# About chtMultiRegionFoam in parallel (v1.6)

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

 September 9, 2009, 22:31 About chtMultiRegionFoam in parallel (v1.6) #1 New Member   Zheng.Zhi Join Date: Jul 2009 Location: LanZhou China Posts: 10 Rep Power: 10 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!

 September 10, 2009, 04:37 #2 Super Moderator   Mattijs Janssens Join Date: Mar 2009 Posts: 1,419 Rep Power: 18 Do you get this error running non-parallel as well?

 September 10, 2009, 05:14 #3 New Member   Zheng.Zhi Join Date: Jul 2009 Location: LanZhou China Posts: 10 Rep Power: 10 Yes，maybe the problem is the wall function needs wallFvPatch , but the directMappedWall is wallPolyPatch ?

 September 10, 2009, 07:25 #4 Super Moderator   Mattijs Janssens Join Date: Mar 2009 Posts: 1,419 Rep Power: 18 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.

 September 15, 2009, 06:00 #5 New Member   Xinyuan FAN Join Date: Sep 2009 Location: Beijing Posts: 13 Rep Power: 10 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.

 September 15, 2009, 10:47 #6 Super Moderator   Mattijs Janssens Join Date: Mar 2009 Posts: 1,419 Rep Power: 18 I've just pushed a lot of changes to 1.6.x to do with wall-type recognition. Could you try again? Thanks, Mattijs

 September 15, 2009, 21:50 #7 New Member   Xinyuan FAN Join Date: Sep 2009 Location: Beijing Posts: 13 Rep Power: 10 Ok, I will give a reply when I try again.

 September 16, 2009, 01:46 #8 New Member   Xinyuan FAN Join Date: Sep 2009 Location: Beijing Posts: 13 Rep Power: 10 The problem has been solved. The multiRegionHeater case can be running in both non-parallel and parallel. Thank you for your update.

 October 14, 2009, 03:39 #9 New Member   Carel Join Date: Mar 2009 Posts: 5 Rep Power: 10 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>>>> 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

 October 14, 2009, 08:20 #10 New Member   Carel Join Date: Mar 2009 Posts: 5 Rep Power: 10 ..never mind, just did not read the instructions! It is working now.

 November 16, 2009, 13:46 #11 Member   Tobias Holzinger Join Date: Mar 2009 Location: Munich, Germany Posts: 46 Rep Power: 10 Hello Mattijs, are there other BC's like directMappedWall to make two regions interact? Thanks Tobias

 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

 Similar Threads Thread Thread Starter Forum Replies Last Post albcem OpenFOAM Bugs 17 April 28, 2013 23:44 asaha OpenFOAM Running, Solving & CFD 12 July 4, 2012 22:51 Peter CFX 10 May 14, 2011 06:17 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58 Amitava Majumdar Main CFD Forum 0 January 5, 1999 13:00

All times are GMT -4. The time now is 02:16.