LES Velocity Profile
 

Hi, I am having trouble running a turbulent simulation of flow over a flat plate. I have air at 1 m/s traveling over a 10m long plate, giving me a Re~600,000 at the outlet. I have followed the Fluent Best Practices guide for my mesh, with my y+ <1, x+ ~ 20, z+ ~ 40.

I started with a k-e RANS run, took the velocity and turbulence data from 1m in, set that as my inlet boundary condition, re-ran RANS again, then took that solution as my initial solution for LES. I initialized turbulence and changed to the transient solver, and am using the vortex method at the inlet for turbulence/unsteadiness. I ran for about 5 flowthroughs, then started collecting statistics. After ~10 flowthroughs, I have looked at the results, and my velocity profile (using mean velocity) is not right.

I plotted my u+ vs y+ and compared to the law-of-the-wall expected results (Spalding curve) but my results do not match. They follow the expected curve for ~1/3 of the curve length, then rise up, giving me a higher u+ than I should get for the corresponding y+.

I have tried this using RANS, LES, and DES. RANS and DES match the Spalding law-of-the-wall curve beautifully, but LES does not. What could be my problem? :confused:

So your computational domain is 10 m in streamwise direction. What about the other directions? What boundary conditions did you use?
If you really want to do it this way, you should take the profiles from as far downstream as possible.

Nevertheless, I recommend periodic boundary conditions between inlet and outlet. This will leave you with much less modeling uncertainties concerning the inlet specification.
Additionally. z+=40 and x+=20 are probably too coarse for a wall-resolving LES.

My domain is ~.5m in the normal direction (y) and .36m in the spanwise direction (x). My inlet is velocity inlet, my outlet is outflow ( I compared with pressure-outlet as well and there is little to no difference). The top of my domain is given the 'symmetry' condition, with the bottom (the plate) set as 'wall'. The boundaries in the spanwise direction are periodic boundaries.

I set my inlet boundary condition from the the profiles at 1m in just to aid in tripping turbulence with the vortex method. When I calculate my velocity profile I do it at 10m.

Some details are missing:

1) Is x your streamwise direction and z the spanwise one? If it is the case i would invert your spacings as dx+=40 and dz+=20. Still, unless you are using a periodic condition streamwise and an equilibrium boundary layer, these values are gonna change in x.

2) What are your discretization parameters? Central schemes for convection and second order in time are mandatory. Also, my experience is that PRESTO! is more dissipative than other pressure discretizations but it is the only one providing meaningful spectral energy distributions and RMS profiles. Finally, the courant number should be below 1, possibly around 0.1

3) What is your SGS model? Static Smagorinsky model is not suitable here and other options should be considered.

4) How much wrong is the velocity profile? And the velocity fluctuations (RMS)? The shear stress (average uv)? Is it laminar like or just overestimating the log part and the x-RMS peak?

5) The vortex method (which is the method of choice in Fluent) requires mean vleocity and turbulent profiles at inlet. I don't understand your procedure to assign them. I would compute an Equilibrium B.L. solution with a Reynolds Stress Model and simply assign them to your inlet method.
Why do you need to do that twice?

At the end of the day, this is still a damn problem to simulate with a low order code and in no way you can be sure of the success of your simulation.

Sorry, yes, x is my streamwise direction and z spanwise, and I am actually using the mesh sizing you suggest above, apologies if I mistakenly said otherwise above.

I'm using PISO scheme for Pressure-Velocity coupling, Bounded Central Difference for Momentum, Body Force Weighted for Pressure, and Bounded 2nd Order Implicit for Transient discretization. My max CFL number is well below 1, close to ~.1 actually as you suggest.

I am using the WALE subgrid scale model. I have also examined the Dynamic Smagorinsky model but this showed no great improvement.

The shear stress is OK, it matches decently well. The problem is in the velocity profile itself. It is not laminar, and it overestimates the u+ (or Ux if I look at dimensional values).

I admit the method I used may be slightly more complicated than need be. It is the way that was suggested to me by my superiors as the method that had been used before. It seems to me that it should work ok, though yes I could do use a RSM and put the stresses in with the inlet BC. I run it twice because the RANS runs are not very time-intensive, though this is not needed I suppose.

Your settings are ok.

Do you recognize any of your problems in the results in the paper below:

http://www.lamc.ing.unibo.it/aimeta2.../MEM-273-0.pdf

In that case it is just that LES is far from perfect, especially in Fluent

The results from that paper look remarkably like what I am seeing. My nondimensional velocity profile looks almost identical to theirs. I have switched my momentum scheme to the unbounded central differencing, and am seeing an improvement - though not perfect - as well.

Do you happen to know if the future investigations into the pressure interpolation schemes mentioned in the paper yielded any information? As I said above I have been using Body Force Weighted, but wonder if trying Second Order might be helpful? Thank you very much, you have been very helpful sbaffini!

The investigations were actually done but i don't have a paper. The result is that PRESTO is to prefer over a second order scheme. Less rigorous tests led to the same conclusions for the standard and linear schemes. Sadly i have no info on the Body force weighted but, according to my experience, it is very similar to the PRESTO! scheme and i do not expect significant differences among the two.

Notice, however, that the main conclusion of the test above was not based on the mean velocity profile but on velocity fluctuations and the relative spectra, which were strongly and badly affected. The mean velocity profile was actually better in terms of overall agreement with the DNS one but, still, the velocity profile was much more a boundary layer one than a channel one, with a sort of potential zone in the middle of the channel (which is clearly wrong).

Alternate URL for Paolo's paper?
 

Do you have a new link to your paper Paolo? This one seems dead, and I would really like to read it.

Dear Alan,

i have no idea why the link is gone (thanks for the information). At the moment i have no access to my laptop, but i will post the paper here (possibly in my blog page on this site) as soon as possible. However, consider reading my Ph.D. thesis (still in the blog). Chapter 6 should have all the information contained in the AIMETA paper (actually there is much more than that).

Regards

http://www.lamc.ing.unibo.it/aimeta2.../MEM-273-0.pdf



Do you have a new link to your paper Paolo? This one seems dead, and I would really like to read it.

Sorry，but i cant find the link in your blog.could you please give me a new link to the paper ？

If you search for the paper:

Sensitivity Analysis on Numerical Parameters for Large Eddy Simulation with an Unstructured Finite Volume Commercial Code

you will find it both under google scholar or researchgate directly. However, the comment on the thesis is still valid.

Best regards

Thank you so much! Good luck!