Validation of LES models
 

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

Hi Bernard,

Good initiative! There was a quite interesting thread already

http://www.cfd-online.com/Forums/ope...nel-flows.html

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

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

some LES channel flow results with two different meshes
 

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

Attachment 9489

Attachment 9490

Attachment 9491

Validation of LES
 

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?

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

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

Validation of SGS models
 

It is very helpful.

Dear Ashvin Chaudhari, I am using pisoFoam with LES for channel flow, but for many days, can not get good velocity curve....really don't know where is wrong.
If it is possible, could you please, let me know some more details about your setting?
Thank you very much!!!! Waiting for your reply.
cheers

Thank u so much for the details, I will do some more investigations right now and let u know more details.
Thanks again!!!

...I guess the problem with your dynamic SGS has its origin in the wall boundary layer. Could you post at which y+ (resp. z+) position your wall-closest cell center is?
Yust being curious, could you rerun the case with dynOneEqEddy with mesh grading towards the wall such that your first cell center is at y+ of about 100? Keylock et al (2012) "The application of computational fluid dynamics to natural river channels: Eddy resolving versus mean flow approaches" suggests the first cell center to be within 30 to 300 wall units close to the wall if wall functions are used, and less than 4 wall units if no wall functions are used. I am not sure if dynamic procedure and wall functions can always be applied at the same time without conflict.

Of interest could be aswell: Notes on Numerical Fluid Mechanics and Multidisciplinary Design, Springer, Vol. 111, pp. 271-281, 2010: "Large Eddy Simulations: Wall Functions with
Forcing given by Backscatter from a
Scale-Similarity Model" in which the underprediction of resolved fluctuation of the wall shear stress in channel flow simulations with coarse wall region resolution and wall functions is adressed.

Thank you Albrecht for the comments .

Earlier I also used fine grid resolution so that the first cell-centre value z+(1) is between 30 and 100, but no improvement was seen. See the attached result, the z+(1) is around 40 and using dynOneEq sgs model result is not good.

I will repeat the similar case with dynOneEqEddy model but for closed channel flow. I will post the results. Reason is that so far i didn't try any dynamic models for closed channel flow, basically I don't want to use symmetryPlane bc on top of my domain so the closed channel flow would be good testing.

Initially, I was suspecting this one, but later I saw several papers written for Atmospheric Boundary Layer flows over flat and smooth terrains. They all used wall-function and also for such a flow, the sgs model play an important role. There were some nice results using dynamic Lagrangian sgs model too. In fact, dynamic Lagrangian sgs model can be good choice for the ABL flow over the complex terrain due to its unique time-averaging approach for the model constant. This is the reason I want to use dynamic sgs model.

Thanks for the references. I will look them and try to post the results for closed channel flow simulation using dynOneEqEddy model.

Hello
I am to run channel flow with dynSmagorinsky(channel395), but my statistics are not in good agreement with Moser DNS(Retau=395)
Dimesion of my domain is : 4*2*2,80*50*60
I run te simulation for long time . After the initial peaks in turbulent kinetic energy the energy fluctuates around a value. After that I run a long simulation and perform average.

1. vrms , wrms are underestimated.
2. urms is overestimated .
3. Uf.xy is also not matching far from the wall.

the schemes of my channel:


ddtSchemes
{
default backward;
}

gradSchemes
{
default Gauss linear;
grad Gauss linear;
grad Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss linear;
div(phi,k) Gauss limitedLinear 1;
div(phi,B) Gauss limitedLinear 1;
div Gauss linear;
div(phi,nuTilda) Gauss limitedLinear 1;
div((nuEff*dev(grad .T()))) Gauss linear;
}

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A ),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DBEff,B) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

interpolationSchemes
{
default linear;
interpolate linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

I use delta cubeRootVol; Same issue I have with static Smagorinsky model also.
Please see my results

Thankyou

How about dynOneEqEddy? Note that dynSmagorinsky only adjusts the model constant in dependency to the overall flow, so you will not get a local adjustment.

Hi,
OneEqEddy sgs model will be fine to bring good agreement for the LES-channel flow case at least. In your case, i think the grid is too coarse. I will suggest you to use finer grid resolution where first y+ is about 0.5 in wall-normal direction for both upper and lower walls. So please use finer grid such as 80 x 160 X 80 for the domain 4x2x2 in x, y and z directions, where y is wall-normal direction.

Also, you are using limitedLinear scheme, so use only the linear scheme for the "divSchemes", i.e.

laplacianSchemes, gradSchemes and ddtSchemes are fine. Use pisoFoam and oneEqEddy model with delta=vanDriest. Run the simulation with low Courant number, i.e. CoMax<0.3.

Good luck !

-- Ashvin

Hello, Ashvin,
Thanks for your suggestion. I have used 40*160*40 points . But still I dont see any improvement. I will update my divergence scheme and run the simulation for higher resolution. Actually I would like to validate static Smagorinsky model. But I first started with dynamic one . Dynamic model results are much better than tha static one. Using static smag is specific to my problem else I would have used OneEqEddy sgs model :(.

Dear subhendu,
I'm simulating a channel-DNS case, I 'm also a newer of OF. Did you get the curves of urms,vrms using postChannel? and do you know how urms et al is calculated in OF?

Thanks!

Hi,Ashvin Chaudhari:
I'm curious about the differences between RK-4 method and the built-in second order time integration. In your case, did you see some significant differences between the two schemes? I recently ran a rotating channel flow and found the Uf differ from DNS in the region far from the wall. However, the result is fine when no rotation is imposed. I would like to know if the schemes can cause this problem

Xianbei

Hi Xianbei,

Sorry for my late reply. I just noticed it now.

Sure, we have made some comparison between the two solvers: rk4+projection and pisoFoam. I would encourage you to look the following two papers in order to see/learn the differences between RK-4 method and the built-in second order time integration.

1) http://www.sciencedirect.com/science...45793014000334
2) http://www.sciencedirect.com/science...65997814001513

- Ashvin

Hi ashvin,

Can u help me to run dynamicLagrangian SGS model ? I run my case but facing following error :

--> FOAM FATAL ERROR:
incompatible dimensions for operation
[flm[0 4 -5 0 0 0 0] ] + [flm[1 1 -5 0 0 0 0] ]

From function checkMethod(const fvMatrix<Type>&, const fvMatrix<Type>&)
in file /mnt/home/SW/CFDSupportFOAM3.0/OpenFOAM-3.0.x/src/finiteVolume/lnInclude/fvMatrix.C at line 1295.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::fvMatrix<double> const&, char const*) at ??:?
#3 Foam::tmp<Foam::fvMatrix<double> > Foam::operator+<double>(Foam::tmp<Foam::fvMatrix<d ouble> > const&, Foam::tmp<Foam::fvMatrix<double> > const&) at ??:?
#4 Foam::LESModels::dynamicLagrangian<Foam::EddyDiffu sivity<Foam::ThermalDiffusivity<Foam::Compressible TurbulenceModel<Foam::fluidThermo> > > >::correct() at ??:?
#5 ? at ??:?
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7 ? at ??:?
Aborted (core dumped)

If u can help, it will be great for my work.

Validation of pressure-incremental projection scheme + dynLagrangian model
 

Hi guys,

I just saw your discussion and I wanted to put my 2 cents on the issue. For the last month I have developed a projection method similar (see Guermond&Shen) to that of Chaudhari for the incompressible N-S equations, and as validation I run the classic channel flows with different Re. The difference of my case with oodlesChannel (or channel365) is that I drive my flow using a certain pressure gradient, not by setting some flow.

Additionally, with the risk of sparking a salty debate, its my opinion that whenever you run openFOAM without any turbulence model you should not call your results 'DNS' but more 'NO-MODEL LES'. This given the 2nd-order FV nature of the library itself, and the boundary conditions that you can impose. In fact, calling 'cyclic' boundary conditions 'periodic' carries a promise that the developers where well aware of and thus decided to call them as the former.

In any case, you'll find attached the velocity profiles and RMS of channel flows run using Re_tau=171 and Re_tau=410. In both the dynamic lagrangian model of Meneveau was used. In general results seem decent.

Tahnk you, that really helps!

Hi Santiago,
I am trying to use the dynamic Lagrangian model of Meneveau(1996) for reacting flows, but somehow for me the flm and fmm values become unbounded at some later stage during the simulation and the Co shoots above 1 and time steps sturuggles to maintain the maxCo and crashes finally. This however is not to be the case with Smagorinksy model.
I am using the IC of flm and fmm form Meneveau(1996) and BC as zero gradient. The flow a is free shear jet flow. I am using `backward` scheme time differencing and `linear` spatial discretisation schems with maxCo 0.35. The mesh is fully structured with max aspect ratio of 15 and max non-orthogonality of 18.

It will be beneficial for the CFD community if you could kindly share the setup values i.e. IC, BC of flm and fmm and the fvSchmes for the dynLag case.


Thanks

The boundary condition you set (zeroGradient) for flm is not correct, if there's a wall. One question: What is flm? is an integral of Lij*Mij. How Lij behaves at a wall? Must be zero, by definition. Hence, flm is *zero* at a wall. In general, there is no "rule" on how to define flm/fmm, it's case dependent. I suggest you to start from the definition of the variables themselves.

Another thing: The dynLagrangian Smagorinsky model implemented in OF (whichever version, fork, etc) is not consistent at the test filter level, thus the results obtained are not going to be "correct". I recently published an article discussing this issue:

https://www.mdpi.com/2311-5521/4/3/171

Cheers,

S

PS.: Initial conditions for a channel flow? A TS wave (doesn't matter the dimensionality). Set-up? Gauss linear all the way. Time? Not Euler.

Hi Santiago,
Thanks for the reply.
1.For my case, it is a jet flow with no walls. Hence I set the values to ZeroGradient. I hope it is correct?
2. The inlet BC for velocity is derived from a precursor pipe flow simulation.
The IC for flm and fmm are based on Meneveau(1996) so that Cs=0.16 initially.
3. Time Scheme: backward Convection: U->linear, flm,fmm->limitedLinear 1.0.
4. fvSolution(flm,fmm)->PBiCG(DILU)

Somehow, I feel that the setup is very unstable as it caused the fmm value to explode somewhere in between the simulation. Is there something incorrect?
Thanks in advance!

From the precursor flow you should be able to determine flm and fmm. For the slip conditions flm/fmm may be zeroGradient. for the solution of the equations put upwind/euler, as you want everthing to be bounded. Notice that meneveau also does upwinding in time, given that flm/fmm are integrated along flow trajectories. Notice that the clipping done by openfoam is "wrong", since the clipping should be made to the source term of the transport equations, via a heaveside function.

Hi Santiago,
About the inconsistency you mentioned for the test filter, can't we use the Laplace test filter( or anisotropic filter) implemented in OF? I understand that the grid level filtering is implicit but for test filter may be specified explicitly as Simple/anisotropic/Laplace. Will it still not give "correct" the results as you have achieve in your article using a Laplace test filter?

Well, the anisotropic filter is the only valid (strictly speaking) explicit filter for hexahedral, non uniform grids. And no, using the anisotropic filter does not resolve the inconsistency I refer to when using the dynamic smagorinsky models.