
[Sponsors] 
November 20, 2016, 20:19 
kklOmega SimpleFoam divergence, kt kl omega

#1 
New Member
Anonymous
Join Date: Apr 2016
Posts: 8
Rep Power: 6 
Hi everyone
I'm fairly new in OpenFoam and I'm trying to do a steady simulation of a NACA0006 airfoil at Re=3*10⁶ and AoA=3 deg. I have chosen the kklOmega turbulence model to try to get a decent drag prediction but I am having trouble achieving a convergent solution. I'm running OpenFoam 3.0 so as far as I can tell the kklOmega bugs from earlier versions should be corrected (but I could be wrong). After reading through the numerous other threads in the forum on how to set up simulations with this model I have tried a lot of different combinations of BC's, schemes and solvers but the problem persists. What happens specifically is that omega, kl, and kt grows to huge max (and also huge negative min) values and also the time step continuity error blows up. This usually happens already after 525 iterations. For meshing I have used this mesher: http://hvirvel.dk/airfoilmesher/ I generates a circular domain and an ogrid around the airfoil. I have been increasing the grading in the direction normal to the airfoil in order to get y+ < 1 and my current mesh has 180k cells. The radius of the domain is 50 chord lengths. My blockMeshDict is attached, but I'm just pasting the checkMesh results here anyway: Code:
Overall domain bounding box (50 50 0) (50 50 0.001) Mesh has 2 geometric (nonempty/wedge) directions (1 1 0) Mesh has 2 solution (nonempty) directions (1 1 0) All edges aligned with or perpendicular to nonempty directions. Boundary openness (1.24534e21 4.7626e22 1.10569e14) OK. Max cell openness = 2.22691e12 OK. Max aspect ratio = 364.255 OK. Minimum face area = 4.61664e13. Maximum face area = 1.86996. Face area magnitudes OK. Min volume = 4.61664e16. Max volume = 0.00186996. Total volume = 7.85374. Cell volumes OK. Mesh nonorthogonality Max: 84.7881 average: 26.2456 *Number of severely nonorthogonal (> 70 degrees) faces: 6856. Nonorthogonality check OK. <<Writing 6856 nonorthogonal faces to set nonOrthoFaces Face pyramids OK. Max skewness = 3.29989 OK. Coupled point location match (average 0) OK. Any help is very much appreciated! Cheers 

November 20, 2016, 20:21 

#2 
New Member
Anonymous
Join Date: Apr 2016
Posts: 8
Rep Power: 6 
And here are the rest of the case files


November 20, 2016, 20:42 

#3 
Member
Join Date: Nov 2009
Posts: 56
Rep Power: 13 
When you ask questions it is always good to give as much relevant info as possible, here it would be nice to see an image of your domain with bc's.
You should try to reduce the number of nonorthogonal faces. Nonorthogonality over 80° can be troublesome. I looked at your p and U bc's and if this is an incompressible simulation, it is most stable to fix your outlet pressure and only fix velocity at the inlet. I am not sure what top and bottom patches are, but for an 2D external aerodynamic case I would use symmetry, slip etc.... Good luck. 

February 16, 2017, 10:04 

#4 
Senior Member
Peter Shi
Join Date: Feb 2017
Location: Davis
Posts: 102
Rep Power: 5 
Hello NRA,
Have you solved your problems yet? Since I met the same problems as yours, could you please tell me your solutions? I really appreciate it. I have emplyed kklomega turbulent transition model in OpenFOAM 4.0, our circumstance is quite similarafter certain number of iterations, my program crashes because the value of omega is too large. I am calculating mutielement 30p30n configuration, and the quality of my mesh is quite good. Thank you in advance. Best, Peter 

February 16, 2017, 15:29 

#5 
New Member
Anonymous
Join Date: Apr 2016
Posts: 8
Rep Power: 6 
Hi Peter,
I wouldn't exactly say I solved the problem since I ended up changing my project slightly and instead consider a NACA 0012 airfoil. Thus I was able to (after converting to OF mesh) use the PLOT3D meshes supplied at the NASA NACA 0012 case validation homepage: https://turbmodels.larc.nasa.gov/naca0012_grids.html I used the 449x129 one and was able to make the kkLOmega work which indicates that my original issue was probably related to grid quality. Furthermore, I also used a komega SST solution as initialization which was itself initialized with a Spalart Allmaras calculation. I'm sorry that I'm not able to be more helpful than this. Perhaps you could benefit from converting and inspecting some of the meshes in the above link (even though your geometry is different) and compare to your own. Best of luck! 

February 18, 2017, 03:58 

#6  
Senior Member
Peter Shi
Join Date: Feb 2017
Location: Davis
Posts: 102
Rep Power: 5 
Quote:
The way that initializing kklomega program by komegaSST did work. Thanks. However, the results of this model are less accurate compared to komegaSST, at least in my 30p30n mutielement flow simulation. How about yours? (The version of my OpenFOAM is 4.0, and previous versions have bugs regarding to this model) Best, Peter 

February 18, 2017, 08:15 

#7 
New Member
Anonymous
Join Date: Apr 2016
Posts: 8
Rep Power: 6 
Hi Peter,
Glad you achieved a solution with the kkLOmega. In my case the kkLOmega was also less accurate in terms of lift coefficient. The predicted value was a bit too high, especially for high angles of attack. For instance, I got something like Cl=2.1 for AoA=18 degrees where the komega SST did instead detect some stall as you would expect from looking at experimental data. However, the drag prediction was really very good for all my angles of attack (18 to 18), compared to experimental values with no boundary layer tripping. Here the komega SST yielded too high values which is of course the common problem with nontransition turbulence models. I ran OpenFOAM 3.0 and it was actually my understanding that the kkLOmega bugs was already solved in this version, but I'm not sure about this. 

February 18, 2017, 08:46 

#8  
Senior Member
Peter Shi
Join Date: Feb 2017
Location: Davis
Posts: 102
Rep Power: 5 
Quote:
Thanks for your information. It is a useful experience for me. Actually, I do not have drag data for my case, hence I am unsure about whether this model can produce reliable data for drag. At least, I've learned that kklomega tends to overestimate CL. To my knowledge, I remember I met a guy who was using OpenFOAM 3.0 and he posted a thread regarding to this new turbulent model. And he did mention that there were some bugs within this model. In fact, the authors of this model published a new paper to revise the original model just in 2016: Maurin Lopez. D. K. Walters. “Prediction of transitional and fully turbulent free shear flows using an alternative to the laminar kinetic energy approach”. Journal of Turbulence, Vol 17, Iss. 3, 2016. From the literature, the most popular transitional turbulent model is gamaRetheta. Unfortunately, this turbulent model is not included in OpenFOAM. However, some developers try to install this model by their own: http://www.tfd.chalmers.se/~hani/kur...transition.pdf And I followed the steps in the tutorial, but I failed to make it. If you have interests, you can look at it to see whether it will work. If it does work, please tell me! Thanks. Peter 

February 18, 2017, 09:38 

#9 
New Member
Anonymous
Join Date: Apr 2016
Posts: 8
Rep Power: 6 
Hi Peter,
Thanks for pointing that out, perhaps it's about time for me to update to 4.0. I am currently busy with some other projects but I would like to give the transitional SST model a go in the future, if I can manage to install it myself Or perhaps it will already have made it's way into the new OpenFOAM version by then. All the best 

February 18, 2017, 09:54 

#10  
Senior Member
Peter Shi
Join Date: Feb 2017
Location: Davis
Posts: 102
Rep Power: 5 
Quote:
All right, I hope so and good luck. Best regards, Peter 

Tags 
divergence, floating point exception, kkl, omega, simplefoam 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
overshooting of Omega in SST komega using simpleFoam  cm_jubayer  OpenFOAM  2  June 7, 2020 13:52 
PEMFC model with FLUENT  brahimchoice  FLUENT  22  April 19, 2020 16:44 
[ANSYS Meshing] Help with element size  sandri_92  ANSYS Meshing & Geometry  14  November 14, 2018 08:54 
fluent divergence for no reason  sufjanst  FLUENT  2  March 23, 2016 17:08 
Divergence problem  Smaras  FLUENT  13  February 21, 2013 06:03 