# Is it wrong to use LES models for low resolution simulations?

 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 10, 2017, 13:44 Is it wrong to use LES models for low resolution simulations? #1 New Member   Lukas Lebovitz Join Date: Mar 2017 Location: Zürich, Switzerland Posts: 25 Rep Power: 2 LES models are designed to resolve a part of the turbulent effects and model the remaining part. There is a the "best-practice saying" that you should resolve at least 80% of the turbulent kinetic energy. Now let's say the variable of interest has already converged with a coarser mesh and that you don't resolve 80% of the turbulent kinetic energy. Is a LES model specifically designed to have at least 80% resolved and will it behave "wrong" when you are too coarse? There are the scale adaptive simulation (SAS) models which switch between RANS (k-omega SST) and LES models depending on the grid. Should you you prefer the SAS model if your LES only resolves 20-60% of the energy? Or can you get good results with low resolved LES when you confirm your variable is converged (respectively grid independent) for the grid? Thank you so much! lkoc likes this.

 April 10, 2017, 21:42 #2 Senior Member     Uwe Pilz Join Date: Feb 2017 Location: Leipzig, Germany Posts: 389 Rep Power: 5 LES models the large vortices directly and calculates their dissipation by a model. What "large vortices" are depends on the mesh. As coarser the mesh as larger the direct modeled eddies, and the more part of the flow needs to be covered by a formula and no by direct numerical calculation. I don't see that there is something wrong with using a mesh which covers less than 80% of the energy. A larger part of the solution depends on the dissipation formula, and therewith the total acuracy is lower - as always with a coarse mesh. __________________ Uwe Pilz -- Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950)

 April 13, 2017, 17:03 #3 New Member   Lukas Lebovitz Join Date: Mar 2017 Location: Zürich, Switzerland Posts: 25 Rep Power: 2 I asked my supervising professor about this. He replied that in LES it is important to resolve the energy containing range of the spectrum. The cutoff should be in the inertial range. The 80% mark for the resolution of the turbulent kinetic energy is a value which guarantees in most cases that the energy containing range is resolved. Hybrid models like SAS are specifically designed for cases where you don't resolve 80% of the energy. Though hybrid models don't really appeal to me.

 April 15, 2017, 07:11 #4 Senior Member   Julio Mendez Join Date: Apr 2009 Location: Greensboro, U.S.A Posts: 275 Rep Power: 11 I agree with your advisor. You must check the spectrum to make sure your grid cut-off lies on the inertial subrange from the energy spectrum. However, your doubt can be very specific to your model. For example, what happen close te wall ??. Are You using Smagorisnky ? If your Re is small then using LES might not hurt you because the mesh requirements is not that strong.

 April 16, 2017, 04:21 #5 New Member   Lukas Lebovitz Join Date: Mar 2017 Location: Zürich, Switzerland Posts: 25 Rep Power: 2 Currently I'm using OneEqEddy, but I might try DynOneEgEddy. With my current mesh I can resolve >95% in the domain and go down to 10% near the wall. I will refine my mesh near the wall but maybe I'm only able to do LES with Near Wall Modeling (LES-NWM). juliom how can I check my spectrum and make a statement on where the cutoff is in my case?

 April 16, 2017, 07:17 #6 Senior Member   Julio Mendez Join Date: Apr 2009 Location: Greensboro, U.S.A Posts: 275 Rep Power: 11 I was about to ask you, how are you sure that you are solving 95% of the scales in the domain ( isotrooic zoned) and 10% close the walls without a plot of the spectrum of the kinetic energy? At least for an untrained eye like me, I will need to see the spectrum before draw that conclusion. In the spectrum you see where the cuttoff ratio imposed by the mesh is.

 April 16, 2017, 09:30 #7 New Member   Lukas Lebovitz Join Date: Mar 2017 Location: Zürich, Switzerland Posts: 25 Rep Power: 2 Ok but how do you plot the spectrum? I can estimate the amount of resolved TKE by computing the resolved turbulent kinetic energy resTKEMean (1/2*trace(uPrime2Mean)) and then then estimate the resolution = resTKEMean/(resTKEMean + kMean), where k is the modeled subgridscale TKE.

 April 16, 2017, 11:15 #8 Senior Member   Julio Mendez Join Date: Apr 2009 Location: Greensboro, U.S.A Posts: 275 Rep Power: 11 Well, my guess is that you are using openFoam. I'm not an expert in openFoam and I rather develop my own codes. I would say that I disagree with that equation because the subgrid scale dresses are a function of the resolved scales and you don't know the exact value for the subgrid stresses. That's is why you have to introduce the model. Therefore, when you perform the division you assume that you know the exact value of the subgrid stresses and that's is why you get " a ratio" but my guess is that ratio is wrong. Make a try with different meshes. And you will see that ratio will change, off course. The spectrum computation is not a trivial task and it is cumbersome to explain it in this forum. However, my first question will be about your boundary conditions. If you have periodic boundary conditions then the pain of computing the spectrum will be lower. You need to develop your subroutines and compute Fourier coefficients. I recommend you to read Pope's book. It took me few weeks to understand that. I'm sure that will not be your case, and you will get it faster. If your boundary conditions a are different then you have to apply a windowing

 April 16, 2017, 11:56 #9 New Member   Lukas Lebovitz Join Date: Mar 2017 Location: Zürich, Switzerland Posts: 25 Rep Power: 2 Yes the ratio is wrong since you don't know if you modeled the right amount of energy. But in my opinion it's a first estimate to evaluate the quality of your mesh. For a coarser mesh the ratio will go decrease and for a finer mesh it will get closer to 1. At locations where you expect smaller scales to be produced you will find that the ratio will be lower compared to other locations. If you want to know the exact ratio you had to do a DNS. I haven't really bothered too much with the spectrum so far but I'm sure that I will have to learn how to compute it. Can you give any good references on how to compute it additionally to pope? I use cyclic boundaries on my lateral side's of my domain. Front and Back is inlet and outlet respectively. The ground is a noslip wall and top is a freeslip wall. I use the filtered noise method to produce turbulent inlet flow. And yes I'm using openFoam.

 April 16, 2017, 12:27 #10 Senior Member   Julio Mendez Join Date: Apr 2009 Location: Greensboro, U.S.A Posts: 275 Rep Power: 11 Well my opinion is that method is not useful at all, I may be wrong though. With your boundary conditions your approach will be very cumbersome because you need to compute Fourier coefficients using the fast Fourier transform and in order to do so you domain hast to be infinite (homogeneous in the dominant direction for convection). I cannot suggest other resource for computing the spectrum. However, there are a lot of discussions in this forum about that. The community helped me a lot. There is another approach that I haven't tested (validate) yet. Is basically assuming the the navier stokes equations is periodic in time (in fact is quasi peridodic). Based on that assumption you can fix on spot in space and comité the spectrum based on the time history on that location.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Xiaoyu Yang OpenFOAM Verification & Validation 18 May 19, 2017 04:48 The King OpenFOAM Running, Solving & CFD 0 April 1, 2017 10:19 dowlee OpenFOAM Running, Solving & CFD 8 October 25, 2016 19:48 saii CFX 2 September 18, 2009 08:07 Ridwan Setiadi Arrizar Main CFD Forum 1 January 30, 1999 18:43

All times are GMT -4. The time now is 09:30.