[cedric_duprat]

Hi OpenFOAM, in particular LES players,

I want to start a new thread about LES channel flow. There is already one but in OpenFOAM-Bugs and here there are no bugs.

The problem here is that I can't get "good" results for a channel flow with OpenFOAM. statistics are not so good and the same for the mean flow.

configuration : I want to validate OpenFOAM from Moser DNS (Retau = 395). This test case was used prveviously by Eugene in his Ph'D and Henry and Gavin in the conference (LES of turbulent channel flows). OpenFOAM "has been" validated in LES with this litterature.
the size of my channel is 2Pi*2*Pi with 96*196*69 node (which is huge).
I'm using the one transport equation for the turbulent kinetic energy (like Eugene's calculation) and it's refered to the B1 models in the paper from Gavin and Henry.

Here are the plots, the mean flow in normal scale then in log scale and then rms values:




You can see from the second picture the mesh which is correct (y+ = 0.11) and I've more than 10 nodes in the viscous area.
So in normal scale, I thing I've the same as the paper (for statistic also) but, in log scale there is a "big" difference when we compared to the DNS calculation.
The rms value are also not realy efficient.
Are these differences due to second order scheme ?
Are these differences due to SGS model ? (I didn't find in the litterature validations for this model in channel flow)

In Gavin and Henry's paper, dynamic models do not improve the results. So my question are:

- Can I have better results in LES with OpenFOAM ?
- Someone has results for a such case?

Thank you for giving your point of view about these calculations.

Cedric

[fugu]

Not sure about the symbols in your plots Uf_0, Uf_2 etc.

If you calculate the Reynolds stresses from the resolved field you are missing the sgs part so my guess would be that you are not going to match DNS values even if everything works fine.

Could you give more details on the B1 model?
Luca

[kumar2]

Hi Cedric,

The difference between the DNS and OpenFOAM result is "big" in the near wall region or the region where the viscosity plays an important role. (y+ < 10). I also got similar results in this region.

But in the region where it matters (y+ 100 - 1000), your results are very good. your slope is (1/0.41) and your constant appears to be very close to what you would get from the DNS calculation.

I see that you have indeed used a large number of cells , 1.3 million. how many cells have Moser et.al used ? for example kim et al used 3.2 million cells in their 1987 smooth wall computation for a Re_tau of 180! . so i think your result is different in the laminar region because it is still unresolved.

what is the time that you take for one flow time in your openfoam LES calculation. ( if flow time is [half of depth of channel/u_tau ] )?

I also did the smooth wall case with my LES solver. if you want i can post it.

Thanks

Kumar

[cedric_duprat]

Thank you for your answers,

@Luca : the only difference between Uf_0 and Uf_2 is the mesh repartition normal to the wall. one is linear and the other is a tanh. But, because in the plots only Uf_2 is symboled (by cross) you won't see the mesh. And in fact, as you can see, the results is the same. then, you have the classic log law and the linear law close to the wall. These last 2 law are the "asymptotic solution" in visous and inertial layer.

for B1 model, I can write you here all the theory but, I think it's better for you to find the reference LES paper in OpenFOAM. For exemple, "Large Eddy Simulation of Turbulent Channel Flows" from C. Fureby, A.D. Grosman, G. Tabor, H.G.Weller . You can find it for free from google. Eugene Ph'D is also very well written and explained the SGS models very clearly. Then you can have a look about Tabor (Gavin) and Fureby who did lot's of work on LES model (in particular OF's LES model).

About your comments, I calculated Re stresses from the resolved field but, the SGS model play as a viscosity in this field (and in the NS equations) so I'm suppose to see it there. don't I ?

@Kumar: I can't find Moser's paper now but, you are right, he probably used more cells but .... he did a DNS :-).
And I wall normal direction, plots show us (from y+) that ... it's resolved at the wall, doesn't it ? Then, conference paper (where the results are "better") obtained good results if
delta x+ = 35
delta z+ = 20
delta y+ between (2,20) without any wall model ...

In my case, utau = 0.0079
yes, I'll be gratefull if you can post here or send by mail your LES results with some description.

Thanks for giving idea, I'll keep looking for .... something :o)

Cedric

[fugu]

Cedric,
I see now you are underpredicting U mean in the viscous and transition layer and on the other hand overpredicting Urms.
If you calculate the Urms on a resolved LES field
it should be less than the corresponding DNS value
since you are missing the small scale motions whose dissipation is taken into account by the SGS model.
However this is not your case since you are actually overpredicting Urms.
I'll try to look at the paper to get more info on the SGS model.
One thing you can try is to run a different geometry and compare to more data.
I would try the Lid Driven cavity flow.

Best

[eugene]

I assume all your configuration settings are identical to those in the channel395 channelOodles tutorial case?

[cedric_duprat]

Hi Eugene,

euh ....not really :o)

As I told, the geometry and the grid are different. it's the same geometry as the DNS calculation. So streaks are shorter than the box and there is (should be) no effect from the outlet on the inlet.

the time discretisation is Crank-Nicholson. (I think it's backward in the tutorial).
For the numerical scheme I using only central diffential scheme (to keep second order accurate).
so there is no limitedLinear 1 for these terms (div(phi,k), div(phi,B))
Then, the time step is different to keep Co number less than 0.4.
For the solver, I'm using ICCG to solve the pressure (and the same PISO as the tutorial) and BICCG for the other quantities, which is quite different from the tutorial also.

Can these settings bring me some over diffusive terms, because, it should not, contrary to the tutorial (convective scheme view).

Thank you for giving advise,... I hope it's not a stupid question. But, because the results are not so "bad" (but also not so good :o) ), I think it's just a small things.


Cedric

[sega]

Originally Posted by cedric_duprat

the time discretisation is Crank-Nicholson. (I think it's backward in the tutorial).
For the numerical scheme I using only central diffential scheme (to keep second order accurate).
so there is no limitedLinear 1 for these terms (div(phi,k), div(phi,B))
Then, the time step is different to keep Co number less than 0.4.
For the solver, I'm using ICCG to solve the pressure (and the same PISO as the tutorial) and BICCG for the other quantities, which is quite different from the tutorial also.

Dear Cedric.

You say you are NOT using limitedLinear 1 for the two terms mentioned.
Can you tell me which one you are using?
Ore actually post your fvSchemes dictionary?

I'm having some problem using oneEqEddy in a square duct LES.
My results are poor and Smagorinsky is far better ...
I don't think thats correct ...

Have a nice day. Sebastian

[sega]

Hello World.

As mentioned above I am doing the channel flow simulation in a square duct with cyclic bc's for in- and outflow.
My Resolution is 56x56x70 with refined mesh towards the wall so there are 7 cells within y+ < 10.

I'm using two different LES models, namely

• Smagorinsky (SMG)
• One Equation Eddy

with two different filter-widths (Delta) each time, namely

• Cube Root Volume (CRV)
• van Driest Damping

Well, the results with Smagorinsky are looking more or less good, the results with the One Equation Eddy are scrap.

I'm even experiencing that the velocity profile is not symmetric.
Unfortunately the asymmetry looks to be getting worse when simulation longer and thus doing longer averaging.

Important information on how these plots are obtained: I'm using my own post-processing tool for averaging in the flow-direction (with MATLAB). I'm not primary doubting my own tool, but is there an OpenFOAM tool for post-processing a square duct channel?

Any ideas why the One Equation model is so bad compared to both DNS and Smagorinsky? Well, I expected vice versa.

[And]

Hi OpenFOAM channel flow community,

I'm working on LES of turbulent channel flow and so I'm deeply interested in your discussions and in particular on the validation on the OpenFOAM results.

As I'm concerned in the study of both spatial than temporal discretizations OpenFOAM schemes for LES, my doubt is if selecting the flag CrankNicholson in ddt schemes would mean the correct use of such scheme as in the FOAM ProgrammersGuide P-43 it is said that:

"The Crank Nicholson scheme can be implemented by the mean of implicit and explicit terms:

solve
(
fvm::ddt(phi)
==
kappa*0.5*(fvm::laplacian(phi) + fvc::laplacian(phi))
)
".

If is this so, I'have to rewrite the left hand side of the corresponding UEqn.H exploiting both fvm and fvc operator in order to implement the Crank Nicholson scheme. Otherwise I would not have an effective Crank Nicholson time integration schemes and consequently losing the second order time accuracy.

Any hints about that

Regards

Andrea

[AirS]

Hi Foamers,

My simulation uses the LES Smagorinsky turbulent model. I would like to use cubRootVol for delta and the VanDriest damping function with it. Is that possible? How can I do that?

Here is my LESProperties file:
LESModel Smagorinsky;
delta cubeRootVol;
printCoeffs on;
...

Thanks for your help,

[lakeat]

Easy, you just need to choose VanDriest

Regards,

[AirS]

So the choice of vanDriest for delta permits to use cubeRootVol for delta along with the Van Driest damping function ?
Another question: Do you know where I can change the Cs coefficient ? I read somewhere it is equal to 0.13, but I'd like to change it to 0.1.
Thanks!

[lakeat]

1. Yes
2. By ajusting Ck you can change Cs, I suggest you read some papers to get an idea about their detailed relationship.

Regards,

[Elham]

Originally Posted by cedric_duprat

Hi Eugene,

euh ....not really )

As I told, the geometry and the grid are different. it's the same geometry as the DNS calculation. So streaks are shorter than the box and there is (should be) no effect from the outlet on the inlet.

the time discretisation is Crank-Nicholson. (I think it's backward in the tutorial).
For the numerical scheme I using only central diffential scheme (to keep second order accurate).
so there is no limitedLinear 1 for these terms (div(phi,k), div(phi,B))
Then, the time step is different to keep Co number less than 0.4.
For the solver, I'm using ICCG to solve the pressure (and the same PISO as the tutorial) and BICCG for the other quantities, which is quite different from the tutorial also.

Can these settings bring me some over diffusive terms, because, it should not, contrary to the tutorial (convective scheme view).

Thank you for giving advise,... I hope it's not a stupid question. But, because the results are not so "bad" (but also not so good ) ), I think it's just a small things.


Cedric

Dear Cedric,

Would you please let me know why you kept Co number less than 0.4? Is it based on your own experience and cause better results?
I had a relatively good results with rough mesh but not with a finer mesh. The time steps for both of them were the same. Is it because of the time step? Co number for the finer mesh is about 1.0.


Cheers,

Elham

[cedric_duprat]

Elham,

Well, as you can see on the forum, I ran these calculations in 2008 (with an old version of OpenFOAM) so .... I don't remember every settings.

What I remember is that if I increased the CFL to much, calculation crashed (which make sence). 0.4 was kind of optimum for my case.

The size of your mesh and your time-step (if it has been fixed) give you the CFL. If you refine your mesh and you keep the same time-step, you'll get a higher CFL value. Why don't you reduce the time step in such a way that the same CFL is used in both calculations ?

What are your results for coarse and fine mesh ? could you give us more details on these meshes ?

Cédric

[tiam]

Originally Posted by cedric_duprat

Elham,

Well, as you can see on the forum, I ran these calculations in 2008 (with an old version of OpenFOAM) so .... I don't remember every settings.

What I remember is that if I increased the CFL to much, calculation crashed (which make sence). 0.4 was kind of optimum for my case.

The size of your mesh and your time-step (if it has been fixed) give you the CFL. If you refine your mesh and you keep the same time-step, you'll get a higher CFL value. Why don't you reduce the time step in such a way that the same CFL is used in both calculations ?

What are your results for coarse and fine mesh ? could you give us more details on these meshes ?

Cédric

This is a good question though. I have no problem running at CFL around 1, but many papers mention 0.4-0.5, is there are a particular reason for these choices?

Also, protip -- to know what time-step to pick for a certain CFL you can use the adjustableTimeStep option during the simulation phase where you dump the transients. Then, you can check out the max time-step you had in the log and use that as a constant time-step value in the part of the simulation where you collect the statistics.

[Elham]

Originally Posted by tiam

This is a good question though. I have no problem running at CFL around 1, but many papers mention 0.4-0.5, is there are a particular reason for these choices?

Also, protip -- to know what time-step to pick for a certain CFL you can use the adjustableTimeStep option during the simulation phase where you dump the transients. Then, you can check out the max time-step you had in the log and use that as a constant time-step value in the part of the simulation where you collect the statistics.

Thanks.

Elham

[Elham]

Dear all,

My results for Re_tau=330, target Re_tau=395, with 5 cells in y+<5 and the first y+=0.73 and Re_b=13350 has been attached. As you see the profile in global coordinate is near to DNS results but in wall coordinate is so far from DNS. I suppose I am doing something wrong in drawing the plots. I let the flow to pass around 90 flow throughs and then averaged just for 8 flow throughs. I know the averaging time is not enough but the difference between DNS results and mine is so big that I think the problem will exist after passing more and more time.
I would appreciate if anyone can give me some clues.
PS: The problem may be come from the spatial averaging as I just do time averaging in a specified plane and no spatial averaging. If I want to use fieldAverage function in ControlDict, I need to keep data of every time step which demands high storage capacity.

Cheers,

Elham

[anishtain4]

Elham,

How are you calculating the wall shear stress? It seems your wall scaled plots are off by a scale, use wallGradU utility to read the velocity gradient at the wall rather than calculating it by matlab or anything else.