CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Parallel processing

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 2, 2005, 00:32
Default While decomposing the grid in
  #1
ghanshyam
Guest
 
Posts: n/a
While decomposing the grid in FoamX GUI, it gives the following error message "Type 'vectorSpace' not defined for invalidType n". What does this mean?

Also if I try to decompose by giving "decomposePar" command in a terminal, it gives following message.

--------------------------
Processor 0
Number of cells = 25119
Number of faces shared with processor 1 = 146
Number of boundary faces = 50854

Processor 1
Number of cells = 25119
Number of faces shared with processor 0 = 146
Number of faces shared with processor 2 = 146
Number of boundary faces = 50584

Processor 2
Number of cells = 25119
Number of faces shared with processor 1 = 146
Number of faces shared with processor 3 = 146
Number of boundary faces = 50584

Processor 3
Number of cells = 25118

--> FOAM FATAL IO ERROR :
Cannot find 'value' entry which is required to set the values of the default patch field.

Please add the 'value' entry to the write function of the user-defined boundary-condition
or link the boundary-condition into libfoamUtil.so

file: /OpenFOAM/shyam-1.2/run/simpleFoam/d_wyg/0/p::inlet_left from line 47 to line 48.

From function defaultFvPatchField<type>::defaultFvPatchField(con st fvPatch&, const Field<type>&, const dictionary&)
in file fields/fvPatchFields/basicFvPatchFields/default/defaultFvPatchField.C at line 127.

FOAM exiting
-----------------------

Note: This heppen when I try to decompose from '0' iteration. If I run it as serial, say for 2-3 iterations, it could decompose from '3' iteration and run in parallel. Am I doing something wrong? I am using "atmosphare" BC for "inlet_left" boundary and specifying total pressure.

Regards
GS
  Reply With Quote

Old   September 2, 2005, 03:14
Default Hello, The answer to your fir
  #2
New Member
 
Stefan Boschert
Join Date: Mar 2009
Posts: 2
Rep Power: 0
boschert is on a distinguished road
Hello,
The answer to your first question is already answerd in another thread:

By Henry Weller on Wednesday, August 24, 2005 - 01:27 am: Edit Post
I have just tried decomposePar from FoamX, there is a problem with the syntax in one of the configuration files, change vectorSpace to fixedList in OpenFOAM-1.2/applications/utilities/parallelProcessing/decomposePar/FoamX/n.cfg

Unfortunately I can not help on the second one

Stefan
boschert is offline   Reply With Quote

Old   September 2, 2005, 03:37
Default I take it your case was saved
  #3
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
I take it your case was saved from FoamX. If so it looks like FoamX is not currently including the value entry for the totalPressure BC which I will look into. There may be more problems like this from the rewite of the FoamX configuration and not everything has been tested. However, the reorganisation of FoamX has made it MUCH easier for users to fix these problems themselves but if you don't want to have a go then simply add the value entry for the totalPressure BC in the file /OpenFOAM/shyam-1.2/run/simpleFoam/d_wyg/0/p by hand.
henry is offline   Reply With Quote

Old   September 2, 2005, 04:04
Default Thanks Stefan, now I can decom
  #4
ghanshyam
Guest
 
Posts: n/a
Thanks Stefan, now I can decompose from FoamX but my second problem is not yet over.

Henry when I decompose from '0' iteration, it is not even creating '0' directory within each processor* directories. For that I manually copied '0' directory inside each processor* and tried running, I get following message:

------------------
--> FOAM FATAL IO ERROR : keyword procBoundary2to1 is undefined in dictionary "/misc/data/ea2502/OpenFOAM/shyam-1.2
un/simpleFoam/d_wyg/processor2/0/p::boundaryField"

file: /misc/data/ea2502/OpenFOAM/shyam-1.2/run/simpleFoam/d_wyg/processor2/0/p::bounda ryField from line 36 to line 6

From function dictionary::lookupEntry(const word& keyword) const
in file db/dictionary/dictionary.C at line 152.

FOAM parallel run exiting



--> FOAM FATAL IO ERROR : keyword procBoundary1to0 is undefined in dictionary "/data/ea2502/OpenFOAM/shyam-1.2/run/
mpleFoam/d_wyg/processor1/0/p::boundaryField"

file:

--> FOAM FATAL IO ERROR : keyword procBoundary3to2 is undefined in dictionary "/misc/data/ea2502/OpenFOAM/shyam-1.2
un/simpleFoam/d_wyg/processor3/0/p::boundaryField"

file: /misc/data/ea2502/OpenFOAM/shyam-1.2/run/simpleFoam/d_wyg/processor3/0/p::bounda ryField from line 36 to line 6

From function dictionary::lookupEntry(const word& keyword) const
in file db/dictionary/dictionary.C at line 152.

FOAM parallel run exiting
/data/ea2502/OpenFOAM/shyam-1.2/run/simpleFoam/d_wyg/processor1/0/p::boundaryFie ld from line 36 to line 69.

From function dictionary::lookupEntry(const word& keyword) const
in file db/dictionary/dictionary.C at line
152.
------------------

Regards
GS
  Reply With Quote

Old   September 2, 2005, 04:07
Default As I say try adding the value
  #5
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
As I say try adding the value entry to the totalPressure BC in /OpenFOAM/shyam-1.2/run/simpleFoam/d_wyg/0/p before you decompose.
henry is offline   Reply With Quote

Old   September 2, 2005, 04:34
Default This is how my pressure 'p' fi
  #6
ghanshyam
Guest
 
Posts: n/a
This is how my pressure 'p' file in '0' directory looks like:

--------------------------
wall
{
type zeroGradient;
}

plenum_inlet
{
type zeroGradient;
}

inlet_top
{
type totalPressure;
p0 uniform 82714.3;
}

frontAndBackPlanes
{
type empty;
}
}
--------------------------
It already has p0 value. Basically it is not having processor interface information which is to be given manually. Am I correct?

For the time being it is less time consuming to run for just one iteration as serial, decompose it and run it as parallel. This is possible for a small case but for a large case we should be able to run parallel right from the begning.

Regards
GS
  Reply With Quote

Old   September 2, 2005, 04:37
Default Please please please add the v
  #7
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
Please please please add the value entry to the totalPressure BC:

inlet_top
{
type totalPressure;
p0 uniform 82714.3;
value uniform 82714.3;
}

then decompose.
henry is offline   Reply With Quote

Old   September 2, 2005, 05:07
Default I am really sorry for botherin
  #8
ghanshyam
Guest
 
Posts: n/a
I am really sorry for bothering you so much. Now it works.

Thanks and regards

GS
  Reply With Quote

Old   September 5, 2005, 05:42
Default How inter processor data commu
  #9
ghanshyam
Guest
 
Posts: n/a
How inter processor data communication is done? It it done using blocking MPI calls?

Regards
GS
  Reply With Quote

Old   September 5, 2005, 05:48
Default It depends on the choice of sc
  #10
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
It depends on the choice of scheduling, without we use MPI_Bsend and with we use MPI_Send.
henry is offline   Reply With Quote

Old   September 5, 2005, 06:11
Default So data coherency is ensured?
  #11
ghanshyam
Guest
 
Posts: n/a
So data coherency is ensured? In Schwartz kind of decomposition, how many elements do you keep common across the processor interface? Or is it non-overlap kind of domain decomposition?

Regards
GS
  Reply With Quote

Old   September 5, 2005, 06:17
Default It is a non-overlap (no halo-c
  #12
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
It is a non-overlap (no halo-cells) kind of domain decomposition using only processor neighbour-neighbour data swaps and global sums and yes data coherency is ensured and there are no restrictions on the kind of decomposition you use.
henry is offline   Reply With Quote

Old   September 5, 2005, 06:23
Default Thanks Henry for the clarefica
  #13
ghanshyam
Guest
 
Posts: n/a
Thanks Henry for the clarefication.

Regards
GS
  Reply With Quote

Old   September 5, 2005, 06:41
Default Sorry for the typo in the prev
  #14
ghanshyam
Guest
 
Posts: n/a
Sorry for the typo in the previous message. How does pressure correction equation is solved? is it solved for "each sub-domain" separately or only once for the "entire" computational domain?

Regards
GS
  Reply With Quote

Old   September 5, 2005, 06:48
Default The pressure equation is ellip
  #15
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
The pressure equation is elliptic and must be solved over the whole domain implicitly. This is done in OpenFOAM by the linear solvers (ICCG, BCG, AMG) being parallelised, i.e. processor boundaries and solution parameters (alpha etc.) are updated within the solver loop for each and every iteration.
henry is offline   Reply With Quote

Old   September 8, 2005, 08:40
Default To fix the problem with the to
  #16
New Member
 
Stefan Boschert
Join Date: Mar 2009
Posts: 2
Rep Power: 0
boschert is on a distinguished road
To fix the problem with the totalPressure BC in FoamX you have to modify the file
OpenFOAM-1.2\.OpenFOAM-1.2\apps\FoamX\types\patchFields\cfd.cfg
In this file you find an entry totalPressure. There you have to insert an entry for value:

totalPressure
{
displayName "totalPressure";
description "Total Pressure";
type patchField;
options
{
type
{
default totalPressure;
}
}

entries
{
p0
{
type field;
displayName "p0";
description "Reference pressure";
}
value
{
type field;
displayName "value";
description "Field value";
}
}
}

Now FoamX should handle the file ok.

BTW: What is the value-field used for???

Regards
Stefan
boschert is offline   Reply With Quote

Old   September 8, 2005, 09:03
Default The value field is only used b
  #17
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
The value field is only used by post-processing codes which don't know about the totalPressure BC because it's in a library not linked into them.
henry is offline   Reply With Quote

Old   April 20, 2006, 14:34
Default Hi, In serial one can loop
  #18
New Member
 
Jeff Allen
Join Date: Mar 2009
Posts: 11
Rep Power: 7
jballen is on a distinguished road
Hi,

In serial one can loop through the cells of the domain as: forAll(mesh.cells(),i)....
What would be the equivalent in parallel?

Resp.
Jeff
jballen is offline   Reply With Quote

Old   September 20, 2008, 13:06
Default Hi all I tried to implement
  #19
Member
 
David Hora
Join Date: Mar 2009
Location: Zürich, Switzerland
Posts: 63
Rep Power: 7
david is on a distinguished road
Hi all

I tried to implement the GGI from OpenFOAM-1.4.1-dev into OpenFOAM-1.5 by creating a dynamic library. The case mixerGGI was computed fine, even in parallel. Unfortunately I had problems with paraFoam. At the beginning I got the following error:

************************************************** ******

[david@localhost mixerGgi]$ paraFoam
--> FOAM Warning :
From function dlLibraryTable::open(const fileName& functionLibName)
in file db/dlLibraryTable/dlLibraryTable.C at line 79
could not load /home/david/OpenFOAM/david-1.5/lib/linuxGccDPOpt/libGGI.so: undefined symbol: _ZTIN4Foam16coupledPolyPatchE


Unknown patchField type ggi for patch type genericPatch

Valid patchField types are :

8
(
symmetryPlane
empty
fixedValue
cyclic
processor
calculated
sliced
wedge
)


file: /home/david/Desktop/mixerGgi/0.006/meshPhi::insideSlider from line 1240 to line 1241.

From function fvsPatchField<type>::New(const fvPatch&, const Field<type>&, const dictionary&)
in file lnInclude/newFvsPatchField.C at line 115.

FOAM exiting

[david@localhost mixerGgi]$


************************************************** ******

I found this thread, modified system/controlDict from ("libGGI.so") to ("libOpenFOAM.so" "libGGI.so") and got:

************************************************** ******

[david@localhost mixerGgi]$ paraFoam
--> FOAM Warning :
From function dlLibraryTable::open(const fileName& functionLibName)
in file db/dlLibraryTable/dlLibraryTable.C at line 79
could not load /home/david/OpenFOAM/david-1.5/lib/linuxGccDPOpt/libGGI.so: undefined symbol: _ZN4Foam7fvPatch14initMovePointsEv


Unknown patchField type ggi for patch type genericPatch

Valid patchField types are :

8
(
symmetryPlane
empty
fixedValue
cyclic
processor
calculated
sliced
wedge
)


file: /home/david/Desktop/mixerGgi/0.006/meshPhi::insideSlider from line 1240 to line 1241.

From function fvsPatchField<type>::New(const fvPatch&, const Field<type>&, const dictionary&)
in file lnInclude/newFvsPatchField.C at line 115.

FOAM exiting

[david@localhost mixerGgi]$


************************************************** ******

Then I tried different things and found out that with LIB_LIBS=-ldynamicFvMesh in Make/options (and ("libOpenFOAM.so" "libGGI.so") in controlDict) I get the following error message in paraFoam:

************************************************** ******

[david@localhost mixerGgi]$ paraFoam


Attempt to cast type ggi to type coupled#0 Foam::error::printStack(Foam:stream&) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam:stream& Foam::operator<<>(Foam:stream&, Foam::errorManip<foam::error>) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so"
#3 void Foam::pointPatchInterpolation::interpolate<double> (Foam::GeometricField<double,> const&, Foam::GeometricField<double,>&, bool) const in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfiniteVolume.so"
#4 Foam::tmp<foam::geometricfield<double,> > Foam::volPointInterpolation::interpolate<double>(F oam::GeometricField<double,> const&) const addr2line failed
#5 void Foam::vtkPV3Foam::convertVolFields<double>(Foam::f vMesh const&, Foam::volPointInterpolation const&, Foam::PtrList<foam::primitivepatchinterpolation<fo am::primitivepatch<foam::face, > > const&, Foam::Vector<double> > > > const&, Foam::IOobjectList const&, vtkDataArraySelection*, vtkMultiBlockDataSet*) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libvtkPV3Foam.so"
#6 Foam::vtkPV3Foam::updateVolFields(vtkMultiBlockDat aSet*) addr2line failed
#7 Foam::vtkPV3Foam::Update(vtkMultiBlockDataSet*) addr2line failed
#8 vtkPV3FoamReader::RequestData(vtkInformation*, vtkInformationVector**, vtkInformationVector*) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libPV3FoamReader_SM.so"
#9 vtkMultiBlockDataSetAlgorithm::ProcessRequest(vtkI nformation*, vtkInformationVector**, vtkInformationVector*) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkFiltering .so.pv3.3"
#10 vtkExecutive::CallAlgorithm(vtkInformation*, int, vtkInformationVector**, vtkInformationVector*) addr2line failed
#11 vtkDemandDrivenPipeline::ExecuteData(vtkInformatio n*, vtkInformationVector**, vtkInformationVector*) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkFiltering .so.pv3.3"
#12 vtkCompositeDataPipeline::ExecuteData(vtkInformati on*, vtkInformationVector**, vtkInformationVector*) addr2line failed
#13 vtkDemandDrivenPipeline::ProcessRequest(vtkInforma tion*, vtkInformationVector**, vtkInformationVector*) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkFiltering .so.pv3.3"
#14 vtkStreamingDemandDrivenPipeline::ProcessRequest(v tkInformation*, vtkInformationVector**, vtkInformationVector*) addr2line failed
#15 vtkCompositeDataPipeline::ProcessRequest(vtkInform ation*, vtkInformationVector**, vtkInformationVector*) addr2line failed
#16 vtkDemandDrivenPipeline::UpdateData(int) addr2line failed
#17 vtkStreamingDemandDrivenPipeline::Update(int) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkFiltering .so.pv3.3"
#18 vtkExecutive::Update() in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkFiltering .so.pv3.3"
#19 vtkDemandDrivenPipeline::Update() addr2line failed
#20 vtkStreamingDemandDrivenPipeline::Update() in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkFiltering .so.pv3.3"
#21 vtkAlgorithm::Update() in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkFiltering .so.pv3.3"
#22 vtkAlgorithmCommand(vtkClientServerInterpreter*, vtkObjectBase*, char const*, vtkClientServerStream const&, vtkClientServerStream&) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkFiltering CS.so"
#23 vtkMultiBlockDataSetAlgorithmCommand(vtkClientServ erInterpreter*, vtkObjectBase*, char const*, vtkClientServerStream const&, vtkClientServerStream&) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkFiltering CS.so"
#24 vtkPV3FoamReaderCommand(vtkClientServerInterpreter *, vtkObjectBase*, char const*, vtkClientServerStream const&, vtkClientServerStream&) in "/opt/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libPV3FoamReader_SM.so"
#25 vtkClientServerInterpreter::ProcessCommandInvoke(v tkClientServerStream const&, int) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkClientSer ver.so"
#26 vtkClientServerInterpreter::ProcessOneMessage(vtkC lientServerStream const&, int) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkClientSer ver.so"
#27 vtkClientServerInterpreter::ProcessStream(vtkClien tServerStream const&) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkClientSer ver.so"
#28 vtkSelfConnection::ProcessStreamLocally(vtkClientS erverStream&) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerC ommon.so"
#29 vtkSelfConnection::SendStreamToClient(vtkClientSer verStream&) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerC ommon.so"
#30 vtkProcessModuleConnection::SendStream(unsigned int, vtkClientServerStream&) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerC ommon.so"
#31 vtkProcessModuleConnectionManager::SendStream(int, unsigned int, vtkClientServerStream&, int) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerC ommon.so"
#32 vtkProcessModule::SendStream(int, unsigned int, vtkClientServerStream&, int) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerC ommon.so"
#33 vtkSMOutputPort::UpdatePipeline(double) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerM anager.so"
#34 vtkSMSourceProxy::UpdatePipeline(double) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerM anager.so"
#35 pqOutputPort::getDataInformation(bool) const in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqCore.so"
#36 pqDisplayPolicy::getPreferredViewType(pqOutputPort *, bool) const in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqCore.so"
#37 pqDisplayPolicy::getPreferredView(pqOutputPort*, pqView*) const in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqCore.so"
#38 pqDisplayPolicy::createPreferredRepresentation(pqO utputPort*, pqView*, bool) const in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqCore.so"
#39 pqPendingDisplayManager::createPendingDisplays(pqV iew*) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqCore.so"
#40 pqMainWindowCore::createPendingDisplays() in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqComponents .so"
#41 pqMainWindowCore::qt_metacall(QMetaObject::Call, int, void**) at moc_pqMainWindowCore.cxx:0
#42 QMetaObject::activate(QObject*, int, int, void**) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtCore.so.4"
#43 QMetaObject::activate(QObject*, QMetaObject const*, int, void**) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtCore.so.4"
#44 pqObjectInspectorWidget::accepted() in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqComponents .so"
#45 pqObjectInspectorWidget::accept() in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqComponents .so"
#46 pqObjectInspectorWidget::qt_metacall(QMetaObject:: Call, int, void**) at moc_pqObjectInspectorWidget.cxx:0
#47 QMetaObject::activate(QObject*, int, int, void**) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtCore.so.4"
#48 QMetaObject::activate(QObject*, QMetaObject const*, int, int, void**) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtCore.so.4"
#49 QAbstractButton::clicked(bool) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#50 ?? in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#51 ?? in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#52 QAbstractButton::mouseReleaseEvent(QMouseEvent*) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#53 QWidget::event(QEvent*) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#54 QAbstractButton::event(QEvent*) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#55 QPushButton::event(QEvent*) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#56 QApplicationPrivate::notify_helper(QObject*, QEvent*) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#57 QApplication::notify(QObject*, QEvent*) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#58 QCoreApplication::notifyInternal(QObject*, QEvent*) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtCore.so.4"
#59 QCoreApplication::sendSpontaneousEvent(QObject*, QEvent*) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#60 ?? in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#61 QApplication::x11ProcessEvent(_XEvent*) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#62 ?? in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtGui.so.4"
#63 QEventLoop::processEvents(QFlags<qeventloop::proce sseventsflag>) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtCore.so.4"
#64 QEventLoop::exec(QFlags<qeventloop::processeventsf lag>) in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtCore.so.4"
#65 QCoreApplication::exec() in "/opt/OpenFOAM/ThirdParty/Qt-4.3.5/lib/libQtCore.so.4"
#66 pqProcessModuleGUIHelper::RunGUIStart(int, char**, int, int) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqCore.so"
#67 vtkProcessModule::StartClient(int, char**) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerC ommon.so"
#68 vtkProcessModule::Start(int, char**) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerC ommon.so"
#69 vtkProcessModuleGUIHelper::Run(vtkPVOptions*) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libvtkPVServerC ommon.so"
#70 pqMain::Run(QApplication&, pqProcessModuleGUIHelper*) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/libpqCore.so"
#71 main in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/paraview"
#72 __libc_start_main in "/lib/libc.so.6"
#73 vtkObject::RegisterInternal(vtkObjectBase*, int) in "/opt/OpenFOAM/ThirdParty/ParaView3.3-cvs/platforms/linuxGcc/bin/paraview"


From function refCast<to>(From&)
in file /opt/OpenFOAM/OpenFOAM-1.5/src/OpenFOAM/lnInclude/typeInfo.H at line 106.

FOAM aborting

/opt/OpenFOAM/OpenFOAM-1.5/bin/paraFoam: line 81: 3684 Abgebrochen paraview --data=$caseFile
[david@localhost mixerGgi]$

************************************************** ******

Does anybody have an idea how this could be fixed or what I did wrong? It would be very nice if I could postprocess the cases directly with paraFoam3.

Thanks,
David
david is offline   Reply With Quote

Old   September 20, 2008, 13:08
Default Sorry, wrong tab & wrong threa
  #20
Member
 
David Hora
Join Date: Mar 2009
Location: Zürich, Switzerland
Posts: 63
Rep Power: 7
david is on a distinguished road
Sorry, wrong tab & wrong thread!!
david 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 Processing pipe FLUENT 0 December 22, 2008 10:34
FSI and parallel processing Jorn CFX 5 June 8, 2007 15:53
Parallel processing and FSI guus_kupers OpenFOAM Running, Solving & CFD 0 March 20, 2007 10:40
Parallel Processing Drew Abbott FLUENT 2 August 29, 2006 12:35
Parallel processing Phil FLUENT 1 May 27, 2004 07:18


All times are GMT -4. The time now is 18:07.