|
[Sponsors] |
October 30, 2011, 19:11 |
Segmentation Fault
|
#1 |
Member
Shawn
Join Date: Oct 2011
Posts: 56
Rep Power: 15 |
I ran into a "Segmentation Fault" that's preventing me from running pimpleDyMFoam. I'm not trying to run in parallel.
My case uses a pretty coarse grid that consists of a 1-cell high square with a round hole, which has a round 1-cell high disc in it that has a blade shaped object in the middle. It's a ggi setup, just a test to get a case running then I can change my geometry to my turbine. I don't get any error message other than "Segmentation Fault": Code:
/*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM Extend Project: Open source CFD | | \\ / O peration | Version: 1.6-ext | | \\ / A nd | Web: www.extend-project.de | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 1.6-ext Exec : pimpleDyMFoam Date : Oct 30 2011 Time : 18:59:33 Host : ubuntu-10 PID : 23326 Case : /home/shawn/Project/vawt nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create dynamic mesh for time = 0 Selecting dynamicFvMesh mixerGgiFvMesh void mixerGgiFvMesh::addZonesAndModifiers() : Zones and modifiers already present. Skipping. Mixer mesh: origin: (0 0 0) axis : (0 0 1) rpm : -60 Reading field p Reading field U Reading/calculating face flux field phi Initializing the GGI interpolator between master/shadow patches: rotorggi/statorggi Selecting incompressible transport model Newtonian Selecting turbulence model type RASModel Selecting RAS turbulence model kOmegaSST kOmegaSSTCoeffs { alphaK1 0.85034; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.85616; gamma1 0.5532; gamma2 0.4403; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; c1 10; Cmu 0.09; } Reading field rAU if present Starting time loop Courant Number mean: 0.18930684 max: 1.5164333 velocity magnitude: 1 deltaT = 0.0003 Time = 0.0003 Segmentation fault Regards, - Shawn |
|
October 31, 2011, 09:41 |
|
#2 |
Senior Member
David Boger
Join Date: Mar 2009
Location: Penn State Applied Research Laboratory
Posts: 146
Rep Power: 17 |
Can you run under the gdb debugger? Something like
Code:
% gdb pimpleDyMFoam (gdb) run (gdb) where
__________________
David A. Boger |
|
October 31, 2011, 13:26 |
|
#3 |
Member
Shawn
Join Date: Oct 2011
Posts: 56
Rep Power: 15 |
Hi boger,
I ran the gdb debugger: Code:
shawn@ubuntu-10:~/Project/vawt$ gdb pimpleDyMFoam GNU gdb (GDB) 7.1-ubuntu Copyright (C) 2010 Free Software Foundation, Inc. License GPLv3+: GNU GPL version 3 or later <http://gnu.org/licenses/gpl.html> This is free software: you are free to change and redistribute it. There is NO WARRANTY, to the extent permitted by law. Type "show copying" and "show warranty" for details. This GDB was configured as "x86_64-linux-gnu". For bug reporting instructions, please see: <http://www.gnu.org/software/gdb/bugs/>... Reading symbols from /usr/lib/OpenFOAM-1.6-ext/applications/bin/pimpleDyMFoam...(no debugging symbols found)...done. (gdb) run Starting program: /usr/lib/OpenFOAM-1.6-ext/applications/bin/pimpleDyMFoam [Thread debugging using libthread_db enabled] /*---------------------------------------------------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM Extend Project: Open source CFD | | \\ / O peration | Version: 1.6-ext | | \\ / A nd | Web: www.extend-project.de | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ Build : 1.6-ext Exec : /usr/lib/OpenFOAM-1.6-ext/applications/bin/pimpleDyMFoam Date : Oct 31 2011 Time : 13:18:07 Host : ubuntu-10 PID : 2345 Case : /home/shawn/Project/vawt nProcs : 1 SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create dynamic mesh for time = 0 Selecting dynamicFvMesh mixerGgiFvMesh void mixerGgiFvMesh::addZonesAndModifiers() : Zones and modifiers already present. Skipping. Mixer mesh: origin: (0 0 0) axis : (0 0 1) rpm : -60 Reading field p Reading field U Reading/calculating face flux field phi Initializing the GGI interpolator between master/shadow patches: rotorggi/statorggi Selecting incompressible transport model Newtonian Selecting turbulence model type RASModel Selecting RAS turbulence model kOmegaSST kOmegaSSTCoeffs { alphaK1 0.85034; alphaK2 1; alphaOmega1 0.5; alphaOmega2 0.85616; gamma1 0.5532; gamma2 0.4403; beta1 0.075; beta2 0.0828; betaStar 0.09; a1 0.31; c1 10; Cmu 0.09; } Reading field rAU if present Starting time loop Courant Number mean: 0.18930684 max: 1.5164333 velocity magnitude: 1 deltaT = 0.0003 Creating ggi check Time = 0.0003 Program received signal SIGSEGV, Segmentation fault. 0x00007ffff7adcca3 in Foam::mixerGgiFvMesh::calcMovingMasks() const () from /usr/lib/OpenFOAM-1.6-ext/lib/libdynamicFvMesh.so (gdb) where #0 0x00007ffff7adcca3 in Foam::mixerGgiFvMesh::calcMovingMasks() const () from /usr/lib/OpenFOAM-1.6-ext/lib/libdynamicFvMesh.so #1 0x00007ffff7addabd in Foam::mixerGgiFvMesh::movingPointsMask() const () from /usr/lib/OpenFOAM-1.6-ext/lib/libdynamicFvMesh.so #2 0x00007ffff7addb00 in Foam::mixerGgiFvMesh::update() () from /usr/lib/OpenFOAM-1.6-ext/lib/libdynamicFvMesh.so #3 0x000000000041772f in ?? () #4 0x00007ffff3ba5c4d in __libc_start_main () from /lib/libc.so.6 #5 0x0000000000415399 in ?? () #6 0x00007fffffffd998 in ?? () #7 0x000000000000001c in ?? () #8 0x0000000000000001 in ?? () #9 0x00007fffffffddd2 in ?? () #10 0x0000000000000000 in ?? () Regards, Shawn |
|
October 31, 2011, 13:37 |
|
#4 |
Senior Member
David Boger
Join Date: Mar 2009
Location: Penn State Applied Research Laboratory
Posts: 146
Rep Power: 17 |
You actually want to read it "backwards": #0 is your culprit: calcMovingMasks. It would be *much* better if you could repeat the same exercise using the dbg-compiled version of OpenFOAM, but if you look in dynamicMesh/dynamicFvMesh/mixerGgiFvMesh/mixerGgiFvMesh.C for calcMovingMasks, you might start to get some idea of where things might go wrong. For example, do you have "static" and "moving" keywords defined in your "slider" dictionary and a "movingCells" cellZone?
__________________
David A. Boger |
|
October 31, 2011, 14:59 |
|
#5 |
Member
Shawn
Join Date: Oct 2011
Posts: 56
Rep Power: 15 |
movingCells: that was the problem. I hadn't realize keeping the same name was required.
Lesson learned: how to use the debugger Lesson learned: make sure not to change names unless you know what the effect will be 3 cheers for boger! One other quick unrelated question (since the case now runs and I admit I did a bit of a happy dance), is there a way to specify what directory the results are written to? It would be nice if I could have a "results" directory where all the data is stored. I didn't see an option for this in controlDict where all the other I/O params are specified. - Shawn |
|
October 31, 2011, 15:32 |
|
#6 |
Senior Member
David Boger
Join Date: Mar 2009
Location: Penn State Applied Research Laboratory
Posts: 146
Rep Power: 17 |
Not that I've ever noticed, but it's probably better to start a different thread with that question.
__________________
David A. Boger |
|
October 31, 2011, 15:38 |
|
#7 |
Member
Shawn
Join Date: Oct 2011
Posts: 56
Rep Power: 15 |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Segmentation fault when running dieselFoam or dieselEngineFoam in parallel | francesco | OpenFOAM Bugs | 4 | May 2, 2017 22:59 |
Segmentation fault in interFoam run through openMPI | voingiappone | OpenFOAM | 16 | November 2, 2011 07:49 |
forrtl: severe (174): SIGSEGV, segmentation fault occurred | therockyy | FLOW-3D | 7 | January 19, 2011 23:52 |
ParaView segmentation fault only for multiphase | gwierink | OpenFOAM | 9 | March 25, 2010 08:23 |
segmentation fault | usker | Siemens | 5 | March 6, 2007 00:14 |