
[Sponsors] 
February 24, 2014, 15:18 

#321 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,332
Blog Entries: 5
Rep Power: 22 
Hi,
1. you fvSchemes are very crazy  you defined the same laplacian schemes twice  you are using limitedLinear01 1 for Zvar  not correct  you can use bounded schemes better than unbounded (in 2.2) if you are using 2.1 you dont have to bound it because its bounded in the source code. you are using a lower type of openfoam 2. Zvar is only set to fixedValue 0 on inlets  not on walls. 3. Z is defined to fixedValue on the bluffBody wall to 4. Question: Which mesher did you use? ICEM ? Nice mesh...! 5. Maybe you have to build the bluff body solid and the burner design for 10 cm or sth. like that. That means: your mesh is to small down the burner. You have to add the walls of the burner etc. At the moment I am calculating the stuff. I keep you posted. Regards Tobi 

February 25, 2014, 02:30 

#322 
Member
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5 
Hi Tobi,
1. Yeh, I have made some silly mistake..in fvScheme. Right now, I corrected and made the modification as per as Bobi's suggestion. My OpenFOAM version 2.2.1 Flamelet model 2.1 2.What kind of boundary condition should i use for Z and Zvar in wall? "type calculated" or "type zeroGradient" please suggest something........ 3. For meshing, I used gambit meshing software....using cooper mesh. Regards, Vishal 

February 25, 2014, 03:31 

#323 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,332
Blog Entries: 5
Rep Power: 22 
Hi,
Z is fixed only on inlets and on other walls and patches "ZeroGradient". Zvar is fixed only on inlets with zero and on other walls and patches "zeroGradient" U on your outlet should be zeroGradient or inletOutlet with inletValue (0 0 0) The suggestion from bobi is the standard fvScheme file coming with the tutorial (: I hope your simulation run now. Gambit  free software? 

February 25, 2014, 05:23 

#324 
Member
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5 
Hi Tobi,
Gambit is free software but this for windows, not for linux, i think. I made the modification for Z, Zvar and lets see what happen.... I have another question. Is it possible to calculate the mixture fraction and its variance using this solver for nonreacting flow? How i have to make modification and decoupled between flow field and PDF library? Regards, Vishal 

February 25, 2014, 06:30 

#325 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,332
Blog Entries: 5
Rep Power: 22 
Hi,
yes you can do this but it is not the same if you decouple from the PDF because you are just solving a scalar field (Z) and (Zvar) which does not have influence to the flow field. That is not correct. But you can do it. Therefor make a new solver and implement the two equations in your solver. Those are calculated then but you will get rho mu etc. from the Standard openfoam thermodynamics (no combustion)... It is just a mixing solver but a bad mixing solver because you always have one constant density. Hence this Problem I made a solver (2 years ago) where you can mix nonreacting flows with two incompressible fluids (different densitys). I am not sure if this is what you want. Regards Tobi 

February 25, 2014, 07:53 

#326 
Member
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5 
Hi Tobi,
I have done this kind of thing using twoliquidMixingFoam under multiphase solver in OpenFoam for calculation of rho,Z,Zvar . But i am unable to calculate Zvar as there was a term mut =rho*nut .In case of incompressible flow there is no "mut" . So i am unable to use this solver for calculation of Zvar. But i have no idea how to implement this standard openfoam thermodynamics library for calculation of rho and mut. Can you suggest something , regarding this issue..? Regards, Vishal 

February 25, 2014, 12:17 

#327 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,332
Blog Entries: 5
Rep Power: 22 
Hi,
well if you are using an incompressible solver all Eqn. are divided with rho. In your case you have to use "nu_t" or "nu_eff". Additionally if you want to use Z, Zvar for the flame calculations you can generate a new scalar called rhoConstant and define a fix value for it. then you can calculate Z like that: Code:
fvm::laplacian(nu_t*rhoConstant, Zvar); If you are using the flameletSolver after that, all thermodynamics especially the density and mu_t are extracted out of the PDFLibraries and changing a lot. Density from 0.2  1.2 (for example). Regards. 

February 26, 2014, 08:53 

#328 
Member
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5 
Hi Tobi,
Thanx a lot for your suggestion, I try to implement this for non reacting flow for calculation of Zvar. Right now my case is running for swirl flame...I keep you update soon about my result... Regards, Vishal 

February 26, 2014, 12:59 
news to libOpenSMOKE

#329 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,332
Blog Entries: 5
Rep Power: 22 
Hi all,
i got a feedback from alberto cuoci. He and his team is still working on the flamelet solver and the flamelet generator. They modified it and made it more stable  especially the calculation of flamelets and solvers. Therefor I will not investigate time into a new flamelet generator or LES or RANS model till the new libraries are published. Alberto mentioned that they will publish the stuff after the they published the stuff on an international journal. The source code of the flamelet generator will also be published after the paper. PS: I kept this information very short because I will wait till the release will come. It is just an information for you that they still working on the solver and the whole stuff. Regards Tobi 

February 27, 2014, 01:55 

#330 
Senior Member
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 304
Rep Power: 6 
Greetings Tobi
Does their solver support LES? Cause, as I knew, they were working on laminar flames. Regards Bobi 

February 27, 2014, 02:56 

#331  
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,332
Blog Entries: 5
Rep Power: 22 
Quote:
I can not tell you if they're working on les sikver but albrto mentioned a lot of topics they are working. Additionally we had a short information transfer about the other flamelet model from the munic guys. I think les is build by the team to. If not, it is very easyvto implement. In our / my case the pressure linked eqn if the piso solver should be corrected. After that I think this solver works better than now (: Regard Tobi
__________________
Best regards, Tobias Holzmann Some interesting OpenFOAM tutorials and videos on www.Holzmanncfd.de Last edited by Tobi; February 27, 2014 at 13:59. 

March 3, 2014, 03:12 

#332 
Member
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5 
Hi Tobi and all,
My swirl flame is not stable at the downward region. I post you my two velocity for 30000 and 32000 iteration, can you kindly suggest something?? https://www.dropbox.com/s/hr0jr3lqzmmtd44/30000.jpg https://www.dropbox.com/s/ag9ovipkkwm2r6f/32000.jpg As well as I plot Z and Zvar but in case of Zvar its prediction is too small. Please comment on this thing. What should I do? https://www.dropbox.com/s/9h1a9b8p05...Zvar_30000.pdf I also tried with kOmegaSST but Zvar prediction is upto 200. So I tried this kOmegaSST model in algebric mode for Zvar. Regards, Vishal 

March 3, 2014, 05:46 

#333 
Senior Member
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 304
Rep Power: 6 
Greetings Vishal
The bluffbody stabilized swirl flames show unsteady behaviour especially in far downstream locations due to local extinction and reignition which both RAS model and steady flamelet approach are incapable of capturing it thoroughly. You should try to compare your results with experiments in locations with x/D less than 3. Cause after passing this distance Your implemented models are incapable of capturing the existing phenomena (vortex breakdown). Regards bobi 

March 3, 2014, 06:28 

#334 
Member
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5 
Hi bobi,
Can you make some suggestion regarding my Zvar calculation, because it is very less compare to the experimental value....how can I improve this value... Regards, Vishal 

March 3, 2014, 06:44 

#335 
Senior Member
Bobi
Join Date: Oct 2012
Location: Chicago, Illinois
Posts: 304
Rep Power: 6 
Greetings Vishal
There are some ways to improve your results in capturing mixing (includes mixture fraction and its variance) But you can not go further than a limit (Cause of the models shortcomings) 1 Modifying the C1 constant in dissipation equation of kepsilon in RAS properties file to 1.60 2 increase your grid nodes in downstream (not very much cause makes discretization errors) 3 try transport equation for mixture fraction variance 4 Using schemes proposed by Tobi in tutorial For your mixture fraction variance I think increasing grid points would make your results a bit Better (especially in near burner region) Regards Bobi 

March 3, 2014, 07:19 

#336 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,332
Blog Entries: 5
Rep Power: 22 
Hi all,
in my opinion a Change in the turbulence model is not a good way. I know a lot of cfdengineers that change empirical model constants but does that makes sence? Therefor you will always get good results with changing "model" Parameters. Hence this is done you never can be sure if the model is consistent or accurate in the next simulation. If the constant of 1.6 is given in literature you can check it out. But if you changing Parameters of models it should be able to get good results in every Simulation  does that makes sence and is this CDF? My hints to you: Decrease your mesh cells because your are very fine and you are solving RANS equations  not LES, DES nor DNS. Ansys CFX or fluent will manage this Problem in a better way but if you are doing RANS simulation with OpenFOAM and apply a very fine mesh you will not get accurate and good/stable results. Hence this is done you will get fluctuations over time and the residuals are not as stable as they should. To decrease your mesh I would doing a 2D Rotation symetric mesh or using symmetryPlanes and just use 1/4 of your Domain  additionally I would decrease the cells in your 3D Domain. To make a Research in your 3D Domain is very expensive (computational costs) Regards Tobi 

March 3, 2014, 14:48 

#337 
Member
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5 
Hi Bobi and Tobi,
I have made a silly mistake regarding the plotting of Zvar, there is experimental data for rms of Zvar .So i get some amount of matching profile. But as there is no effect of mixture fraction and mixture fraction variance after axial distance of 55 mm. How do I take care of this issue as tobi said fine mesh would not be help anyway and it should create unstable residual?? Regards, Vishal 

March 4, 2014, 05:58 

#338 
Senior Member
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,332
Blog Entries: 5
Rep Power: 22 
Therefor you should use transient solver but the piso solver I created is not stable due to the pressure equation
I will work on that (maybe) but first I think I am going to check out the release of the libOpenSMOKE tool! 

March 4, 2014, 06:00 

#339 
Member
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5 
Hello,
I plot the residuals, it is seen that after around 10000 iteration residual start oscillating. Oscillation of P residual is fluctuated more, I used fvSolution for P is PCG. plots are here ... https://www.dropbox.com/s/k2u3df1ktrx9a9c/residual.pdf What is the reason of this oscillation...fine mesh or any other reason is also there ...??? ....I am really confused about this issue...please suggest...... Regards, Vishal 

March 4, 2014, 06:48 

#340 
Member
vishal
Join Date: Mar 2013
Posts: 55
Rep Power: 5 
Hi all,
What is the function of 'reltol'....? Can it be help in any way for improvement of the solution?? Regards, Vishal 

Thread Tools  
Display Modes  

