
[Sponsors] 
December 27, 2013, 14:00 
Unstructured Large Eddy Simulation Solver problems

#1 
Member
Join Date: Oct 2012
Location: IITHyderabad, India
Posts: 42
Rep Power: 7 
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 

December 27, 2013, 14:20 

#2 
Senior Member
cfdnewbie
Join Date: Mar 2010
Posts: 557
Rep Power: 13 
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?) 

December 27, 2013, 14:46 

#3 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 3,818
Rep Power: 42 
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. 

December 27, 2013, 15:30 

#4 
Member
Join Date: Oct 2012
Location: IITHyderabad, India
Posts: 42
Rep Power: 7 
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?? 

December 27, 2013, 17:27 

#5 
Senior Member

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). BabaAhmadi 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 cellcentered 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 underdetermined 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. 

December 27, 2013, 19:20 

#6 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 3,818
Rep Power: 42 
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. 

December 29, 2013, 04:52 

#7 
Member
Join Date: Oct 2012
Location: IITHyderabad, India
Posts: 42
Rep Power: 7 
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? 

December 29, 2013, 05:06 

#8 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 3,818
Rep Power: 42 
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.... 

December 29, 2013, 07:24 

#9  
Member
Join Date: Oct 2012
Location: IITHyderabad, India
Posts: 42
Rep Power: 7 
@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? Quote:
(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). 

December 29, 2013, 09:41 

#10 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 3,818
Rep Power: 42 
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 

December 30, 2013, 04:17 

#11 
Senior Member

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 cellcentered gradient (first term, the one you want to compute in a leastsquares sense) and a facecentered 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 cellcentered gradient) and only a single equation. The way i understood the algorithm is that you compute the three components in a leastsquares sense (MoorePenrose pseudoinverse, i guess) and use the so computed cellcentered pressure gradient in correcting the cellcentered 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 RhieChow, i repeat, is fairly obscure to me. 

Tags 
cfd, les, les jet, smagorinsky model, turbulence 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
ABL solver  Large eddy simulation  Davidlt  OpenFOAM Programming & Development  1  May 8, 2017 01:01 
Large Eddy Simulation  Nijanthan  FLUENT  13  January 30, 2014 20:28 
Reversed flows in Large Eddy Simulation  luc89ita  FLUENT  0  August 3, 2013 07:15 
[ICEM] Problems with coedge curves and surfaces  tommymoose  ANSYS Meshing & Geometry  0  August 5, 2011 16:02 
Large eddy simulation  David  FLUENT  1  December 11, 2006 13:18 