
[Sponsors] 
October 13, 2013, 04:01 

#241 
Senior Member
Bobi
Join Date: Oct 2012
Posts: 286
Rep Power: 6 
Hi Tobi
After trying to optimize my grid; I went to change my turbulence model. As suggested by hannes (FGM forum); I tried to implement realizableKE; However this error happens (even with RNGKEpsilon this error appears) Do you have any hint for this error? Code:
Starting time loop Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 1.76289432e08, No Iterations 6 DILUPBiCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0 GAMG: Solving for p, Initial residual = 1, Final residual = 0.000958120731, No Iterations 40 time step continuity errors : sum local = 0.0906109149, global = 0.00473111621, cumulative = 0.00473111621 DILUPBiCG: Solving for H, Initial residual = 0.999999999, Final residual = 1.40752135e08, No Iterations 9 Updating lookup table extractions... Updating mass fraction extractions... DILUPBiCG: Solving for csi, Initial residual = 1, Final residual = 3.12448826e08, No Iterations 10 DILUPBiCG: Solving for csiv2, Initial residual = 1, Final residual = 5.93143858e09, No Iterations 4 #0 Foam::error::printStack(Foam::Ostream&) in "/home/babak/OpenFOAM/OpenFOAM2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/babak/OpenFOAM/OpenFOAM2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/babak/OpenFOAM/OpenFOAM2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/babak/OpenFOAM/babak2.1.x/platforms/linux64GccDPOpt/bin/turbulentFlameletRhoSimplecFoam" #5 at realizableKE.C:0 #6 Foam::compressible::RASModels::realizableKE::correct() in "/home/babak/OpenFOAM/OpenFOAM2.1.x/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #7 in "/home/babak/OpenFOAM/babak2.1.x/platforms/linux64GccDPOpt/bin/turbulentFlameletRhoSimplecFoam" #8 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #9 in "/home/babak/OpenFOAM/babak2.1.x/platforms/linux64GccDPOpt/bin/turbulentFlameletRhoSimplecFoam" Floating point exception Bobi 

October 13, 2013, 04:49 

#242 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,125
Blog Entries: 6
Rep Power: 20 
Hi Bobi,
1. you ever need k and epsilon for that model so your turbulence model should work 2. as I realize the calculation of Z and Zvar is completed and the k value should be calculated while the error occure. Therefor I think its a problem of: a) Boundery b) Initial solution (did you use value uniform in every BC?) 3. I had a look at your case, there are some problems I found. 3.1. The side wall should not be a symmetryPlane 3.2. You should create your bluff body down the bottom (see attachment) 3.3. I changed some values of k and epsilon Have fun and I hope that my recirculation field is bigger than yours Kind Regards Tobi 

October 13, 2013, 05:38 

#243 
Senior Member
Bobi
Join Date: Oct 2012
Posts: 286
Rep Power: 6 
Many thanks to my friend Tobi.
Some hints For guys who want to change the turbulence model: the error that I posted earlier appears with GAMG solver and GaussSeidel smoother. Try using PCG and PBiCG solvers. the error would remove. Then kOmegaSST turbulence model is easily applicable. Regards Bobi 

October 13, 2013, 06:02 

#244 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,125
Blog Entries: 6
Rep Power: 20 
Hi all,
another hint to the solvers. In most cases its the best way to use PBiCG solver. numeric schemes I will update the tutorials today evening that none smoothsolver is used anymore. Regards Tobi 

October 13, 2013, 06:05 

#245 
Member
sonu
Join Date: Jul 2013
Location: delhi
Posts: 85
Rep Power: 4 
Greetings tobi,
just a kind reminder that in last updated tutorial the files in the constant folder like faces , points etc is missing . plz have a look on it . 

October 13, 2013, 13:32 

#247 
Member
sonu
Join Date: Jul 2013
Location: delhi
Posts: 85
Rep Power: 4 
ok tobi
Thank you . 

October 26, 2013, 07:20 

#248  
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,125
Blog Entries: 6
Rep Power: 20 
Quote:
Hi TBO, is your problem still there? I think the main reason you want not to simulate the cold flow with rhoSimpleFoam is the fact that the two different fluids are using different densitys. Therefor rhoSimpleFoam is not a good deal. With libOpenSmoke I think its possible but I will say that it s more commen to use a modified rhoSimpleFoam solver with two densitys I build this solver a time ago because one friend made a simulation of mixing air and methan. At the beginning he used a transient combustion solver. After that he used my scalarSimpleFoam (there is only one density  like rhoSimpleFoam). He get good results but after that I build a new solver with two densitys. He get a better accuracy there Sorry I don 't read your posts befor and therefor my answer is too late. With lib open smoke its not possible or better  it would be more work because the thermodynamic values are used out of the PDFLibrary. Therefor you had to change more things in the thermodynamic. Additionally all values are depend on "Z" and therefor you have different mixture fraction therefor different densitys etc. The libOpenSmoke solvers are none combustion solvers as xiFoam or sth. like that because you do not calculate the combustion while solving the flow field. Its separated into: 1. calculate chemistry 2. calculate flowfield Regards Tobi 

October 28, 2013, 03:54 

#249 
Member
Join Date: May 2013
Location: Netherlands
Posts: 30
Rep Power: 4 
Hi Tobi,
The problem is still there, I am very interested in your solution with using two different densities. Can you share that one (or where can I find it?) Regards, 

October 29, 2013, 07:20 

#251 
Senior Member
Bobi
Join Date: Oct 2012
Posts: 286
Rep Power: 6 
Hi Tobi
I am interested to the discussion with TBO as well. Is there any way that I have access to that solver too? Does your solver employs flamelet tabulation? Or is it a cold flow simulator? It seems that TBO is interested in cold flow simulations. Regards Bobi Last edited by babakflame; October 29, 2013 at 08:50. 

October 29, 2013, 09:33 

#252 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,125
Blog Entries: 6
Rep Power: 20 
Hi Bobi,
my solver is just a incompressible solver for mixing up two gases or liquids (Ma < 0,3). I think TBO wants to know the mixture fraction of two gases without chemical reactions. This solver is just a modified simpleFoam solver. I have to search for my solver today. Maybe I have to conntact my old friend that had made some simulations with that. It is not possible to connect it with the flameletlib. Why? Or what do you think is an advantage of that? Regards Tobi 

October 29, 2013, 11:07 

#253 
Senior Member
Bobi
Join Date: Oct 2012
Posts: 286
Rep Power: 6 
Hi Tobi
Thanks for your reply. Actually I thought that maybe you are talking about a kind of high mach algorithm .(Although RhoSimple and RhoPiso are high mach algorithms too). Cause You said this solver predicts mixing more efficient than RhoSimple algorithm, I thought that maybe its a better high mach solver. Since high mach algorithms take into account density fluctuations, I got a bad impact. Regards Bobi 

November 1, 2013, 11:02 

#255 
Senior Member
Bobi
Join Date: Oct 2012
Posts: 286
Rep Power: 6 
Hi Tobi
I have a doubt about radiation source term that is due to closed code of flamelet. ( Once, I met alberto but I forgot to ask about this part of his code, although he said that he does not work on turbulent flames anymore). I have seen both radiation source term in and out of flamelet equations. However according to pitsch papers I know that including radiative source terms in steady flamelet equations yields to unrealistic results. I think radiative source term is just in the enthalpy equation. Am I right? Also would you PLZ write the enthalpy equation of the code in latex form? I have a problem with this phi in the equation. 2 Your Rhopiso code has the ability to compute rms fluctuations. Since we can move in real times. I am computing these dataset now, if right results achieved, my proposal is to put the codes (available in O.F.) in the end of control dict so as to help users calculating rms data. 3 A question about RhoPiso algorithm: In this algorithm the spatial and temporal fluctuations of density and pressure are related to chemistry. Am I right? Regards Bobi Last edited by babakflame; November 1, 2013 at 12:16. 

November 4, 2013, 11:28 

#256 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,125
Blog Entries: 6
Rep Power: 20 
Hi Bobi,
the code for the enthalpy equation in the flamelet*Foam is that one: PISO SIMPLE If you compare it with the equation of the mixture fraction Z its the same: PISO Its just a conserved scalar equation. If you turn off radiation these both fields should be look identically. At least if you turn on the radiation you modify your terms like that: PISO SIMPLE and the additional source term Q_R is: The first variable is the boltzmannconstant and the second one is caclulated during teh flamelet calculation and is called planscher absorptionscoefficient. More informations can be found here: www.sandia.gov/TNF/radiation.html The last coefficient depend on the species and temperature. In the link you find the calculation of that coefficient with fitting curves. Additionall information can be found here: B.Marracino, D.Lentini: Radiation modelling in nonluminous nonpresmixed turbulent flames, Combustion Science and Technology, 128:2348 (1997) Hope this help you. Regards Tobi 

November 4, 2013, 11:54 

#257 
Senior Member
Bobi
Join Date: Oct 2012
Posts: 286
Rep Power: 6 
Hi Tobi
So Many thanks from your hints. Actually I am familiar with an optically thin radiation model. The point that I am investigating is the factor as (mean absorption coefficient). This factor is calculated from CO2,H2O and maybe CO and CH4 which are absorbing species. My problem is finding this procedure in this code. I couldn't find that which species are included in computing planck mean absorption coefficient? And If we can modify the featuring species or not? I invstigated the files, however with no success. I do not know how the code compute this factor. (From which source?) From your reply, It seems that this factor is again computed during this ..... flamelet calculation If I see alberto again, I am going to ask him that Why and Why his flamelet calculation step is closed. Just another short question:Is there any way to put out our PDF solutions? I mean our PDF plots. for instance PDF (Z) as a function of Z or PDF(chi) as a function of chi in different axial locations? Regards Bobi 

November 4, 2013, 14:09 

#258 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,125
Blog Entries: 6
Rep Power: 20 
Hi Bobi,
you are right. The mean absorption coefficient is calculated during the flamelet generation with the nice closed binaries. Therefor I can not say anything about it  which species are included and what exactly is calculated. I wrote an email to Alberto to ask about help of building my own flameletgeneration code  but still no feedback. But I think they are using the fitting curves in the link I wrote above. As I know from the Homepage it seems that there is only the laminar flamelet model available. Hmmm ... :/ It seems that they do not extend the code. Regards Tobi PS: Yes you can have a look at the laminar flamelets and plot everything (phi = f(Z)) or you can plot the PDFs (phi=f(Z,Zvar,enthalpydefect). 

November 6, 2013, 11:13 

#259 
Senior Member
Bobi
Join Date: Oct 2012
Posts: 286
Rep Power: 6 
Greetings Tobi
I am still working on my RhoPiso case. My case after trying different solvers (PCG and GAMG) for rho and P AND PBiCG for other variables still crashes. Always the same error: Code:
[4] #0 Foam::error::printStack(Foam::Ostream&) at ??:? [4] #1 Foam::sigFpe::sigHandler(int) at ??:? [4] #2 in "/lib/x86_64linuxgnu/libc.so.6" [4] #3 Foam::pdfFlameletThermo<Foam::flameletThermo, Foam::pureMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::update() at ??:? [4] #4 Foam::pdfFlameletThermo<Foam::flameletThermo, Foam::pureMixture<Foam::sutherlandTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:? [4] #5 [4] at ??:? [4] #6 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" [4] #7 [4] at ??:? [babakSystem:02614] *** Process received signal *** [babakSystem:02614] Signal: Floating point exception (8) [babakSystem:02614] Signal code: (6) [babakSystem:02614] Failing at address: 0x3e800000a36 It seems that the error is related to enthalpy and my thermotype. However cause we use flamelet , I can not change it. It's very odd. The position of myflow field when crashing is always neat the exit plane for fuel jet (bluffbody edge); even I computed my grid cells values in a way that compression before exit and expansion after exit are the same,But it crashes again. Do you have any hint for me? I have also tried upwind schemes, But I think that their convergence is lower than central schemes. Best Regards Bobi 

Thread Tools  
Display Modes  

