Total heat release rate - variation not expected
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 |
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 |
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 |
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.cfd-online.com/Forums/ope...chemistry.html just to have all entries concerning fireFoam and the problems linked. Cheers, Michael |
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 |
How to calculate the heat release rate HRR
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 Hope this helps. Cheers, Michael |
Quote:
I put the below code to logSummary.H and dieselEngineFoam.C Code:
scalar HRRate = fvc::domainIntegrate(chemistry.dQ()).value(); Code:
foamCalcEx volIntegrate dQ Best regards. Code:
/*---------------------------------------------------------------------------*\ |
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? |
4 Attachment(s)
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 n-heptan 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 pressure-temp and HRRate and heat release graphics. I could not upload entire log file due to file size limit. Code:
/*---------------------------------------------------------------------------*\ Code:
massFlowRateProfile |
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..
|
5 Attachment(s)
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 n-heptan LHV= 44600 kJ/kg Added gas mass................. | 7.96266 mg heat=fuelmass*LHV= 355.134636 J (what i expected) and unit section... i use foam-extend.3.1 i suppose dQ calculated according to the below file /opt/foam/foam-extend-3.1/src/thermophysicalModels/chemistryModel/chemistryModel/ODEChemistryModel/ODEChemistryModel.C Code:
Line 576 Code:
/*--------------------------------*- C++ -*----------------------------------*\ when we calculate dQ*dt we get Joule Any information would be greatly appreciated. thanks in advance. Best regards. |
Ayhan,
graphic picture 3 looks too "thin" for me. I mean peak value is OK, but decrease very fast. Perhaps not all of the n-heptain evaporated and burns? |
you are right all of the n-heptane 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.cfd-online.com/Forums/ope...tml#post505976 Thanks for your reply Anthony, I really appreciate your help for HRRate... Best regards. |
Please how do I calculate the total release heat for plume rise @ gas flare stack
|
Hi everyone,
I am desperately trying to add the cumulative heat release vector in the logSummary file of my modified engineFoam solver. Indeed I am running a lot of engine (HCCI) simulations and I would like to have an easy access to the cumulativeHR in order to determine the combustion timing parameter (CA10,CA50 and CA90) for each simulations. This tread help me a lot as I am quite new to OpenFOAM and C++ programming. My first idea was to use run-time data processing with "#includeFunc Qdot" in my controlDict file. That allowed me to have a value in [J/m³ s] for each cell of my mesh (6500) at each write interval. However this is still not the value that I am interested in and I would prefer to have it directly in the logSummary file for easy post processing of the data using MatLab. Here is how I modified the logSummary.H file Code:
Info<< "Mean pressure:" << p.weightedAverage(mesh.V()).value() << endl; Code:
Info<< "Total cylinder mass: " << fvc::domainIntegrate(rho).value() << endl; Code:
root@LAPTOP-6V17VGK6:/opt/openfoam7/applications/solvers/lagrangian/sprayFoam/myEngineFoam# wmake Could anynody suggest me a fix to that problem ? I am running on a short notice as I have to finish my master thesis simulations within two weeks. Any help is therefore welcomed, Kind regards, François VdP. |
All times are GMT -4. The time now is 14:35. |