[Flowkersma]

Hello everyone,

I'm trying to validate my impinging jet simulation with v2f model by comparing it with the ERCOFTAC experimental results. Behnia et al. has already made simulations with v2f and the agreement of their simulation with the experiment is excellent. In my simulation I get too high turbulence kinetic energy close to the stagnation region.

Geometry and boundary conditions are given in Figure geom.png. I have done mesh independence studies and the first cell wall distance is below one everywhere (y+<1 ). I use mapped inlet boundary condition which develops a fully developed turbulent inflow. The velocity profile and the turbulence quantities seem to have reasonable values at the inlet. The boundary conditions for the walls are following (in brackets different combinations which I have tried):

k fixedValue 1e-10 (kLowReWallFunction)
epsilon lowReWallFunction (groovyBC 2*nu*internalField(k)/sqr(mag(delta())))
v2 fixedValue 1e-10 (v2WallFunction)
f fixedValue 0 (fWallFunction)
nut nutUWallFunction (nutLowReWallFunction, fixedValue 0)

I'm running the simulation as steady state and I have verified that the results are converged. The turbulence kinetic energy contours with v2f and kOmegaSST models are given in Figure KE.png. The velocity and Nusselt number comparison with the experiment are given in Figures U.png and Nusselt.png. The agreement between the v2f model and the experiment is much worse than in the simulation by Behnia et al. (See Figures 4, 5 and 6 in their paper). In my simulation the high turbulence kinetic energy with v2f results in high nut and alphat and therefore the wall heat transfer is too high close to the stagnation. I get much better results with kOmegaSST than with v2f which is not expected. Any suggestions how to improve the results are highly appreciated.

Regards,
Mikko

[canopus]

Hi You can find the suggested combination of Wall Boundary conditions in v2f.H
alongwith nut as -

k       = kLowReWallFunction                                        
epsilon = epsilonLowReWallFunction
v2      = v2WallFunction                                        
f       = fWallFunction

But i think this might also not work!

Can you try the following for wall ?

k fixedValue uniform 1e-10
epsilon zeroGradient
v2 fixedValue uniform 1e-10
f   fixedValue uniform 1e-10
nut nutLowReWallFunction uniform 0

[Flowkersma]

Thank you for the suggestion! Unfortunately it didn't improve the results. I'm already wondering if there's something wrong with the v2f implementation? I compared the basic channel flow with an experiment and got quite good results. I can't say the same about this impinging jet.

[canopus]

Ok. I got closest with

epsilon = zerogradient

though not very good results while simulating asymmetric diffuser.
What schemes do you use for div?

[michele]

Hello,
I'm the original implementer of the v2f (or, better, it can be called "zeta2f", with some modifications popular about 10 years ago) model in OpenFOAM. I left the code to the community and, after some time, it was incorporated in the official release.
I explicitly tested it against the asymmetric diffuser, and v2f provided good results.
It may be of interest to you to study the configuration (and the sources I provided, for checking if in the meantime something was changed in the code).
In the link below you may find some info (and in the thread I provided some more details)

http://www.cfd-online.com/Forums/ope...tml#post192451

Hope this helps

[canopus]

Dear Michele
Thanks for the link. Could it be possible to post the polymesh files to try
a comparison?
I am not sure but the current implementation maybe from someone else.
Further to my understanding the current model even works for y+ > 1 .

[Flowkersma]

Hi,

Actually, I downloaded an OpenFOAM impinging jet case folder with results from somewhere (sorry cannot find it anymore). The simulation has been carried out with DurbinV2f (RASProperties) and the results seem much better. I guess that this is the model that you Michele originally have implemented and I think that the results are quite different compared to the present v2f model in OpenFOAM. Unfortunately, I haven't managed to port your version to the latest OpenFOAM. If you have it I would be very grateful if you could share it.

[michele]

@SM: sorry the case is really old, I don't remember where the mesh could be.
Alberto Passalacqua indeed asked to me permission to review and submit the code I delivered. From what I know, he made some modifications (not under my review). I'm happy that this code is now included in OpenFOAM, but I never tested it (I switched to other formulations when I need the elliptic relaxation...)
The new model has indeed the possibility to work for y+>1 via universal wall functions. In this case you should be aware that, in my opinion, it becomes questionable a 4-equations model (the effects of elliptic relaxation may be lost). In an industrial case, where you may be interested in specific regions, a multi y+ mesh (with y+<1 only where interested) could be however a huge benefit.
In benchmarks like the ones you are discussing I strongly suggest to keep y+<1.

@mikko: I switched to other formulations when I need the elliptic relaxation. For the record, at the moment I'm pretty happy with is this one:
Billard, Laurence: "A robust k-eps-v2/k elliptic blending turbulence model with improved prediction..." Journal of Heat and Fluid Flow

[chku24]

Hello Mikko,

I'm working on impinging jet and my numerical results are not good comparing to experimental data. You can see my results on the following links : http://www.cfd-online.com/Forums/ope...t-results.html

Could you please send me your set up files ?

Regards,
Christian

[The_seeker]

@Mikko,
Were you able to find the suitable boundary conditions for jet impingement. Setting very low fixed values near the wall is not giving correct results because after few iterations, the values of v2 and k residual drop to order of -6 and there is no change in k but the velocity profile changes.

[Flowkersma]

Hi,


I could not get acceptable results with v2f model when I tried it more than 5 years ago. Maybe I had something wrong in my setup or OpenFOAM has/had a bug.

[The_seeker]

Thank you very much for your quick response. I am also trying to see if there is original v2f model by Durbin available for compilation but I guess there is only modified version.