CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Too much turbulence (http://www.cfd-online.com/Forums/openfoam-solving/60234-too-much-turbulence.html)

andimb March 20, 2006 09:39

Hi! I'm still calculating a
 
Hi!

I'm still calculating a flow around a NACA airfoil and compare it to a CFX solution.
I use the LaunderSharmaKE turbulence model with an yplus near 1.
If I start a calculation with the same boundary condiations as in CFX, where epsilon is calculated by epsilon = density*C_mu*k^2/eta_T and eta_T=10*eta where eta is the dynamic viscoity, the solver reaches no steady solution, seen in the first image. http://www.cfd-online.com/OpenFOAM_D...ges/1/1981.jpg

If I use the following formulationfor epsilon: epsilon = k^(3/2)/L with L as an charactersitic length as the chordlength, I get a much lower epsilon and the solution is steady but with a too big boundary layer ass seen in the picture.
http://www.cfd-online.com/OpenFOAM_D...ges/1/1982.jpg

I also try other turbulence models and guessed epsilons and finer or coarser meshes, with no dramatic change.

I don't see the mistake I make.

Thanks for help!
Andreas

pierre March 20, 2006 10:31

Are the numerical set-up ident
 
Are the numerical set-up identical in both CFX and Foam?

Pierre

andimb March 20, 2006 10:45

Hi! I think completly ident
 
Hi!

I think completly identical is not possible. I used the Hiresolution scheme in CFX which, as I understood, should be equal to the gamma scheme in OpenFOAM.
So it should be equal.
You just have not as much possibilities to choose in CFX as in OpenFOAM. And you need something better than upwind to get right results.

Andreas

andimb March 21, 2006 12:02

Hi! I tried the easiest cas
 
Hi!

I tried the easiest case I can think of with simpleFoam. Coarse mesh with no turbulence model (exactly laminar dummy model) and upwind scheme where possible.
There are still seperation bubbles. Perhaps the boundary consditions are wrong but I don't know which?

Perhaps someone can help me.

http://www.cfd-online.com/OpenFOAM_D...ges/1/1997.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/1998.jpg

Thanks
Andreas

andimb March 21, 2006 12:07

Hi, again! I use an own wri
 
Hi, again!

I use an own written mesh generator. I just give the profil coordinates and the mesh is autogenerated. Perhaps there is something wrong. But checkMesh doesn't throw any error.

Andreas

pierre March 21, 2006 14:33

I recall that I had something
 
I recall that I had something similar early on in my PhD, i.e. my calculation would always show behaviour that looked physical to a point but not what was wanted. eventually it was due to the fact that my generated mesh had inconsistent coordinates (I can't recall if i had used checkMesh to verify ny mesh). In the blockMesh I had messed up some of the points ordering. I don't if that helps. I have you tried to look at the mass continuity, not just locally but what come in and out of the domain.
I am not sure whether that helps.

Pierre

andimb March 22, 2006 09:14

Hi! I checked the mass cont
 
Hi!

I checked the mass continuity, but everthing is like it should be. And I checked the mesh by hand and found no mistake.

Andreas

eugene March 22, 2006 09:42

What is your boundary conditio
 
What is your boundary condition for k and epsilon?
If it is zero gradient, that might be your problem. For low Re models, the BC should be "fixedValue" with the value set to some small non-zero number e.g. 1e-10;

andimb March 22, 2006 09:53

Hi! First I want to thank y
 
Hi!

First I want to thank you all for your help!!

Yes, the boundary conditions were zero gradient, so I'll try fixed value. But why could this matter with turbulence model laminar? k and epsilon won't be calculated, right?
This was the reason I did the run laminar, to check if the turbulence boundary conditions are a problem.

Andreas

eugene March 22, 2006 10:08

Laminar flow seperates easier
 
Laminar flow seperates easier than turbulent flow. Have you run laminar using a different solver?

andimb March 22, 2006 14:42

Hi! I tried a run with the
 
Hi!

I tried a run with the "fixed value" boundary conditions. But there was no difference.

So I did a calculation with 0 angle of attack. Even there the flow "seperates", means there is an subboundary layer with goes the other way. I made a picture to show.

http://www.cfd-online.com/OpenFOAM_D...ges/1/2010.jpg

I did a laminar run with simpleFoam and icoFoam.

Andreas

hartinger March 23, 2006 11:31

Hey Andreas, Are you sure,
 
Hey Andreas,

Are you sure, that the flow shouldn't seperate.
I mean, why not?

markus

eugene March 23, 2006 12:59

By different solver, I meant o
 
By different solver, I meant other than OpenFOAM.

Laminar flow seperates very easily so the laminar seperation results might be correct. For instance, on a cylinder you get seperation quite early before 90 deg if the flow is laminar.

Turbulent seperation is probably wrong. Have you rerun the turbulent case with small fixedValue BCs for k and epsilon?

Also, give the SpalartAllmaras model with nuTilda fixedValue 0 on the wall a try. As far as I know it is one of the better turbulence models for wings.

andimb March 24, 2006 06:33

Hi! I think, I've got the p
 
Hi!

I think, I've got the problem now.

As I wrote in the start post, I used two definitions of epsilon at the inlet. The first one gave a small and the second (CFX) a great epsilon. As I understood a large epsilon means nearly laminar calculation because all turbulent energy dissipates to velocity. In the OpenFOAM formulation this is just a wrong value of epsilon and that's why the calculation shows a laminar behaviour.

So I have to use the "small" epsilon. There is the problem of the "stagnation point anomaly", which is an overpredicition of turbulent energy at stagnation points in k-epsilon models. The only High-Re models that doesn't have this problem are the "LRR" and the "NonlinearKEShih" turbulence models. They have another formulation of the production term. But as I said and you know, they are High-Re models. There is no low-Re model without this problem.
This overprediction causes the huge boundary layer over the profile and as a consequence of this to less velocity.

But there is still the question why CFX didn't have these problem. They use a scalable wallfunction for some of there turbulence models. So as a consequence they are not as yPlus sensitive as a normal formulations. When I used the standard wallfunction CFX has the same Problems.
And this was the point I wasn't able to see. There boundary contitions are not portable to OpenFOAM, because of the differnce in the wall function theory.

So there is the posibility of the Kato Launder modification of k-epsilon models, that should solve the "stagnation point anomaly". It's an reformulation of the turbulent production.

A laminar run with CFX gave the same results as OpenFOAM. So it's ok.

The fixedValue run gave the same results as the zeroGradient with the right epsilon at the inlet.

So if I don't want to change stuff in the code, I have to live with a too low lift and too high drag. But this is ok as long as I know why this is happening.

As far as I know the Spalart Allmaras model give a good lift prediction but also too high drag (drag is a near wall problem, so you need a good describtion what is happening there). But I'll try, because it is easier and perhaps give better results.

I really want to thank you for your help. This is a great forum with great guys, who want to help.

Please tell me, if I understood something wrong or desripted wrong.

Andreas

hjasak March 24, 2006 06:48

Well, if it is the stagnation
 
Well, if it is the stagnation point anomaly that's giving you trouble, try using the high-Re RNG k-epsilon: that should do a better job.

If you are set on Kato-Launder, its implementation in OpenFOAM is (almost) trivial: copy k-epsilon, rename the files and class names and change the form of the generation term to use grad U - grad U^T and you're done (it would be worth checking my words in the original reference though).

As for the results by CFX, I would consider it a distinct possibility that they have messed about with the k-epsilon model (to deal with the kind of problem you are seeing) without giving you chapter and verse of what they have done. As you know, CFX have got a very competent guy leading the turbulence work (Dr. Florian Menter) and it would be by no means unusual to do this kind of thing. A correction could be done in several places and you will probably find a brief comment about it somewhere in the documentation if you look closely.

Finally, I can tell you that the k-epsilon implementation in OpenFOAM is strictly "by the book" in all the details including the wall functions, which you can easily check by inspecting the source.

Enjoy,

Hrv

kumar2 May 2, 2006 04:43

Hi Eugene & Andreas, i am m
 
Hi Eugene & Andreas,

i am modeling flow over a NACA12 hydrofoil at 5 deg at Re about 10^5 . when i used a k-epsilon i got results similar to klaus wittig ( please search with naca23012 + klaus , for his results - basically the stagnation point cp is larger than 1 and the suction peak is underpredicted ) . when i chose the launderSharma low Reynolds number i got results similar to Andreas.

Prediction of lift is very important in my case since the free surface charecteristics is affected by the suction . so i would like to use the spalartAllmaras turb.model .

Eugene has mentioned that the boundary condition for nuTilda is fixedValue 0 on the wall . isn't the turbulence model used as a low Re model in this case ? is the yplus < approx 5 in this case ? is the physicalType of wall wall & ( not wallFunctions )? If i use the model as a high Re case will the nuTilda be zeroGradient on the wall and the physicalType of wall wallFunctions ? if i know the inlet velocity , what is a quick way of guessing nuTilda at inlet ?

Andreas , did you try out with the spalartAllmaras model and what was your experiance ?

Thanks a lot
Regards
Kumar

kumar2 May 2, 2006 04:57

Hi Eugene & Andreas, i am m
 
Hi Eugene & Andreas,

i am modeling flow over a NACA12 hydrofoil at 5 deg at Re about 10^5 . when i used a k-epsilon i got results similar to klaus wittig ( please search with naca23012 + klaus , for his results - basically the stagnation point cp is larger than 1 and the suction peak is underpredicted ) . when i chose the launderSharma low Reynolds number i got results similar to Andreas.

Prediction of lift is very important in my case since the free surface charecteristics is affected by the suction . so i would like to use the spalartAllmaras turb.model .

Eugene has mentioned that the boundary condition for nuTilda is fixedValue 0 on the wall . isn't the turbulence model used as a low Re model in this case ? is the yplus < approx 5 in this case ? is the physicalType of wall wall & ( not wallFunctions )? If i use the model as a high Re case will the nuTilda be zeroGradient on the wall and the physicalType of wall wallFunctions ? if i know the inlet velocity , what is a quick way of guessing nuTilda at inlet ?

Andreas , did you try out with the spalartAllmaras model and what was your experiance ?

Thanks a lot
Regards
Kumar

andimb May 3, 2006 12:21

Hi Kumar, the SpalartAllmar
 
Hi Kumar,

the SpalartAllmaras model did a good job. The lift prediction was ok.

As far as I understood the SpalartAllmaras model, it is like a low-Re formulation. The formulation has no real Re-limits.

The boundary conditions are fixedValue 0 at walls and nuTilda=0.1*nu at inlets.

Andreas

kumar2 May 3, 2006 16:45

Hi Andreas Thanks a lot for
 
Hi Andreas

Thanks a lot for the information . i am also going to try out the spalartAllmaras turb.model on my naca12 wing. ( i also started with the standard k-epsilon , then RNG kepsilon , then a low re launderSharma ... and my experiances were very similar to yours )

thanks again for sharing your experiances

regards

kumar


All times are GMT -4. The time now is 07:37.