# LES

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

 June 20, 2012, 12:49 #201 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hello everyone, Trying to improve my case I implemented the following changes in fvSchemes: ------ ddtSchemes { default backward; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss linearUpwindV grad(U); div(phi,k) Gauss upwind; div(phi,B) Gauss limitedLinear 1; div(phi,nuTilda) Gauss limitedLinear 1; div(B) Gauss linear; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear limited 0.333; laplacian((1|A(U)),p) Gauss linear limited 0.333; laplacian(DkEff,k) Gauss linear limited 0.333; laplacian(DBEff,B) Gauss linear limited 0.333; laplacian(DnuTildaEff,nuTilda) Gauss linear limited 0.333; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default limited 0.333; } fluxRequired { default no; p ; } ----------------------- I tried all variants of OneEqEddy LES model (cubeRootVol, vanDriest, smooth) with the above corrections. The solution diverges after 100 time steps. Then i made some change: ----- gradSchemes { default cellLimited Gauss linear 1; grad(p) cellLimited Gauss linear 1; grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) Gauss filteredLinear2V 0.5 0; div(phi,k) Gauss linearUpwind grad(k); div(phi,B) Gauss limitedLinear 1; div(phi,nuTilda) Gauss limitedLinear 1; div(B) Gauss linear; div((nuEff*dev(T(grad(U))))) Gauss linear; } ------ Other schemes remain the same. The solution blows up even faster (arond 30 time steps). Could anybody tell what the problem is? Kind regards, Achinta Last edited by achinta; June 20, 2012 at 12:49. Reason: improvement

 June 20, 2012, 12:52 #202 Member   achinta Join Date: May 2010 Location: Sydney Posts: 66 Rep Power: 9 Hi Rob, Please let me know what specific information you need (except for the mesh, which is confidential ). Kind regards, Achinta

 October 5, 2012, 08:16 #203 Member   Paula Join Date: Aug 2012 Posts: 30 Rep Power: 7 Hi, I´m also interested on this topic? Did anyone got the answer to Roland´s question?

 October 5, 2012, 08:35 #204 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 15 The logfile can give some information. Can you show part of the logfile, where the divergence occurs?

October 5, 2012, 10:46
#205
Member

Paula
Join Date: Aug 2012
Posts: 30
Rep Power: 7
Quote:
 Originally Posted by Bernhard The logfile can give some information. Can you show part of the logfile, where the divergence occurs?
Sorry Bernhard, I wrote at the wrong thread :S

 October 21, 2012, 05:12 #206 New Member   Ken Tay Join Date: Oct 2012 Location: Singapore Posts: 5 Rep Power: 7 Hi all, Am new here. I am looking to implement a 2-part eddy viscosity model as outlined by Sullivan et al (1994) www.mmm.ucar.edu/people/sullivan/talks/papers/sgs.pdf Currently, I am thinking of using pimpleFoam solver and have been looking at modifying the oneEqEddy LES model, changing the divDevbeff in GenEddyVisc.C to the appropriate formulation of tau_ij. However, I am running into several issues: 1. How to get the homogeneous averages for , , during runTime as I need these values for each time-step 2. I am still unsure if using pimpleFoam is ideal, even if I want to neglect the effects of temperature and hence the buoyancy effect Anyway, I would appreciate any pointers from you guys if any of you have attempted to do this implementation. Thanks a lot.

October 23, 2012, 05:17
#207
Senior Member

Albrecht vBoetticher
Join Date: Aug 2010
Location: Zürich, Swizerland
Posts: 218
Rep Power: 10
Quote:
 Originally Posted by kentriarch Hi all, Am new here. I am looking to implement a 2-part eddy viscosity model as outlined by Sullivan et al (1994) www.mmm.ucar.edu/people/sullivan/talks/papers/sgs.pdf Currently, I am thinking of using pimpleFoam solver and have been looking at modifying the oneEqEddy LES model, changing the divDevbeff in GenEddyVisc.C to the appropriate formulation of tau_ij. However, I am running into several issues: 1. How to get the homogeneous averages for , , during runTime as I need these values for each time-step 2. I am still unsure if using pimpleFoam is ideal, even if I want to neglect the effects of temperature and hence the buoyancy effect Anyway, I would appreciate any pointers from you guys if any of you have attempted to do this implementation. Thanks a lot.
Have you taken a look at the LTT-Rostock OpenFOAM extensions? Matthias Walter has developed several dynamic subgridscale models for OpenFOAM and you can find the source code on their repository, there it should be possible to find code snippets you could use. (By the way, I strongly recommend the DMM SGS model)

October 23, 2012, 06:15
#208
New Member

Ken Tay
Join Date: Oct 2012
Location: Singapore
Posts: 5
Rep Power: 7
Quote:
 Originally Posted by vonboett Have you taken a look at the LTT-Rostock OpenFOAM extensions? Matthias Walter has developed several dynamic subgridscale models for OpenFOAM and you can find the source code on their repository, there it should be possible to find code snippets you could use. (By the way, I strongly recommend the DMM SGS model)
Nope, I have not, but thanks for the recommendations and I will look in them!

January 13, 2013, 20:13
#209
New Member

Ali Lohrasbi Nichkoohi
Join Date: Oct 2011
Posts: 15
Rep Power: 8
Quote:
 Originally Posted by grandgo hi gregor, yes, it was my worry, that it has something do to with my domain not being cube-shaped. thanks anyway. best regards grandgo
HI GREGOR and grando
i copied and do wmake your code above. my case is rectangular(3d). i want to :
1: write the E-K in one dimentional in space
2: write the E-K in one dimentional in time
3: write the E-K in 3 dimentional in space
4: write the E-K in 3 dimentional in time
how can i do it?
lohrasbi2013@gmail.com

 January 17, 2013, 08:11 #210 Member   Gregor Olenik Join Date: Jun 2009 Location: http://greole.github.io/ Posts: 80 Rep Power: 10 Hi Lohrasbi, for the E-K in space you can have a look at how it is done in the dnsFoam solver. In principle you could use: Code: ```#include "Kmesh.H" #include "calcEk.H" Kmesh K(mesh); calcEk(U, K).write(runTime.timePath()/"UEk", runTime.graphFormat());``` this will give you the E-K of the whole domain (for the three components of U). If you want E-K of a single velocity component you could just create a vector with three identical components (e.g Ux[0]=U[0], Ux[1]=U[0],Ux[2]=U[0]) and then use calcEk(Ux,K) and divide the result by three (hope thats correct). For E-K over time you mean E-K at a specific point of the domain, right ?

 December 19, 2013, 16:46 #211 Senior Member     Hasan K.J. Join Date: Dec 2011 Location: Bristol, United Kingdom Posts: 199 Rep Power: 7 Hi all, I am using this mapped value of fields from a setup to simulate flow around an airfoil, now for this particular case, when i use RANS i map the Nut field because it is non-uniform on the top and bottom of the airfoil, so to get accurate results i have to map it. now when i want to perform LES ? what do i do, do i map the nuSgs field ? if so how because I am mapping from a RANS simulation and it does not have nuSgs field or do i just map the Nut and change its name to nuSgs and the dimensions !!! ? does it work like that ? do they have any similar relation Thanks for your time, Regards, Hasan K.J

 December 26, 2013, 16:23 #212 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,036 Blog Entries: 39 Rep Power: 110 Greetings to all! @Hasan: AFAIK, when LES is involved, what usually is done is to first run the simulation with a steady-state solver with LES; then run a transient solver with LES as well. One such tutorial in OpenFOAM that demonstrates this, is this one: "incompressible/pisoFoam/les/motorBike" If you need to pass RAS fields to LES ... either you'll need an utility that calculates an estimate from the RAS fields to LES fields, or you'll have to create one yourself. Have a look into this utility "applications/utilities/postProcessing/turbulence/createTurbulenceFields" - it's meant for creating RAS turbulence fields, but perhaps you can create a similar utility for LES... because I'm not aware of any existing already... Wait, apparently someone already created the utility "createTurbulenceFieldsLES": http://www.cfd-online.com/Forums/ope...ields-les.html Beyond this, the turbulence fields are usually calculated from the pressure and velocity fields, using the initial turbulence fields only as a reference. Therefore, you don't need to specifically map the LES related turbulence fields... you just need to give non-ridiculous initial values for the turbulence fields and after some iterations it should be able to sort things out on its own. Best regards, Bruno edit: conversation on the related topic to Hasan's case is here: http://www.cfd-online.com/Forums/ope...-openfoam.html Alhasan and adambarfi like this. __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide What am I doing/planning: blog/wiki Read this before sending me PM Last edited by wyldckat; December 28, 2013 at 16:52. Reason: see "edit:"

February 26, 2014, 21:35
#213
Member

Peter
Join Date: Nov 2011
Posts: 46
Rep Power: 8
Quote:
 Originally Posted by eugene np. p=0 and small k is fine. nuSgs doesn't matter because it is calculated from k and delta.
Hi, Eugene!

The y+ is smaller than 2 in my case which is a LES simulation. I set k a small value (1e-5) at the inlet boundary. How should I set k at the wall boundary?

Best regards,
Peter

May 22, 2014, 07:13
#214
Senior Member

ArathoN
Join Date: Jul 2011
Posts: 137
Rep Power: 9
Quote:
 Originally Posted by palmerlee Hi, Eugene! The y+ is smaller than 2 in my case which is a LES simulation. I set k a small value (1e-5) at the inlet boundary. How should I set k at the wall boundary? Best regards, Peter
The turbulent kinetic energy is null at the walls. And for the value at the inlet you can define it after considering a turbulence intensity of 5÷7% then knowing U it's easy to calculate it.

May 22, 2014, 07:44
#215
Senior Member

Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 20
Quote:
 Originally Posted by ArathoN The turbulent kinetic energy is null at the walls.
Right, but set it to some really low number (such as 1e-12) at the wall in OpenFoam. At some places OpenFoam divides by "k", so setting it to "0.0" will result in an error. Now, a really low value will give a correct division, but is pratically zero for all multiplications.
__________________
The skeleton ran out of shampoo in the shower.

 March 1, 2016, 14:44 #216 Senior Member   Mahdi Hosseinali Join Date: Apr 2009 Location: NB, Canada Posts: 271 Rep Power: 11 Hi everyone, I know this thread has not been active for a while but I guess this is the most related topic so I'm going to post here. I'm running the channel flow LES which is now under pimpleFoam. The tutorial case runs well but my trouble is that I need the structures which are being compromised in the current domain as mentioned in Eugene's thesis. When I extend the length of the domain (and consequently the grid numbers) the profiles are not valid any more. Even though the bulk velocity, CFL, and Retaw and everything else should be the same. I think is is coming from the initial conditions. Does anyone else has experience with this?

March 1, 2016, 14:53
#217
Member

Timofey Mukha
Join Date: Mar 2012
Location: Uppsala, Sweden
Posts: 83
Rep Power: 7
Quote:
 Originally Posted by anishtain4 Hi everyone, I know this thread has not been active for a while but I guess this is the most related topic so I'm going to post here. I'm running the channel flow LES which is now under pimpleFoam. The tutorial case runs well but my trouble is that I need the structures which are being compromised in the current domain as mentioned in Eugene's thesis. When I extend the length of the domain (and consequently the grid numbers) the profiles are not valid any more. Even though the bulk velocity, CFL, and Retaw and everything else should be the same. I think is is coming from the initial conditions. Does anyone else has experience with this?
Hello!
I am not sure I understood what the problem is, what do you mean by "the profiles are not valid any more"? Your results don't compare well with dns?

For the initial conditions, you can use the perturbU
https://github.com/wyldckat/perturbU

Some other tips based on my experience.
• Ditch the SGS model. Specifically, Smagorinsky and oneEqEddy only make things worse, even though van Driest damping does imporve things significantly. Other models are tried were on par with not having a model at all.
• A grid with delta x+=25 and delta z+ =10, and a good amount of points along y, with y+=1 should give very nice results.

 March 4, 2016, 06:48 #218 Member   taygun gungor Join Date: Mar 2015 Posts: 37 Rep Power: 4 What do you mean extend the length of domain? If you extend it in streamwise direction, it should be fine, for other directions it fails if I remember the case correctly.

March 14, 2016, 09:53
#219
Senior Member

Mahdi Hosseinali
Join Date: Apr 2009
Posts: 271
Rep Power: 11
Quote:
 Originally Posted by tiam Hello! I am not sure I understood what the problem is, what do you mean by "the profiles are not valid any more"? Your results don't compare well with dns? For the initial conditions, you can use the perturbU https://github.com/wyldckat/perturbU Some other tips based on my experience. Ditch the SGS model. Specifically, Smagorinsky and oneEqEddy only make things worse, even though van Driest damping does imporve things significantly. Other models are tried were on par with not having a model at all. A grid with delta x+=25 and delta z+ =10, and a good amount of points along y, with y+=1 should give very nice results.
I tried multiple tests. In all of which the grid was fine enough (y+=0.6, z+=20, z+=10) and CFL<0.5. But my results were still off (not in agreement with theory or dns). I came to realizes when I change the domain size and use the perturbUChannel the perturbations are being damped! I tried the perturbUChannel with the tutorial case and it does not work!!! I've tried OF 2.4 and 3.0.

Quote:
 Originally Posted by clktp What do you mean extend the length of domain? If you extend it in streamwise direction, it should be fine, for other directions it fails if I remember the case correctly.
If the grid size, CFL, and Re are in the range it should work for any setting.

 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

All times are GMT -4. The time now is 15:09.