CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

Enable LESModel in a foam solver

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 9, 2013, 18:51
Default Enable LESModel in a foam solver
  #1
New Member
 
Amir Abbas Aliabadi
Join Date: Mar 2013
Posts: 17
Rep Power: 3
amir.a.aliabadi is on a distinguished road
Hello There,

I am new to OpenFoam and interested to use LESModel with buoyantBoussinesqSimpleFoam solver. The standard solver is only equipped with RASModel. Can you advise if it is possible to enable LESModel with this solver? I appreciate if you tell me the steps that I need to take.

I have a rough idea that a few files in the opt/openfoam211 directory have to change, and there are some commands involved. For example I may have to #include "LESModel.H" in buoyantBoussinesqSimpleFoam.C under opt/openfoam211/applications/solvers/heatTransfer/buoyantBoussinesqSimpleFoam. But this is probably not the only step!

Many Thanks
amir.a.aliabadi is offline   Reply With Quote

Old   March 10, 2013, 05:46
Default
  #2
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 294
Rep Power: 11
Lieven will become famous soon enough
Hey Amir,

This wouldn't make sense. The simpleFoam solver is a steady state solver (not time derivative in its equations) while LES requires by definition a transient solver.

So, if you want to run a simulation with LES, you should switch to pisoFoam or pimpleFoam. If you are not interested in the transient behaviour but only in the averaged flow field, you can consider using functionObjects.

Cheers,

L
Lieven is offline   Reply With Quote

Old   March 10, 2013, 14:11
Default
  #3
New Member
 
Amir Abbas Aliabadi
Join Date: Mar 2013
Posts: 17
Rep Power: 3
amir.a.aliabadi is on a distinguished road
Hi and Thank You Lieven,

That is a good point. I think I have to start with modifying the buoyantBoussinesqPimpleFoam and create a new application that substitutes RASModel with LESModel. I am just getting a handle of creating a new application and linking libraries using section "3.2 Compiling applications and libraries" in the OpenFoam manual.

Cheers,
aaa
amir.a.aliabadi is offline   Reply With Quote

Old   March 10, 2013, 16:05
Default
  #4
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 294
Rep Power: 11
Lieven will become famous soon enough
Well, that's the nice thing of the piso and pimple solvers. The turbulence modelling is generic meaning that both RANS and LES models can be chosen. Just have a look at the tutorials of these solvers on how to do this exactly (you need to set the proper constant/...Dict dictionaries. If any questions arise, feel free to post them.

Cheers,

Lieven
Lieven is offline   Reply With Quote

Old   March 10, 2013, 18:18
Default
  #5
New Member
 
Amir Abbas Aliabadi
Join Date: Mar 2013
Posts: 17
Rep Power: 3
amir.a.aliabadi is on a distinguished road
Thank You Lieven,

It is finally working! I started with channel395 (1 eqn LES) and hotRoom (k-e RAS) and combined the functionalities of both tutorials to be able to create a solver for natural convection problems. A tricky part was to include all proper addresses for header files (*.H) under make/files make/options. The System files, 0 files, and Constant files also needed to be adjusted. I have called this solver: buoyantBoussinesqPimpleLESFoam. If anyone is interested please let me know.

Regards,
aaa
amir.a.aliabadi is offline   Reply With Quote

Old   December 24, 2013, 06:43
Default
  #6
Member
 
Peter
Join Date: Nov 2011
Posts: 43
Rep Power: 4
palmerlee is on a distinguished road
Quote:
Originally Posted by amir.a.aliabadi View Post
Thank You Lieven,

It is finally working! I started with channel395 (1 eqn LES) and hotRoom (k-e RAS) and combined the functionalities of both tutorials to be able to create a solver for natural convection problems. A tricky part was to include all proper addresses for header files (*.H) under make/files make/options. The System files, 0 files, and Constant files also needed to be adjusted. I have called this solver: buoyantBoussinesqPimpleLESFoam. If anyone is interested please let me know.

Regards,
aaa
Hi, aaa!

I am trying to use buoyantBoussinesqPimpleFoam with LES too. Could you please let me know if your buoyantBoussinesqPimpleLESFoam gives good results in LES simulation? So that I can determine that whether or not the modified buoyantBoussinesqPimpleFoam solver is suitable to my case or other LES simulations.

If the solver is suitable to LES, could you let me know which part of the original buoyantBoussinesqPimpleFoam solver need to be modified besides the Make dir and "RASModel" in createFields file?

Thank you!

palmerlee
palmerlee is offline   Reply With Quote

Old   December 24, 2013, 06:44
Default
  #7
Member
 
Peter
Join Date: Nov 2011
Posts: 43
Rep Power: 4
palmerlee is on a distinguished road
Quote:
Originally Posted by amir.a.aliabadi View Post
Thank You Lieven,

It is finally working! I started with channel395 (1 eqn LES) and hotRoom (k-e RAS) and combined the functionalities of both tutorials to be able to create a solver for natural convection problems. A tricky part was to include all proper addresses for header files (*.H) under make/files make/options. The System files, 0 files, and Constant files also needed to be adjusted. I have called this solver: buoyantBoussinesqPimpleLESFoam. If anyone is interested please let me know.

Regards,
aaa
Hi, aaa!

I am trying to use buoyantBoussinesqPimpleFoam with LES too. Could you please let me know if your buoyantBoussinesqPimpleLESFoam gives good results in LES simulation? So that I can determine that whether or not the modified buoyantBoussinesqPimpleFoam solver is suitable to my case or other LES simulations.

If the solver is suitable to LES, could you let me know which part of the original buoyantBoussinesqPimpleFoam solver need to be modified besides the Make dir and "RASModel" in createFields file?

Thank you!

palmerlee
palmerlee is offline   Reply With Quote

Old   December 27, 2013, 01:23
Default
  #8
Member
 
Thangam Natarajan
Join Date: Dec 2010
Location: Perth
Posts: 35
Rep Power: 6
Thangam is on a distinguished road
Quote:
Originally Posted by amir.a.aliabadi View Post
Thank You Lieven,

It is finally working! I started with channel395 (1 eqn LES) and hotRoom (k-e RAS) and combined the functionalities of both tutorials to be able to create a solver for natural convection problems. A tricky part was to include all proper addresses for header files (*.H) under make/files make/options. The System files, 0 files, and Constant files also needed to be adjusted. I have called this solver: buoyantBoussinesqPimpleLESFoam. If anyone is interested please let me know.

Regards,
aaa
Hi,

I have tried something similar but I have modified the buoyantBoussinesqPisoFoam for the LES capability and I have managed to compile it but still in the process of evaluating it. I found this link very useful for this modification http://openfoamwiki.net/index.php/Bu...sinesqPisoFoam however, some more changes had to be made pertaining to the calculations of p_rgh. I have attched the solver here I would be pleased to have some feedback from the foamers. Also it would be interesting to compare your solver(with PIMPLE equation) if you could make it available on the forum.

Cheers.
Attached Files
File Type: gz buoyantBoussinesqPisoFoam.tar.gz (6.1 KB, 3 views)
Thangam is offline   Reply With Quote

Old   December 27, 2013, 03:58
Default
  #9
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 782
Rep Power: 11
Bernhard is on a distinguished road
Hi Thangham

Some hints and question
1. Make sure your solver compiles, without additional work. For me, readTransportProperties.H was missing. Also, update Make/files: now, you would be overwriting your original buoyantBoussinesqPisoFoam, which is undesirable for people downloading the source.
2. wclean would make the tarbal neat.
3. Also, write the solver to $FOAM_USER_APPBIN.

Some questions
1. Which version of OpenFOAM are you using?
2. Which solver did you start from?
3. What specific changes did you make to p_rgh?
Bernhard is offline   Reply With Quote

Old   December 27, 2013, 04:48
Default
  #10
Member
 
Thangam Natarajan
Join Date: Dec 2010
Location: Perth
Posts: 35
Rep Power: 6
Thangam is on a distinguished road
Quote:
Originally Posted by Bernhard View Post
Hi Thangham

Some hints and question
1. Make sure your solver compiles, without additional work. For me, readTransportProperties.H was missing. Also, update Make/files: now, you would be overwriting your original buoyantBoussinesqPisoFoam, which is undesirable for people downloading the source.
2. wclean would make the tarbal neat.
3. Also, write the solver to $FOAM_USER_APPBIN.

Some questions
1. Which version of OpenFOAM are you using?
2. Which solver did you start from?
3. What specific changes did you make to p_rgh?


Hi Bernhard,

Thanks for your reply.

1. Make sure your solver compiles, without additional work. For me, readTransportProperties.H was missing. Also, update Make/files: now, you would be overwriting your original buoyantBoussinesqPisoFoam, which is undesirable for people downloading the source. - Yes, the solver compiles without any additional work. I dont understand the significance of readTransportProperties.H.On a quick check most of the solvers in heat transfer dont use this file.(please enlighten)

2. wclean would make the tarbal neat.
- My bad. Would do it.

3. Also, write the solver to $FOAM_USER_APPBIN. - Yes, copied.


Some questions
1. Which version of OpenFOAM are you using?
- version 2.1.x

2. Which solver did you start from? - I started with the buoyantBoussinesqPisoFoam solver which was available in a 1.6.x git repository and followed the instructions on the openfoam wiki site (http://openfoamwiki.net/index.php/Bu...sinesqPisoFoam) to have the LES capability.

3. What specific changes did you make to p_rgh? - Though the code compiled without any warnings, when I tried to run the case with this solver, I got the error :
Code:
--> FOAM FATAL IO ERROR: 
keyword laplacian((1|A(U)),p) is undefined in dictionary 
"/home/thangam/Documents/LES_dec23/system/fvSchemes::laplacianSchemes"

file: /home/thangam/Documents/LES_dec23/system/fvSchemes::laplacianSchemes from line 48 to line 56.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

FOAM exiting
The solver was reading laplacian((1|A(U)),p) though I had laplacian((1|A(U)),p_rgh). Though I had no clue why this was happening, I tried to edit the pEqn.H to its present form. And with this current form, I believe im solving for p_rgh twice! Im ignorant about where Im going wrong.
Thangam is offline   Reply With Quote

Old   December 27, 2013, 05:50
Default
  #11
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 782
Rep Power: 11
Bernhard is on a distinguished road
All of the solvers use readTransportProperties.H ! Check createFields.H, line 47.

Ah, you started from the 1.6 version. Why not from the 2.1 version of buoyantBoussinesqPimpleFoam?
Check http://www.openfoam.org/archive/1.7....ease-notes.php "Modifications to multiphase and buoyant solvers". It explains why p has been replaced by p_rgh.
Bernhard is offline   Reply With Quote

Old   December 27, 2013, 06:42
Default
  #12
Member
 
Thangam Natarajan
Join Date: Dec 2010
Location: Perth
Posts: 35
Rep Power: 6
Thangam is on a distinguished road
Thanks Bernhard. I would give it a try and repost on the outcome!

cheers.
Thangam is offline   Reply With Quote

Reply

Tags
enable lesmodel

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
CGNS converters available mbeaudoin OpenFOAM Meshing & Mesh Conversion 123 April 9, 2013 09:53
Import problem ARC Open Source Meshers: Gmsh, Netgen, CGNS, ... 0 February 27, 2010 10:56
StarToFoam error Kart OpenFOAM Meshing & Mesh Conversion 1 February 4, 2010 04:38
why the solver reject it? Anyone with experience? bearcat CFX 6 April 28, 2008 14:08
Simple foam solver mardinoglu OpenFOAM Running, Solving & CFD 0 November 13, 2006 06:25


All times are GMT -4. The time now is 18:18.