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

Problem with icoDyMFoam tutorial

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 24, 2007, 11:19
Default I just installed OpenFOAM-1.4
  #1
New Member
 
Mattias Liefvendahl
Join Date: Mar 2009
Posts: 5
Rep Power: 9
matlie is on a distinguished road
I just installed OpenFOAM-1.4 and tested the tutorials for icoFoam and oodles, which worked fine.

The tutorial for icoDyMFoam crashes however, see below for the error message.

The error seems to occur in the polyMesh::calcDirections function. Maybe it is the case/mesh/boundary conditions which are not set up correctly. They seem to be the same as the corresponding tutorials in versions 1.2 and 1.3, however. These tutorials work fine on my machine by the way.

checkMesh complains about skew faces, but that shouldn't cause this kind of crash.

This seems to be related to the thread by Joakim Möller about SetField.

So - what can be the problem ?

Regards,
Mattias


/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : icoDyMFoam .. movingCone
Date : Apr 24 2007
Time : 17:18:13
Host : matlie
PID : 3240
Root : ..
Case : movingCone
Nprocs : 1
Create time

Create mesh

Selecting dynamicFvMesh dynamicMotionSolverFvMesh
Selecting motion solver: componentLaplacian
#0 Foam::error::printStack(Foam:stream&)
#1 Foam::sigFpe::sigFpeHandler(int)
#2 Uninterpreted: [0xffffe420]
#3 Foam::polyMesh::calcDirections() const
#4 Foam::polyMesh::directions() const
#5 Foam::polyMesh::nSolutionD() const
#6 Foam::polyMesh::nGeometricD() const
#7 Foam::twoDPointCorrector::twoDPointCorrector(Foam: :polyMesh const&)
#8 Foam::motionSolver::motionSolver(Foam::polyMesh const&)
#9 Foam::fvMotionSolver::fvMotionSolver(Foam::polyMes h const&)
#10 Foam::componentLaplacianFvMotionSolver::componentL aplacianFvMotionSolver(Foam::p olyMesh const&, Foam::Istream&)
#11 Foam::motionSolver::adddictionaryConstructorToTabl e<foam::componentlaplacianfvmo tionsolver>::New(Foam::polyMesh const&, Foam::Istream&)
#12 Foam::motionSolver::New(Foam::polyMesh const&)
#13 Foam::dynamicMotionSolverFvMesh::dynamicMotionSolv erFvMesh(Foam::IOobject const&)
#14 Foam::dynamicFvMesh::addIOobjectConstructorToTable <foam::dynamicmotionsolverfvme sh>::New(Foam::IOobject const&)
#15 Foam::dynamicFvMesh::New(Foam::IOobject const&)
#16 main
#17 __libc_start_main
#18 __gxx_personality_v0 at ../sysdeps/i386/elf/start.S:122
Floating exception (core dumped)
matlie is offline   Reply With Quote

Old   April 24, 2007, 15:49
Default Are you running single or doub
  #2
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 14
henry is on a distinguished road
Are you running single or double precision? If single try double.
henry is offline   Reply With Quote

Old   April 24, 2007, 16:01
Default There is a problem with calcDi
  #3
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 14
henry is on a distinguished road
There is a problem with calcDirections for meshes in which all patches of type empty contain no faces, as is the case for this tutorial. One option is to change the patch type of the axis in the blockMeshDict file or change the logic in calcDirections in OpenFOAM-1.4/src/OpenFOAM/meshes/polyMesh/polyMesh.C by moving

nEmptyPatches++;

from line 66 to line 70, i.e. inside the

if (boundaryMesh()[patchi].size())

However, even after this change this case will still not run correctly single precision because the accumulation of error causes problems with the mesh motion.

Henry
henry is offline   Reply With Quote

Old   April 25, 2007, 09:14
Default Thanks Henry for the quick res
  #4
New Member
 
Mattias Liefvendahl
Join Date: Mar 2009
Posts: 5
Rep Power: 9
matlie is on a distinguished road
Thanks Henry for the quick response.

1. I am running in double precision.
2. I tried to change the patch type in blockMeshDict from 'empty' to 'patch'. It still didn't work (same error message).
3. I cannot try your suggestion of changing the code since I cannot recompile libOpenFOAM.so since the compiler cannot find 'demangle.h'. I saw that other people have had this problem. I couldn't fix it. I run Ubuntu 6.10.

Mattias
matlie is offline   Reply With Quote

Old   April 25, 2007, 09:37
Default 2. I have changed the tutorial
  #5
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 14
henry is on a distinguished road
2. I have changed the tutorial case so that it works without my suggested change to calcDirections:
movingCone.tbz2

Unpack using tar xjf movingCone.tbz2

3. I do not have any experience with Ubuntu Linux so cannot advise on how to install demangle.h.

Henry
henry is offline   Reply With Quote

Old   April 25, 2007, 13:15
Default Hi Mattias! I ran the tutor
  #6
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 9
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Hi Mattias!

I ran the tutorial on my SuSE box without any trouble... are you running the 32 or 64-bit OF-version?

//Eric
lillberg is offline   Reply With Quote

Old   April 26, 2007, 03:53
Default Thanks Henry, Now movingCone
  #7
New Member
 
Mattias Liefvendahl
Join Date: Mar 2009
Posts: 5
Rep Power: 9
matlie is on a distinguished road
Thanks Henry,
Now movingCone case works.
Compared to 1.3, the execution is almost six times as fast!
Is that because of the finite volume mesh motion solver ?

Eric, I'm running the 32-bit version.

/Mattias
matlie is offline   Reply With Quote

Old   April 26, 2007, 03:59
Default Yes the finite volume mesh mot
  #8
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 14
henry is on a distinguished road
Yes the finite volume mesh motion solver is much faster. For me the difference was even larger on this case.

Henry
henry is offline   Reply With Quote

Old   April 26, 2007, 04:29
Default On large FSI cases using the l
  #9
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 9
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
On large FSI cases using the laplacian solver with quadratic inverse distance diffusivity I found the fvMotionSolver to be about two times faster then the tetDecomp version. But then again I haven't look through all the code.

Is there some useful tuning for general 3D motion with preserved BL grids? Could you give a brief explanation on the different diffusivities.

Regards

/Eric
lillberg is offline   Reply With Quote

Old   April 26, 2007, 04:39
Default You may get significant perfor
  #10
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 14
henry is on a distinguished road
You may get significant performance improvements on large problems by changing/tuning the solvers. The GAMG solver has a large number of parameters which if tuned carefully can give substantial benfits.

I implemented a large number of diffusivities for the fvMotionSolver but didn't have time to play with them much. It is also very easy to create new diffusivity functions for particular type of problems if the need arises. To preserve BL grids it might be useful to use a distance to the wall function to alter the diffusivity in that region. It would be very useful for all if you can play around with some of these options and let us know your findings.

Henry
henry is offline   Reply With Quote

Old   April 26, 2007, 04:51
Default I'll do my best ;-)
  #11
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 9
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
I'll do my best ;-)
lillberg 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
MovingCone tutorial and icoDyMFoam with addingremoving mesh layers idosil OpenFOAM Running, Solving & CFD 30 July 29, 2016 05:42
Mesh Problem with icoDyMFoam yuhai OpenFOAM Running, Solving & CFD 5 January 14, 2009 15:57
Problem with icoDyMFoam olivier OpenFOAM Running, Solving & CFD 13 December 19, 2008 10:03
Problem starting with icoDyMFoam kassiotis OpenFOAM Running, Solving & CFD 1 March 12, 2007 12:12
Problem with icoDyMFoam philippose OpenFOAM Running, Solving & CFD 19 March 7, 2007 13:06


All times are GMT -4. The time now is 04:06.