CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Bugs

About chtMultiRegionFoam in parallel (v1.6)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 9, 2009, 23:31
Default About chtMultiRegionFoam in parallel (v1.6)
  #1
New Member
 
Zheng.Zhi
Join Date: Jul 2009
Location: Beijing China
Posts: 9
Rep Power: 7
Zheng.Zhi is on a distinguished road
When I use chtMultiRegionFoam to solve multiRegionHeater case in parallel, I want to set topAir_to_heater with kqRWallFunction and epsilonWallFunction boundary conditions. But there was the error said topAir_to_heater must be wall instead of directMappedWall. Is there any method to solver this problem?
Thanks!
Zheng.Zhi is offline   Reply With Quote

Old   September 10, 2009, 05:37
Default
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
Do you get this error running non-parallel as well?
mattijs is offline   Reply With Quote

Old   September 10, 2009, 06:14
Default
  #3
New Member
 
Zheng.Zhi
Join Date: Jul 2009
Location: Beijing China
Posts: 9
Rep Power: 7
Zheng.Zhi is on a distinguished road
Yes,maybe the problem is the wall function needs wallFvPatch , but the directMappedWall is wallPolyPatch ?
Zheng.Zhi is offline   Reply With Quote

Old   September 10, 2009, 08:25
Default
  #4
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
directMappedWall is derived from wallPolyPatch. The problem was that the finite volume equivalent wasn't derived from wallFvPatch. I pushed a fix to 1.6.x. Give it a go.

Thanks for reporting.
mattijs is offline   Reply With Quote

Old   September 15, 2009, 07:00
Default
  #5
New Member
 
Xinyuan FAN
Join Date: Sep 2009
Location: Beijing
Posts: 13
Rep Power: 7
autumn1012 is on a distinguished road
Here is another problem when I tried 1.6.x,

Solving for fluid region bottomAir
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Ux, Initial residual = 2.211858e-16, Final residual = 2.211858e-16, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 6.771384e-09, No Iterations 22
DILUPBiCG: Solving for Uz, Initial residual = 1.036037e-15, Final residual = 1.036037e-15, No Iterations 0
DILUPBiCG: Solving for h, Initial residual = 0.6044857, Final residual = 8.30665e-09, No Iterations 40
Min/max T:300 300
GAMG: Solving for p, Initial residual = 1, Final residual = 0.005459487, No Iterations 2
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (bottomAir): sum local = 0.001237545, global = 4.109187e-06, cumulative = 4.109187e-06
GAMG: Solving for p, Initial residual = 0.6006277, Final residual = 6.905954e-09, No Iterations 27
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (bottomAir): sum local = 2.018032e-09, global = -4.377309e-11, cumulative = 4.109143e-06
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib64/libc.so.6"
#3 Foam::compressible::RASModels::epsilonWallFunction FvPatchScalarField::updateCoeffs() in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#4 Foam::compressible::RASModels::kEpsilon::correct() in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/lib/linux64GccDPOpt/libcompressibleRASModels.so"
#5 main in "/home/fxy/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linux64GccDPOpt/chtMultiRegionFoam"
#6 __libc_start_main in "/lib64/libc.so.6"
#7 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception

Then I checked epsilonWallFunctionFvPatchScalarField and found there are some calculations like this

const scalarField& y = rasModel.y()[patch().index()];

forAll(nutw, faceI)
{
...
epsilon[faceCellI] = Cmu75*pow(k[faceCellI], 1.5)/(kappa_*y[faceI]);
...
}

So I modified chtMultiRegionFoam to output rasModel.y() of patch like bottomAir_to_heater, then I found all of them are 0, so the above error happened.

Is there any method to solver this problem? Thanks.
autumn1012 is offline   Reply With Quote

Old   September 15, 2009, 11:47
Default
  #6
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
I've just pushed a lot of changes to 1.6.x to do with wall-type recognition. Could you try again?

Thanks,

Mattijs
mattijs is offline   Reply With Quote

Old   September 15, 2009, 22:50
Default
  #7
New Member
 
Xinyuan FAN
Join Date: Sep 2009
Location: Beijing
Posts: 13
Rep Power: 7
autumn1012 is on a distinguished road
Ok, I will give a reply when I try again.
autumn1012 is offline   Reply With Quote

Old   September 16, 2009, 02:46
Default
  #8
New Member
 
Xinyuan FAN
Join Date: Sep 2009
Location: Beijing
Posts: 13
Rep Power: 7
autumn1012 is on a distinguished road
The problem has been solved. The multiRegionHeater case can be running in both non-parallel and parallel. Thank you for your update.
autumn1012 is offline   Reply With Quote

Old   October 14, 2009, 04:39
Default
  #9
cvv
New Member
 
Carel
Join Date: Mar 2009
Posts: 5
Rep Power: 7
cvv is on a distinguished road
Hi,

Can someone perhaps post a link to the tutorial for chtMultiRegionFoam in 1.6? I tried the one from 1.5 but get the following error when I run the solver:
Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>


Not Implemented
Trying to construct an genericFvPatchField on patch bottomAir_to_rightSolid of field h#0 Foam::error:rintStack(Foam::Ostream&) at /opt/Op enFOAM/r1.6/debug/OpenFOAM-1.6/src/OSspecific/POSIX/printStack.C:203

I read on another thread that this may be due to the boundary type. In this case the type is solidWallTemperatureCoupled. Was this changed in 1.6?

Regards
Carel
cvv is offline   Reply With Quote

Old   October 14, 2009, 09:20
Default
  #10
cvv
New Member
 
Carel
Join Date: Mar 2009
Posts: 5
Rep Power: 7
cvv is on a distinguished road
..never mind, just did not read the instructions!

It is working now.
cvv is offline   Reply With Quote

Old   November 16, 2009, 13:46
Default
  #11
Member
 
Tobias Holzinger
Join Date: Mar 2009
Location: Munich, Germany
Posts: 46
Rep Power: 7
woody is on a distinguished road
Hello Mattijs,

are there other BC's like directMappedWall to make two regions interact?

Thanks

Tobias
woody 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
Parallel Moving Mesh Bug for Multi-patch Case albcem OpenFOAM Bugs 17 April 29, 2013 00:44
Script to Run Parallel Jobs in Rocks Cluster asaha OpenFOAM Running, Solving & CFD 12 July 4, 2012 23:51
HP MPI warning...Distributed parallel processing Peter CFX 10 May 14, 2011 07:17
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 03:58
Parallel Computing Classes at San Diego Supercomputer Center Jan. 20-22 Amitava Majumdar Main CFD Forum 0 January 5, 1999 13:00


All times are GMT -4. The time now is 21:38.