CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   kklOmega SimpleFoam divergence, kt kl omega (https://www.cfd-online.com/Forums/openfoam-solving/180292-kklomega-simplefoam-divergence-kt-kl-omega.html)

NRA November 20, 2016 20:19

kklOmega SimpleFoam divergence, kt kl omega
 
5 Attachment(s)
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 5-25 iterations.

For meshing I have used this mesher: http://hvirvel.dk/airfoilmesher/

I generates a circular domain and an o-grid 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 (non-empty/wedge) directions (1 1 0)
    Mesh has 2 solution (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (1.24534e-21 -4.7626e-22 1.10569e-14) OK.
    Max cell openness = 2.22691e-12 OK.
    Max aspect ratio = 364.255 OK.
    Minimum face area = 4.61664e-13. Maximum face area = 1.86996.  Face area magnitudes OK.
    Min volume = 4.61664e-16. Max volume = 0.00186996.  Total volume = 7.85374.  Cell volumes OK.
    Mesh non-orthogonality Max: 84.7881 average: 26.2456
  *Number of severely non-orthogonal (> 70 degrees) faces: 6856.
    Non-orthogonality check OK.
  <<Writing 6856 non-orthogonal faces to set nonOrthoFaces
    Face pyramids OK.
    Max skewness = 3.29989 OK.
    Coupled point location match (average 0) OK.

Does anyone have any suggestions as to what is causing these divergence problems? I suspect it is mesh related but I am not sure how to determine which improvements I need to make (if possible). I have also attached the case files since these could also very well be causing trouble.

Any help is very much appreciated!

Cheers

NRA November 20, 2016 20:21

4 Attachment(s)
And here are the rest of the case files

fusij November 20, 2016 20:42

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 non-orthogonal faces. Non-orthogonality 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.

PeterShi February 16, 2017 10:04

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 similar-after certain number of iterations, my program crashes because the value of omega is too large.

I am calculating muti-element 30p30n configuration, and the quality of my mesh is quite good.

Thank you in advance.

Best,
Peter

NRA February 16, 2017 15:29

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 k-omega 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!

PeterShi February 18, 2017 03:58

Quote:

Originally Posted by NRA (Post 637446)
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 k-omega 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!

Hello NRA,

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 muti-element flow simulation.

How about yours? (The version of my OpenFOAM is 4.0, and previous versions have bugs regarding to this model)

Best,
Peter

NRA February 18, 2017 08:15

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 k-omega 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 k-omega SST yielded too high values which is of course the common problem with non-transition 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.

PeterShi February 18, 2017 08:46

Quote:

Originally Posted by NRA (Post 637595)
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 k-omega 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 k-omega SST yielded too high values which is of course the common problem with non-transition 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.

Hello NRA,

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 gama-Retheta. 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

NRA February 18, 2017 09:38

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

PeterShi February 18, 2017 09:54

Quote:

Originally Posted by NRA (Post 637599)
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

Hi NRA,

All right, I hope so and good luck.

Best regards,
Peter


All times are GMT -4. The time now is 00:49.