
[Sponsors] 
January 31, 2010, 04:00 
Reg. LES in OpenFOAM

#1 
Member
Ganesh Vijayakumar
Join Date: Jan 2010
Posts: 44
Rep Power: 9 
hi !
Newbie alert !! Wherever I look, I get redirected to Oodles or ChannelOodles for LES in OpenFOAM. I have OpenFOAM1.6.x installed finally and there's no solver called Oodles. Code:
[blah@blah incompressible]$ pwd /opt/OpenFOAM/OpenFOAM1.6.x/applications/solvers/incompressible [blah@blah incompressible]$ ls boundaryFoam nonNewtonianIcoFoam pisoFoam simpleFoam channelFoam pimpleDyMFoam porousSimpleFoam icoFoam pimpleFoam shallowWaterFoam 1. Is an LES solver in OpenFOAM nothing more than SGS stress terms added to the NS equation ? So it's pisoFOAM with SGS stress terms with appropriate turbulence models and modified boundary conditions, wall functions etc. ? 2. I do want to do a channel flow simulation. But what solver do I use in general for LES of incompressible flows ? pisoFoam ? 3. Can you suggest any better place than Eugene's thesis to start looking inside the box ? ganesh 

February 1, 2010, 13:44 

#2 
Member
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 10 
I would to add one more question:
 Is there already a solver in OF suitable for external aerodynamics LES? Best Regards, Paulo Rocha. 

February 2, 2010, 05:39 

#3 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
For LES I would suggest pimpleFoam with the appropriate turbulenceProproperties (LES) settings and boundary conditions. pimpleFoam is like pisoFoam but with incomplete convergence of the corrector steps.
For external aero LES just use the SpalartAllmaras DES model as SGS model. 

February 2, 2010, 20:13 

#4 
Member
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 10 
Thank you very much for the fast reply.
I will investigate further. Best Regards, Paulo Rocha. 

February 3, 2010, 07:36 

#5  
Member
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 10 
Quote:
Isn't DES a hybrid approach between RANS (near wall) and LES (free stream)? Isn't there a way to test pure LES for external aero? Thanks in advance, Best Regards, Paulo Rocha 

February 3, 2010, 22:35 

#6  
Senior Member
Daniel WEI (老魏)
Join Date: Mar 2009
Location: Beijing, China
Posts: 689
Blog Entries: 9
Rep Power: 14 
Quote:
Of coarse you can, provided you have a suitable mesh, etc. Try pisoFoam, I used to use them to do flow like flow past circular cylinder, building, etc. It works very well. Regards,
__________________
~ Daniel WEI  Boeing Research & Technology  China Beijing, China 

February 4, 2010, 07:48 

#7 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
DES is indeed a hybrid approach. I just assume that you would not be able to mesh external aerodynamic cases fine enough to use pure LES. If you do have the meshes to do pure LES, then I suggest you try the oneEqEddy, dynOneEqEdy or locDynOneEqEddy SGS models to start off with.
Check the openfoam workshop and open source cfd conference proceedings for similar applications. 

February 4, 2010, 09:10 

#8  
Senior Member
Jiang
Join Date: Oct 2009
Location: Japan
Posts: 186
Rep Power: 9 
Quote:
I have two questions: 1. If using oneEqEddy model, how we can set boundary for k? because for RANS model, we can get k from experiment for inlet condition. But for LES, we couldn't get subgrid turbulent kinetic energy for inlet. Or just give a small value is OK ? for example 5e5. So I think why so many people use Smagorinsky model, maybe don't need to set boundary for k, am I right ? 2. I have read your paper, that is very good! the size of my case is very similar to your "Side Mirror" one. First I use 300000 meshes Smagorinsky+ Spading law wall function, and then I use a little finer mesh 500000 mesh Smagorinsky+ VanDriset damping function, both of my velocity value is smaller than RANS and Experiment data above ground 12mm position, that meas my LES result shear stress is larger, so velocity is small. Could you give me some suggestions to improve my LES result ? Tnank you very much. 

February 5, 2010, 05:47 

#9 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
Hi,
The boundary for k is pretty straightforward, since you will have no resolved scale turbulence at the inlet, just set it to the equivalent RANS value. It will adjust really quickly once things start happening. Setting it too small is not a good idea, as this can lead to spurious numerical noise if you have any grid abnormalities. All I can suggest, is that you try the other turbulence models and see what happens. I haven't run pure LES for a while, but in literature most people use some kind of dynamic model. Also, the oneEqEddy model I used in my thesis is not the same as the one currently in OPENFOAM. I had a separate nearwall dissipation lengthscale that was independent of the turbulent energy length scale. This improved results on channel flows by a few percent relative to the current model. The independent dissipation scale does not fit into the current SGS model framework though and was not incorporated into the release code as a result. Unfortunately, I no longer have the code for this. 

February 6, 2010, 19:21 

#10 
Member
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 10 
Eugene, Daniel and all
Thanks a lot for the information and time. I will start trying to solve my problem. Best Regards, Paulo Rocha 

February 7, 2010, 04:02 

#11  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Quote:
If there are numerical problems due to grid anomalies when k is set to be small, it simply means the mesh is not good enough for a LES anyway, or there is some problem in the numerics. Remember that, strictly speaking, you cannot use a nonuniform mesh in LES, since you assume you can commute the integral and the derivative operators, and you neglect the terms depending on the filter size when you filter the conservation equations. The error is generally not negligible. It was shown (Guerts and coworkers, take a look at what they published in Physics of Fluids in 2005 on the commutation error) that the error becomes small if the change in the filter is slow and its skew is limited, but this is surely not the case if the mesh anomalies can cause numerical problems. In addition, there is quite some interest around commutative filters and other approches to account for the commutation error. You might be interested in reading, for example, the work of Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 7, 2010, 15:12 
LES turbulent inlet

#12 
Senior Member
n/a
Join Date: Sep 2009
Posts: 198
Rep Power: 9 
Hey there Eugene. I have a question that has being ongoing for a short while. My research entails feeding the mean velocity and temperature profile into the lower portion of a plate (turbulent natural convection flow). So, to accurately predict the turbulent flow field downstream, what is the best approach to take in setting the turbulent inlet. I have considered superimposing some perturbations at the inlet and also remapping the flow field downstream back into the inlet. So any thoughts on this? Thanks.
And, I have not found any literature on how to set these turbulent boundaries in openFOAM. Is there any documentation or example in the code? Thanks. Kind regards Deji 

May 10, 2010, 04:48 

#13 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
Hi Deji,
The only implementation available in the standard code for LES inlets is the directMapped boundary for looping stuff back onto the inlet. You can find an example case here: $FOAM_TUTORIALS/iincompressible/pisoFoam/pitzDailyDirectMapped You could of course also write your own boundary with perturbation specifications. For a reference, search for papers by Gavin Tabor. (There are others as well, if you don't mind digging in the forum and online.) 

May 10, 2010, 09:42 

#14 
Senior Member
n/a
Join Date: Sep 2009
Posts: 198
Rep Power: 9 
Thank you very much Eugene.


May 24, 2010, 10:12 
Inlet velocity profile

#15 
Senior Member
n/a
Join Date: Sep 2009
Posts: 198
Rep Power: 9 
Hey there Eugene, I have a question. I am trying to implement the directmapped inlet for my LES simulation, and I happen to have my nonuniform velocity and temperature profiles at the inlet. I am unsure as to how to prescribe the average profile on the line I have marked on the posted sample velocity inlet profile. If possible , kindly give me some input on this matter. Thanks much.
inlet { type directMapped; value nonuniform 2 ( (0 0 .15) (0 0 .12) ); setAverage true; average ( ); < ?? } 

May 24, 2010, 11:42 

#16 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
Its not an average profile, its an average value.
average (<x y z>); for velocity and other vectors. average <x>; for temperature and other scalars. 

May 24, 2010, 12:48 

#17 
Senior Member
n/a
Join Date: Sep 2009
Posts: 198
Rep Power: 9 
Thanks for the response Eugene. Hence, to clarify, for each vector that I prescribe at the inlet, there should be an average (<x y z>) when utilizing the directmapped inlet bc. For example,
inlet { type directMapped; value nonuniform 2 ( (0 0 .15) (0 0 .12) ); setAverage true; average ( <x y z> ) ( <x y z> ); } Thanks 

May 27, 2010, 05:22 

#18 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
Unfortunately, what you want is not possible without code alteration. I checked the directMapped source code and it only admits a single value. This value fixes the mapped field average at every single timestep  i.e. the average is constant in time.
You are trying to impose a mean distribution, should not the shape of the distribution emerge from the flow calculation itself? It should not be too difficult to add an "average" field distribution, but I have no idea how you would use this to force your timemean input field (instead of you instantaneous field) toward the desired value. 

May 27, 2010, 08:44 

#19 
Senior Member
n/a
Join Date: Sep 2009
Posts: 198
Rep Power: 9 
Unfortunately, what you want is not possible without code alteration. I checked the directMapped source code and it only admits a single value. This value fixes the mapped field average at every single timestep  i.e. the average is constant in time.
You are trying to impose a mean distribution, should not the shape of the distribution emerge from the flow calculation itself? It should not be too difficult to add an "average" field distribution, but I have no idea how you would use this to force your timemean input field (instead of you instantaneous field) toward the desired value. Eugene, With the directMapped code, I assume it feeds the instantaneous field back into the inlet. So, I gather it would be more feasible to use the instantaneous field rather than some mean distribution. And it seems that the use of the single average value is only for a uniform inlet? I did take a look at your thesis work as you utilized this capability for the diffuser's inlet. In my research, there was a free convection experiment along a vertical plate and at some point the flow became turbulent. So, I am basically taking data at the inception of turbulence for the experiment and using it for my CFD calculation. Thanks. Best regards Deji 

May 27, 2010, 13:49 

#20 
Senior Member
n/a
Join Date: Sep 2009
Posts: 198
Rep Power: 9 
Hey there Eugene. I thought about this and the fact is I would rather have the instantaneous profiles at the inlet instead of the mean quantities. Mean profiles are utilized since that is all I have at that particular location of the start of a turb. b.L. Perhaps, the directMapped code should be suitable for my computation. The only thing that I am still somewhat confused by is the average quantity.
Kind regards Deji 

Tags 
les, pisofoam 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
LES of turbulent channel flows  cedric_duprat  OpenFOAM Running, Solving & CFD  213  March 20, 2017 23:20 
Serious bug in LES interface  fs82  OpenFOAM Bugs  21  November 16, 2009 09:15 
Implementing a new LES Model in OpenFoam  fs82  OpenFOAM  6  October 13, 2009 09:58 
Modified OpenFOAM Forum Structure and New MailingList  pete  Site News & Announcements  0  June 29, 2009 05:56 
LES at OpenFOAM Workshop  grtabor  OpenFOAM Running, Solving & CFD  0  March 25, 2008 05:36 