e08, Final residual = 8.70896e08, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 4.89819e11, global = 3.52484e11, cumulative = 3.5871e06 pEqn.H dosyası tamam DILUPBiCG: Solving for epsilon, Initial residual = 0.00578654, Final residual = 8.97304e09, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.0019395, Final residual = 6.74305e09, No Iterations 1 Mean pressure (pa): 2.68524e+06 Mean temperature (K): 998.228 Mean u'(m/s): 1.15799 Hacim (cmküp) 38.3245 Toplam silindir kütlesi (gram): 0.395487 Number of parcels in system....  14527 Injected liquid mass...........  12.8189 mg Liquid Mass in system..........  4.85623 mg SMD, Dmax......................  111.955 mu, 158.943 mu Added gas mass.................  7.96266 mg Evaporation Continuity Error...  1.69948e06 mg enjekte edilmis kutle..........  12.8189 mg Buharlasan kütle...............  7.96266 mg liquidPenetration (1)..........  1.56647 mm liquidPenetration (0.95).......  0.803003 mm enjekte edilecek sivi kutle....  12.8189 mg enjekte edilmis entalpi........  27.1022 J sivi entalpisi.................  9.22292 J toplam sivi entalpisi..........  9.20413 J sivi_fazin_kinetik_enerjisi....  1.30673e07 J puskurtulen_sivi fazin kinetik enerjisi....  0.00737491 J HRRate = 0.000292321 J/sW Heat release [J]: 5.53638e10 ExecutionTime = 666.54 s ClockTime = 667 s End Code:
massFlowRateProfile ( (24 0.320472458) (23 0.320472458) (22 0.320472458) (21 0.320472458) (20 0.320472458) (19 0.320472458) (18 0.320472458) (17 0.320472458) (16 0.320472458) (15 0.320472458) (14 0.320472458) (13 0.320472458) (12 0.320472458) (11 0.320472458) (10 0.320472458) (9 0.320472458) (8 0.320472458) (7 0.320472458) (6 0.320472458) (5 0.320472458) (4 0.320472458) (3 0.320472458) (2 0.320472458) (1 0.320472458) (0 0.320472458) (1 0.320472458) (2 0.320472458) (3 0.320472458) (4 0.320472458) (5 0.320472458) (6 0.320472458) (7 0.320472458) (8 0.320472458) (9 0.320472458) (10 0.320472458) (11 0.320472458) (12 0.320472458) (13 0.320472458) (14 0.320472458) (15 0.320472458) (16 0) (1000 0) ); 

August 1, 2014, 09:30 

#10 
Member
Anthony Nitski
Join Date: Aug 2009
Location: Earth
Posts: 35
Rep Power: 10 
I guess its wrong. More correct is to sum dQ for all cells in domain. and then * dt and accumulate total heat release over all timesteps. What is dimension of dQ in dieselEngineFoam? in old versions of solver dQ=HRR/Cp AFAIK. not J/s..


August 12, 2014, 08:35 

#11  
Member
Ayhan Eses
Join Date: Mar 2009
Posts: 35
Rep Power: 10 
Quote:
I really appreciate your help... << fvc::domainIntegrate(chemistry.dQ()).value(); (graphic picture 1) << fvc::domainIntegrate(chemistry.dQ()).value() * runTime.deltaTValue() (graphic picture 2) i sum dQ for all cells in domain as you said in your last post. scalar sumHRRate = gSum(chemistry.dQ()()); << sumHRRate (graphic picture 3) << sumHRRate * runTime.deltaTValue() (graphic picture 4) cummulative_sum ( sumHRRate * runTime.deltaTValue() ) (graphic picture 5) i am not an expert i think the last 2 things seem true (graphic picture 4) & (graphic picture 5) what do you think about them are they logic? My problem is HRRate is lower (cummulative heat release 120 J graphic picture 5) than what i expected. i use nheptan LHV= 44600 kJ/kg Added gas mass.................  7.96266 mg heat=fuelmass*LHV= 355.134636 J (what i expected) and unit section... i use foamextend.3.1 i suppose dQ calculated according to the below file /opt/foam/foamextend3.1/src/thermophysicalModels/chemistryModel/chemistryModel/ODEChemistryModel/ODEChemistryModel.C Code:
Line 576 template<class CompType, class ThermoType> Foam::tmp<Foam::volScalarField> Foam::ODEChemistryModel<CompType, ThermoType>::dQ() const { tmp<volScalarField> tdQ ( new volScalarField ( IOobject ( "dQ", this>mesh_.time().timeName(), this>mesh_, IOobject::NO_READ, IOobject::NO_WRITE, false ), this>mesh_, dimensionedScalar("dQ", dimEnergy/dimTime, 0.0), // J/s zeroGradientFvPatchScalarField::typeName ) ); if (this>chemistry_) { volScalarField& dQ = tdQ(); dQ.dimensionedInternalField() = this>mesh_.V()*Sh()(); } return tdQ; } Code:
/** C++ **\  =========    \\ / F ield  foamextend: Open Source CFD   \\ / O peration  Version: 3.1   \\ / A nd  Web: http://www.extendproject.de   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class volScalarField; location "20"; object dQ; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 2 3 0 0 0 0]; // kgm^2/s^3 J/s internalField nonuniform List<scalar> 2288 ( 0 0 0 0 2.19708e06 3.48255e06 5.39679e06 when we calculate dQ*dt we get Joule Any information would be greatly appreciated. thanks in advance. Best regards. 

August 12, 2014, 23:19 

#12 
Member
Anthony Nitski
Join Date: Aug 2009
Location: Earth
Posts: 35
Rep Power: 10 
Ayhan,
graphic picture 3 looks too "thin" for me. I mean peak value is OK, but decrease very fast. Perhaps not all of the nheptain evaporated and burns? 

August 14, 2014, 09:02 

#13 
Member
Ayhan Eses
Join Date: Mar 2009
Posts: 35
Rep Power: 10 
you are right all of the nheptane not evaporated and burns
i think i also have some problems about to write correct species amounts. so i write a new thread about that problem. http://www.cfdonline.com/Forums/ope...tml#post505976 Thanks for your reply Anthony, I really appreciate your help for HRRate... Best regards. 

April 3, 2017, 10:12 

#14 
New Member
Okoye Emmanuel
Join Date: Apr 2017
Posts: 1
Rep Power: 0 
Please how do I calculate the total release heat for plume rise @ gas flare stack


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Nonpremixed combustion: local heat release rate  LB  FLUENT  0  September 3, 2007 12:58 
Compiling OpenFOAM13 on AMD64 with OpenSUSE 101  silent_missile  OpenFOAM Installation  5  August 10, 2007 07:31 
heat tansfer rate and mass transfer rate  Ryan  FLUENT  0  June 29, 2007 11:13 
heat release?  eric  Siemens  1  February 27, 2006 18:53 
total pressure influence on heat transfer  fab  Main CFD Forum  8  May 19, 2005 09:24 