[Bernhard]

Dear all,

Let me make use of this new subforum to post a request here. I am not an OpenFOAM nor an LES expert by any means, but I am very interested in the stories of people that validated or benchmarked the LES models of OpenFOAM against DNS databases or other modelled results.

I think that it will be a waste of time when everybody does this him- or herself with the same repeated cases. I'd like to ask the people that have a ready-to-use test case somewhere on their desk to share their experiences (including case and results) with the community using this thread. I think a lot of people can benefit from all the efforts that has been put into it already.

Regards,
Bernhard

[eelcovv]

Hi Bernard,

Good initiative! There was a quite interesting thread already

LES of turbulent channel flows

But nevertheless, not all aspect have been covered yet. For instance, I would like to have some more information on LES wall functions. In the thread above, the complete boundary layer was resolved. My question is: can we get away with this by using appropriate wall functions ?

I did some tests with LES in the Moin and Kim channel (because the DNS data can be obtained from the internet), but I am really not happy with the result. I find that I can only get the pressure drop correct (I use the channelFoam trick, so I set the mass flow fixed by adjusting the pressure gradient) if I really resolve the wall boundary layer (fist grid point within one wall unit from the wall). I use the nuSgsUSpaldingWallFunction from OF 2.0.x, and in my understand it should be possible to put the first grid cell somewhere between 10 and 30 y+, but this yields a pressure drop which is too high.
Another trick I tried was to use grid refinement using snappyHex mesh. In that you you can easily double the grid resolution near the wall. However, at the transition from the refined layer to the course grid, the grid exapansion is almost a factor of 2, and this spoils the solution completely (in LES, ideally uniform grid must be used, or at least a very smoothly varying grid).

I could send in some more details, but I need to summarise my results a bit. I am curious if other users have experience in get a correct LES simulation of a channel using wall functions or grid refinement near the wall such that the total grid size remains within feasible limits (at least < 2 mlj cells).

Regards
Eelco

[timo_IHS]

Hallo Eelco,

I also tested the wall function of Spalding (different names in different OF-versions) for a RANS pipe flow with different y+-values (1-150). I also determined a too high pressure drop for y+-values of above approx. 10. I suppose there's the same problem in LES. Perhaps you or we can check this.

There are DNS-data for pipe flow from Eggels or Fukagata:
http://www.thtlab.t.u-tokyo.ac.jp/DNS/dns_database.html
The problem here is the small Re-number, so you almost have to stay in lowRe-regions, otherwise the core flow is not well resolved.

Best,
Timo

[eelcovv]

Hi Timo,

Thanks for the link, I didn't know this one. Very interesting for validating purpose.

I just send here two small examples of attemps of a channel LxHxB=6.4x1x1.6 at Re=Um*H/nu=29,000 by setting Um=0.3306 m/s with nu=1.14e-5 m2/s. Care was taken to get a fully developped flow. backward time integration with dt=0.01 s was used, leading to Co_max=0.75. Gauss linear interpolation was used for all matrix solvers, using GAMG with the residual set at 1e-7.

The expected pressure drop I estimated by using the relation
Ref=0.09*Re**0.88 (Pope), so the Reynolds number based on the friction velocity uf is 760. Using Ref=uf*wh/nu (wh=H/2) gives me uf=0.017 m/s. Finally, the pressure drop is obtained by gradP/rho=uf**2/wh=0.00060 m/s2.

Well, tested several turbulence models (smagorinsky, 1 equation eddy, DES), all with nuSgsUSpaldingWallFunction at the wall bc of nuSgs. Not much difference between the results for the different turbulence models The grid has actually the greatest impact on the results. I compare here for instance two grids: g0 and g1.

g0:
grid info: 2.1 mlj (256x128x64) cells created with blockmesh using a simpleGrading (1 10 1) at the walls (so two blocks where formed, just like channel395 from the tutorials).
yplus : 1.70512780145771
uf : 0.0195762739049085
gradP : 0.000766461

g3
grid info: 1.6 mlj cells. Course uniform grid (no simplegrading) was formed with blockMesh (100x50x30 cells) and refinement was made using snappyhexmesh (with a block near the wall with double refinement and a block in the log layer with a single refinement)
yplus : 0.719308714802291
gradP : 0.00102801
uf : 0.022671678367514

Pictures of the grids g0 and g3 together with their mean U profiles are included to this post. As you can see, the g0 performce best in terms of the presure gradient (and therefore the velocity profile), but the gradP=0.0007 I find is still 20% too high with respect to the value based on Popes relation So the refinement using snappyhex mesh is not applicable for LES I assume? Netherless, I would hope to get a bit better result then the plot I show using 2.1 mlj cell for g0.

Unfortunately I am occupied with other stuff right now so I don't have really time to find out how to improve my LES simulation of the channel. I am sure if I resolve the full boundary layerI get better results (in other posts on the forum with LES, the first grid point was at y+=0.2), but if you try to do that LES becomes almost as expensive as DNS. I don't see the point in using a wall function if you still have to put your first grid point within y+=1. Hopefully somebody could comment on that: am I doing something wrong? Or are there any alternatives beside Spalding ? Well, if somebody has obtained better results then I am showing here, I would be very interested in the settings.

Regards
Eelco

cav_g0_gridvelo_t00000.jpg

cav_g3_gridvelo_t00960.jpg

turbprofile-Umean.jpg

[bageshwar]

I have incorporated Smagorinky subgrid scale model in my code and now I want to validate it. I am looking for a Turbulent jet case with free shear flow, preferebly square jet. 3D. Can anyone help?

[atmcfd]

Bageshwar,

Couldn't find anything exact, but this might be a good reference. Look for other cases in this repository which might suit you.

http://qnet-ercoftac.cfms.org.uk/w/i...erexpanded_jet

Regards

Atm

[vonboett]

Hi all,

concerning LES of turbulent channel flow with wall functions, I follow currently the approach of hybrid URANS-LES for OpenFOAM developed at LeMoS at the University of Rostock. First results are promising, especially because the domain gets decomposed into URANS region and LES region dynamically dependend on local grid resolution and flow.
The idea is that one can model the turbulent flow field with complex surface structures on the channel bed that become URANS region, with wall functions this would not work I guess. Currently I simulate a 32 m long and 2 m wide paved channel of a natural torrent with 16 mio cells and results fit the overall behavior of the channel. As soon as we can get surface velocity measurements this summer this might turn into a validation test case, then it might be redone with hLES for comparison.

The other test case is a 6 m long flume, 0.3 m wide, with fixed gravel bed that find its way into the simulation by an .stl file from surface scan and snappyHexMesh. I would like to discuss that case because of the 'Lego-Brick' kind of representation of the gravel bed and because of the jump in mesh resolution from high resolution close to the gravel bed to coarse resolution above the gravel bed. Again, this test yust started and currently we compare travel times of spheres in the flume with simulated spheres using CFDEM-LIGGGHTS