[samurai_01]

Hi everyone!!

I am developing a solver with LES for solving turbulent flows on unstructured grid for my Master's thesis.
The solver gives good results for standard laminar flow problems like Lid driven cavity, backward facing step validated duly with fluent and the experimental papers.Also I've simulated laminar jet emerging from an inlet of say D at inlet RE=300, and having a domain of 80D in length, and 40D in height with outflow condition at outlet and walls for surroundings with 2nd order time stepping(Crank Nicolson), with Upwind, central difference and a weighted mix of upwind and central difference known as deferred correction, and have validated the results from fluent for the same.

Now, when i implemented Static Smagronski model of LES with cs as 0.1, and for the problem of jet at RE=10,000 and 1,00,000; the jet appears to be falling one side as shown in the image(Fluent says it should be symmetric about mid plane).
After doing google and brainstorming for a long time I am unable to find the source of error.
I was using the deferred correction method for discretization of convection method.(also defined in Fluent manual as 26.2.11 : http://cdlab2.fluid.tuwien.ac.at/LEH...ug/node881.htm)

Inlet fluctuations are generated using adding random numbers (white noise method).
PLEASE HELP!!!
(if you need any more information please ask!!)
IMG: LES jetLES jet.jpg
IMG: Fluent LES jet:Fluent.jpg

[cfdnewbie]

a few thoughts:
a) did you run your code with CS=0.0, and compare the results (for a laminar case) to the old version without the added smagorinsky?
b) Is your mesh maybe biased?
c) I would assume that you have an error in your computation of mu_smago. Could you please initialize a symmetric field, and have your implementation compute the the mu_smago for that? (for a single step)?
d) looking at the plots, are you sure your inflow condition isn't wrong (angled down?)

[FMDenaro]

you are running a 3D case, right? what about the spanwise extension?
Could you plot the velocities at the inlet plane?

What I see from your plot is that you are following just the initial transient of the jet developping, this is not meaningful for LES. You must run your code for long time...

Concerning LES in Fluent with unstructured grids, some problems are known, sbaffini (Paolo) had several tests.

I suggest to use a low value for Cs or use the dynamic version.

[samurai_01]

Thank you everyone cfdnewbie and FMDenaro for your valuable replies. The code is still in development phase and is still in serial version, so I'll leave the simulations in the morning and will report the results ASAP.

@cfdnewbie:
a> Yes, but I'll redo it.
b>No the mesh is not biased, it gives results in agreement to laminar jet of RE=300 with fluent in same mesh.
c>I'll do that and report
d>No my inflow is not angled,(although I am using random number generator but will run the simulation without the same (I think i had... but never mind, I'll redo it)). Any references for Inlet conditions for LES ?

@FMDenaro:
I'll lower the cs value, to say 0.075 if that's ok? also I'll run the les code for longer time... 3 times the flow time perhaps??

I also read a paper by Krishnan et al(2004) CTR on "A numerical method for les on complex geometries" Journal of Computational Physics, there its mentioned about computation of pressure at n+1 level by minimizing the pressure gradients in least square sense... what does that mean.. any idea??
link:http://www.aem.umn.edu/~mahesh/03_04pubs.htm 5th paper from top, pg no. 230.
Can anyone explain what does it mean??

[sbaffini]

Few suggestions assuming that, in comparisons with Fluent, you are using exactly the same grids:

1) Do not compare with Fluent. As a Fluent user working in LES i usually have to compare with something else. If classical laminar tests worked fine for your code, that part should be considered validated. However, consider that, especially for unstructured codes, this might imply much more than simply running on a few cases. You are expected to test any possible grid topology, with any possible boundary condition (Dirichlet, Neumann, Periodic if present) and any possible numerical scheme; possibly under rotation of the reference frame.

2) When you have to go LES, you should not start by a case requiring a complicated inflow, as that is another part to test. If you just want to test the Smagorinsky part, you can first set Cs to 0, as suggested by cfdnewbie. Then, i also suggest to run a simple laminar flow in a channel where, if i remember well, a solution should still be possible (still, i might be wrong). Other than that (even if i understand that you might have not yet implemented periodic boundary conditions), there are still the Taylor 3D vortices, the mixing layer and the channel flow as benchmarks to validate your code (Homogeneous Isotropic Turbulence would require additional testing).

3) Let's say you have to work on the jet. The case is such that even a laminar inlet profile should eventually lead to turbulence. I would possibly test that first.

4) If everything really works, then your results clearly suggest some problem in the random number generator, as already suggested. I would check for the inlet contours to verify they really appear as randomly distributed and not, say, biased by the face numbering at inlet or something else.

5) Besides everything, the random number generator is not really going to solve your problems in LES. The easiest way to produce a meaningful inflow in LES/DNS remains, in my opinion, the remap strategy with an auxiliary domain. As i was able to implement it in Fluent, in parallel, in 2 days, i expect no problem for your code. Additional references for the inlet are the method of Smirnov, Shi and Celik (which i not suggest) or the vortex method (Jarrin, if i remember correctly). There have been some recent developments for both but, still, their implementation remain fairly complicated (in the sense that their implementation should be validated as well). Baba-Ahmadi and Tabor produced a not anymore recent review (because of the advancement in the two cited methods above).

6) The term referred to in the paper is the last step in the pressure correction, assuming you used a pressure free approach, that is, no pressure at all in the prediction. Once you know the pressure from the relative pressure poisson equation, you need to update the velocity field with a cell-centered pressure field, by adding its gradient. The way you compute it affects the conservation of energy; still, there is no way to conserve it as in a staggered approach. The suggested method to compute it involves solving the under-determined system (54), where the unknown is the cell centered gradient (the first term). Still, the details of the method are fairly obscure, especially in relation to the discretization of the pressure poisson equation in the first place which, as i understand, reappears in equation (54) as the second term.

[FMDenaro]

Paolo, I agree...more simple case would be better... I remember you had problems in solving even the simple channel flow using unstructured mesh..

furthermore, the total time required to run the LES is subdivided in two parts:
a) the numerical transient, where the code runs just to "clear" the memory of any arbitrary initial condition that is not physically correlated to the real turbulence. The period can be checked in several ways, I suggest to plot the total kinetic energy versus the time to see when an energy balance is reached.
b) the physical time interval in which a certain number of sample must be memorized and used for computing the statistics.

3 time units are less than required, you probably need more than 10 times such estimation.

[samurai_01]

Thank you for your replies.... I've put the simulations, and will report as soon as I get some results.
I have drichlet and neumann BC in my code, not the periodic(but i plan to implement them as soon as possible).
Can it be said that if an algorithm works for laminar flow(finite volume using collocated approach), after modification, it will work for LES? (only mu changes to mu_eff = mu+mu_turb).
I'll upload the algo and all calculations shortly, but still any opinion.. or should i proceed as said in the paper I've given reference above.

@sbaffini:
I have pressure poisson discretization figured out for the algo mentioned in the paper, but its said that the first term in 54 is calculated at cell centers and the second term is calculated on face centers, so it can't be used directly for computing velocities at cell center. This minimization in "least square sense" allows the second term to be used instead of first term as the difference between the two has been minimized.

now my question is how do i minimize this difference, i can compute the second term and the first term, get the difference between the two. but acc. to me, the minimum value of the expression should be zero!! which means we are using second term instead of first term to compute velocities at cell center, which has been discouraged(or rather said to be wrong) by the paper... Please throw some light on this .. how should the minimization be done?

[FMDenaro]

No, a method working well for laminar flow is not necessarily accurate for LES. For example, first order methods can work very well for laminar flows but not for LES.
Furthemore, LES does not mean you simply add some eddy viscosity term to your laminar code....

[samurai_01]

@FMDenero

Yes, i agree i cannot have first order method like upwind working for my code for LES.
I have stated earlier in a that i was using deferred correction scheme, something between central difference and upwind, and am also searching for bounded central difference.
Is there any other scheme that i can see to use for my convective terms?

Furthemore, LES does not mean you simply add some eddy viscosity term to your laminar code....

Can please elaborate a bit more or perhaps give few direction on this? I read the books, and they seem to suggest that the difference in NS and filtered LES is only of modeling the subgrid stresses, done by using different models, incorporated through mu_eff...
(I am a beginner in the subject, please pardon my ignorance on the matter, as I am the only one working on this topic here).

[FMDenaro]

Try using central scheme without bounding or defferred correction...

LES is quite complicated to understand fully, filtering the equation can be done in different way and different becomes the SGS meaning...
I suggest to have a reading about it starting from the book of Sagaut and using the book of Pope for general topics about turbulence

[sbaffini]

Dear Samurai,

what i get from the relation (54) in the paper (and i want to stress that i might be wrong) is that you have the cell-centered gradient (first term, the one you want to compute in a least-squares sense) and a face-centered one (second term, the one that you actually know as, possibly, consistent with your pressure poisson equation).

Now, the way equation (54) is written, involves 3 unknowns (the 3 components of the cell-centered gradient) and only a single equation. The way i understood the algorithm is that you compute the three components in a least-squares sense (Moore-Penrose pseudo-inverse, i guess) and use the so computed cell-centered pressure gradient in correcting the cell-centered velocities, as required by the final step of the fractional step algorithm.

Why this method should be any better than other approaches and why it doesn't require Rhie-Chow, i repeat, is fairly obscure to me.