
[Sponsors] 
September 18, 2013, 15:24 

#221  
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 
Quote:
You have no species in the folder 0! Otherwise you have the MASS FRACTION! Code:
// 13  species mass fractions Regards Tobi 

September 19, 2013, 02:44 

#222 
Member
Join Date: May 2013
Location: Netherlands
Posts: 30
Rep Power: 13 
I was to quick with answering, I didn't see the reply of Tobi untill I posted my reply


October 4, 2013, 15:25 

#224 
New Member
payal
Join Date: Aug 2013
Location: banglore
Posts: 14
Rep Power: 13 
Greetings Tobi,
actually after doing the given tutorial , i started to solve my case but to have some fair amount of idea i tried to use the PDFlibrary of the tutorial and rest of the files according to my own problem . case running well , but i don't have any idea upto how much time i should run it ? i tried to check the initial and final residual but there is still difference after T=15000 . so can you plz guide me through this . Thank You : Regards , Payal 

October 5, 2013, 14:07 

#225 
Senior Member
Bobby
Join Date: Oct 2012
Location: Michigan
Posts: 454
Rep Power: 15 
Hi Payal
Code:
but i don't have any idea upto how much time i should run it ? i tried to check the initial and final residual but there is still difference after T=15000 . @ Tobi Hi buddy I have found a point in flamelet model 2.2.x lookup table folder. You have put these lines in runFlameletGeneration.sh file: Code:
kinetics="PolimiC1C3" # # # aiabate flame # fEd[0]=800 # # # defects Another question buddy: Have you ever simulated a bluffbody stabilized flame (Sydney Items) with the solver? If hopefully yes, How was your accuracy? Regards Bobi 

October 5, 2013, 15:27 

#226 
New Member
payal
Join Date: Aug 2013
Location: banglore
Posts: 14
Rep Power: 13 
Thanks Bobi , i wl check that .....


October 5, 2013, 15:28 

#227 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 
Hi all,
@Bobi, 1. thanks for your hint to the tutorial with the wrong enthalpy defect for the adiabatic state. I changed that file. I think this mistake was a wrong key pressing in vim but now its corrected. 2. I never simulated a bluffbody stabilized flame. But I think Alberto and his team did it. But I am not sure if I mean the right kind of flames. So I can not give you an advice. 3. At the moment I am configurating my new server and therefor I have no time for cfd anymore. I wanted to calculate a complex gas burner but not now. @payal, 1. hello and welcome to the libOpenSMOKE thread. 2. for checking if your simulation is converged you have several options: a) checking the residuals with pyFoam/gnuplot or what ever you want. But keep in mind, that with the SIMPLE algorithm its not possible to get always nice residual graphics (eg. sandia flame tutorial  does not converge after 20.000 iterations; and would not du it) b) Check the residuals till they have a steady / or periodic fluctuations after that check your last timesteps (maybe everry 50 or 100 iterations; eg. 1500 1550 1600). If you can not realize big changes in your domain (U,T,csi etc.) then your solution should be converged. Problem of that solver is, that combustions always are very instationary and its hard to get a converged solution. There are always fluctuations in your domain  compare the CH4N2H2 flame  there is at the nozzle a field with fluctuation of U, and p so you will never get a convergence till 1e6 or something like that. c) Play with schemes and relaxation factors d) check the transient solver (PISO algorithm). Compared with the steady state solution you will get a very good convergence compared with SIMPLE algorithm in the tutorial case. Negativ aspect  not steady and therefor it take long time for calculation. 3. you have to create new PDFLibs for your problem Regards Tobi Last edited by Tobi; October 6, 2013 at 05:22. 

October 6, 2013, 13:33 

#228 
Senior Member
Bobby
Join Date: Oct 2012
Location: Michigan
Posts: 454
Rep Power: 15 
Hi Tobi
I think I have found my problem with complex flows. In my bluffbody stabilized burner (according to exp data) I should confront negative velocity fields (Due to recirculation zones both for fuel and oxidizer jets), However the achieved numeric data has minimum of zero. I took a look into fvSchemes file. I found that my scheme for velocity is bounded i.e. can not take negative values. Code:
divSchemes { div(phi,U) bounded Gauss limitedLinearV 1; div(phi,epsilon) bounded Gauss limitedLinear 1; div(phi,k) bounded Gauss limitedLinear 1; div(phiU,p) bounded Gauss limitedLinear 1; div(phi,H) bounded Gauss limitedLinear 1; div(phi,Z) bounded Gauss limitedLimitedLinear 1 0 1; div(phi,Zvar) bounded Gauss limitedLimitedLinear 1 0 0.25; div((muEff*dev2(T(grad(U))))) Gauss linear; } Do you have any hint for me that which type should I select to show the negative fields more accurate? Regards Bobi 

October 7, 2013, 02:32 

#229  
Member
Join Date: May 2013
Location: Netherlands
Posts: 30
Rep Power: 13 
Quote:
Please correct me if I'm wrong, shouldn't the velocity vector U always be positive (so the size of the velocity), of course the different components (Ux, Uy, Uz) can have negative values (which is the case for e.g. a recirculation zone). Regards 

October 7, 2013, 04:03 

#230 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 
Hi all,
for the schemes: the bound keyword is a trick for stabilisation: Code:
bound = Sp(...) Code:
Gauss limitedLimitedLinear 0 1 0,4 To clear the mind  the following declaration should be correct: Code:
Gauss limitedLinear 0 = Gauss linear Due to your fact of negative recirculation zones. TBT is correct  a vector is only positiv  just its components can be negativ. In the sandia flame you have already recirulation fields. 

October 7, 2013, 04:13 

#231  
Member
sonu
Join Date: Jul 2013
Location: delhi
Posts: 92
Rep Power: 13 
Greetings Tobi ,
Quote:
Code:
# aiabate flame # fEd[0]=800 Thank You , sonu 

October 7, 2013, 06:29 

#232 
Senior Member
Bobby
Join Date: Oct 2012
Location: Michigan
Posts: 454
Rep Power: 15 
Hi all
@sonu Simply, replace 800 with 0 and it's ok. @Tobi Thanks buddy for your hints.However, My problem is clearly poor prediction of flow field especially when we leave the nearfield region; Do you have any hint for me? I have exerted some modifications like as: finer mesh, C1 constant change from 1.45 to 1.60 I think may be change the kepsilon model and use another model. @TBO You are of course right, But actually I meant that my calculated data does not predict negative axial velocities and instead zero or near zero values are presented. Bobi 

October 7, 2013, 09:42 

#233 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 
Hi Bobi,
a) can you give me more information about your mesh ? maybe the whole case ? A link to that flame? b) how fine is your mesh in the area you should have recirculation? Can you give some pictures of U, p? c) Are your BC correct? d) A other turbulence model can be used ... hmm... e) SIMPLE or PISO ? did you tested both? f) 2D or 3D model? Hi sonu, as Bobi mentioned  adiabatic flame means that there is no enthalpy defect. So change the value of 800 to 0. https://github.com/shorty/flameletM...f61a406e0bc7f8 Further more you can find the description (in runFlameletGeneration.sh): Code:
# Description: # # This script builds nonadiabatic flamelet libraries for OpenFOAM and fluent used by the binaries from Alberto # # Cuoci. The defects has to be defined like below: # # # # fEd[0] >>> adiabat flame # # fEd[1] > fEd[x] >>> positiv enthalpy defects ( 10 20 30 100 200 ...) # # fEd[x+1] > fEd[end] >>> negativ enthalpy defects (10 20 30 100 200 ...) Regard 

October 7, 2013, 13:11 

#234 
Senior Member
Bobby
Join Date: Oct 2012
Location: Michigan
Posts: 454
Rep Power: 15 
Hi Tobi
Many thanks for your quick reply. 1 This the link to the HM1 flame http://sydney.edu.au/engineering/aer...uids/bluff.htm I will email you my 2D mesh (wedgetyped) 2 I think my mesh is fine enough. I have attached a pic of my flow field and temperature. Each stream (fuel and oxidizer) has its own recirculation zone in the wake behind the bluffbody. My problem is predicting of RZ not in the right place that has affected all of data. 3 Although other turbulence models like komegaSST might be more accurate but I have seen papers with kepsilon presenting bluffbody flames. 4 I have tested both Piso and Simple (the poor velocity field in farfield still appears in both), with no noticeable difference. 5 I have tested both 2D and 3D; no difference in accuracy. Regards Bobi 

October 7, 2013, 13:30 

#235 
Member
sonu
Join Date: Jul 2013
Location: delhi
Posts: 92
Rep Power: 13 
Thanks Tobi and Bobi for replying ....


October 7, 2013, 14:07 

#236 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 
Hi Bobi,
I think I know where the problem could be. Just let me check your geometry today night. I will have a try on that Bluff  Body  Flame. As I understand it right. The fuel is in the inner nozzle and the nozzle has a big thickness so you get air and fuel recirculation areas ? 

October 8, 2013, 15:32 

#237 
New Member
payal
Join Date: Aug 2013
Location: banglore
Posts: 14
Rep Power: 13 
Greetings all ,
i have a few very basic doubts. someone please clarify. i was just going through the Sandia_CH4H2N2 tutorial and there PHP Code:
Best Regards , Payal . 

October 8, 2013, 17:45 

#238  
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 
Quote:
first question  this variable has no sence to me I tryed several settings but nothing changed in the files  maybe its "initial" value to be faster in the iterations ? dont know  maybe its not used in the binaries (could be as possible too). second question  this is the math background. You create flamelets (2D  solutions). This solution describe every pyhsical and chemical variable like  temperature, density, mass fraction, cp ... depend on the mixture fraction Z. This flamelets are steady  state laminar flamelets and could be used for counterflow diffusion flames (like a candle). For ingenieering issues we always (or in most of the topics) have turbulent flow fields to get a better mixture of air and fuel. For that we have to expand the counterflow flamelets for turbulent flow fields. With the reynoldsaverage method we will have the average mixture fraction Z and its fluctuation Z''. In research it could be found that the best application for that is the favre averaging ... (i stop here). The thing you should know now it that you expand all variables which depend on the mixture fraction Z are now dependend on the average mixture fraction Z and its fluctuation Z'' (turbulent flow fields). This expansion are generated with the PDF's (probability distribution functions) for all variables (phi). Exeption 1: enthalpydefect = delta dirac function Exeption 2: scalar dissipation = log normal function (I hope its correct ) Back to the topic for Z and Z''. In the attachment you find two pictures. The first one is the 2D graphic  phi depends on Z The second one is the 3D graphic  phi depends on Z and Z'' How many calculation points you set for Z'' = No. of variance (here = 20 points) Further more you realize that the gradients are very high between 0 < Z'' < 0.1 So you can set a strech factor so that you can get more lines / points in the area of high gradients. At least you normalize the variance: Z is defined as: 0 <= Z <= 1 (0 = oxidator, 1 = fuel) Z'' is defined as: 0 <= Z'' < 0.25 (that depend on the betaPDF) OF solves two equations for Z and Z'' and for that you can interpolate in those graphics. The trick therefor is to normalize the Z'' lines so that the value is new defined: Z''_normalized defined as: 0 <= Z''_normalized <= 1 That is shown in picture 3. If you have that both values Z and Z''_normalized you can calculate all variables (area weighted interpolation). Hope that are enough information. regards Tobi 

October 9, 2013, 18:13 

#239 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 
At all,
I updated the flameletPisoFoam and flameletSimpleFoam tutorial (update of files) ... nothing necessary but for a clean tutorial its helpful. Regards Tobi 

October 10, 2013, 02:23 

#240 
New Member
payal
Join Date: Aug 2013
Location: banglore
Posts: 14
Rep Power: 13 
Thanx Tobi for such a explained answer and clearing my doubts. Also for updated tutorial
Regards, Payal. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Numerical treatment of the source term in combustion equations  Tobi  Main CFD Forum  37  September 15, 2020 13:42 
[openSmoke] flameletSmoke + new ODESolver (by Alberto Cuoci)  Tobi  OpenFOAM Community Contributions  1  November 21, 2017 18:24 
Unsteady solver with Flamelet Model (libOpenSMOKE)  francesco_capuano  OpenFOAM Running, Solving & CFD  11  November 26, 2013 04:50 
LibOpenSmoke, getting the species in ParaFoam  Christoph_84  OpenFOAM  1  May 31, 2012 14:42 