CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

how to change code in channelFoam for RAS

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 12, 2012, 14:47
Default how to change code in channelFoam for RAS
  #1
Member
 
Join Date: Jun 2012
Posts: 65
Rep Power: 4
conceptone is on a distinguished road
Hi everyone, I wanna use channelFoam with RAS model. However, the solver seems to be designed specially for LES, which leads to incredible large Courant number and pressure, pressure gradient and velocity as below then OpenFoam crashes, so I hope someone can tell me how to change the code in solver for RAS, thanks!

Time = 0.18

Debug:
gSum(mesh.V().field())16
gSum(sumPhi)4.84696e+66
gMax(sumPhi/mesh.V().field())4.12859e+69

Courant Number mean: 3.02935e+63 max: 4.12859e+67
DILUPBiCG: Solving for epsilon, Initial residual = 1, Final residual = 19.3092, No Iterations 1001
bounding epsilon, min: -2.73732e+98 max: 8.22502e+99 average: 1.61408e+95
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 758720, No Iterations 1001
bounding k, min: -3.0437e+89 max: 3.58778e+97 average: 5.9839e+92
#0 Foam::error:rintStack(Foam::Ostream&) in "/usr/apps1/openfoam-2.1.1/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/usr/apps1/openfoam-2.1.1/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#2 __restore_rt at sigaction.c:0
#3 Foam:ILUPreconditioner::calcReciprocalD(Foam::Fi eld<double>&, Foam::lduMatrix const&) in "/usr/apps1/openfoam-2.1.1/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#4 Foam:ILUPreconditioner:ILUPreconditioner(Foam: :lduMatrix::solver const&, Foam::dictionary const&) in "/usr/apps1/openfoam-2.1.1/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#5 Foam::lduMatrix:reconditioner::addasymMatrixCons tructorToTable<Foam:ILUPreconditioner>::New(Foam ::lduMatrix::solver const&, Foam::dictionary const&) in "/usr/apps1/openfoam-2.1.1/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#6 Foam::lduMatrix:reconditioner::New(Foam::lduMatr ix::solver const&, Foam::dictionary const&) in "/usr/apps1/openfoam-2.1.1/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#7 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/usr/apps1/openfoam-2.1.1/OpenFOAM-2.1.1/platforms/linux64Gcc44DPOpt/lib/libOpenFOAM.so"
#8 Foam::fvMatrix<Foam::Vector<double> >::solve(Foam::dictionary const&) in "/usr/erc/people/liao23/OpenFOAM/liao23-2.1.1/platforms/linux64Gcc44DPOpt/bin/mychannelFoam_RAS"
#9 Foam::fvMatrix<Foam::Vector<double> >::solve() in "/usr/erc/people/liao23/OpenFOAM/liao23-2.1.1/platforms/linux64Gcc44DPOpt/bin/mychannelFoam_RAS"
#10 main in "/usr/erc/people/liao23/OpenFOAM/liao23-2.1.1/platforms/linux64Gcc44DPOpt/bin/mychannelFoam_RAS"
#11 __libc_start_main in "/lib64/libc.so.6"
#12 Foam::UOPstream::write(char) in "/usr/erc/people/liao23/OpenFOAM/liao23-2.1.1/platforms/linux64Gcc44DPOpt/bin/mychannelFoam_RAS"
conceptone is offline   Reply With Quote

Old   December 12, 2012, 15:49
Default
  #2
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 294
Rep Power: 11
Lieven will become famous soon enough
Hi conceptone,

channelFoam is in the end an extension of pisoFoam. So just have a look at how the turbulence is implemented in pisoFoam and modify it accordingly in the channelFoam solver.

In summary, you need to modify createFields.H, the include statements in channelFoam.C, and of course the momentum equation. To compile it afterwards, have a look at the Make/option file of pisoFoam as well...

Cheers,


L
Lieven is offline   Reply With Quote

Old   December 12, 2012, 16:41
Default
  #3
Member
 
Join Date: Jun 2012
Posts: 65
Rep Power: 4
conceptone is on a distinguished road
Thanks Lieven, I guess what you mentioned is the declaration of that pointer in createFields.H, which I have done below and in solver. If I didn't do this modification, the solver even can't be compiled well. However, my issue is that channelFoam returns the very large Courant No. and pressure and velocities, which exceeds the extent of C++ calculation capability so openfoam crashed after runs some time...I don't know whether there are bugs here or other codes need to be changed..

Modified Coding:
autoPtr<incompressible::turbulenceModel> sgsModel
(
incompressible::turbulenceModel::New(U, phi, laminarTransport)
);

#include "RASModel.H"
#include "turbulenceModel.H"
(I've already deleted #include "LESModel.H" in solver.C)

fvVectorMatrix UEqn
(
fvm::ddt(U)
+ fvm::div(phi, U)
+ sgsModel->divDevReff(U)
==
flowDirection*gradP
);

Thanks
conceptone is offline   Reply With Quote

Old   December 13, 2012, 06:09
Default
  #4
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 294
Rep Power: 11
Lieven will become famous soon enough
That's indeed how you needed to change it.

The problem with the courant number is not related to the solver but to your time step. You can try two things to solve it:
1. Use a small, constant time step such that the max courant number < 1 at all times
2. Enable variable time stepping based on courant number control as explained in http://www.idurun.com/?p=371 . This way you can use the maximal "allowable" time step.
Both approaches work with RANS and LES

Regards,

L
Lieven is offline   Reply With Quote

Old   December 13, 2012, 16:25
Default
  #5
Member
 
Join Date: Jun 2012
Posts: 65
Rep Power: 4
conceptone is on a distinguished road
Hi Lieven, yep, the problem is done, it turns out the time step leads to this. I tried small time step before, but not small enough. This time I try really small one, which works. This may turn out LES's advantage in time step compared with RAS.
Thanks so much!
conceptone is offline   Reply With Quote

Reply

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
Radiation interface hinca CFX 15 January 26, 2014 18:11
Cfd code for phase change model mohsen.kh Main CFD Forum 0 June 10, 2009 09:07
Multicomponent fluid Andrea CFX 2 October 11, 2004 06:12
Design Integration with CFD? John C. Chien Main CFD Forum 19 May 17, 2001 16:56
What is the Better Way to Do CFD? John C. Chien Main CFD Forum 54 April 23, 2001 09:10


All times are GMT -4. The time now is 01:07.