CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Parallel processing (http://www.cfd-online.com/Forums/openfoam-solving/58530-parallel-processing.html)

ghanshyam September 2, 2005 00:32

While decomposing the grid in
 
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

boschert September 2, 2005 03:14

Hello, The answer to your fir
 
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

henry September 2, 2005 03:37

I take it your case was saved
 
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.

ghanshyam September 2, 2005 04:04

Thanks Stefan, now I can decom
 
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

henry September 2, 2005 04:07

As I say try adding the value
 
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.

ghanshyam September 2, 2005 04:34

This is how my pressure 'p' fi
 
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

henry September 2, 2005 04:37

Please please please add the v
 
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.

ghanshyam September 2, 2005 05:07

I am really sorry for botherin
 
I am really sorry for bothering you so much. Now it works.

Thanks and regards

GS

ghanshyam September 5, 2005 05:42

How inter processor data commu
 
How inter processor data communication is done? It it done using blocking MPI calls?

Regards
GS

henry September 5, 2005 05:48

It depends on the choice of sc
 
It depends on the choice of scheduling, without we use MPI_Bsend and with we use MPI_Send.

ghanshyam September 5, 2005 06:11

So data coherency is ensured?
 
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

henry September 5, 2005 06:17

It is a non-overlap (no halo-c
 
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.

ghanshyam September 5, 2005 06:23

Thanks Henry for the clarefica
 
Thanks Henry for the clarefication.

Regards
GS

ghanshyam September 5, 2005 06:41

Sorry for the typo in the prev
 
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

henry September 5, 2005 06:48

The pressure equation is ellip
 
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.

boschert September 8, 2005 08:40

To fix the problem with the to
 
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

henry September 8, 2005 09:03

The value field is only used b
 
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.

jballen April 20, 2006 14:34

Hi, In serial one can loop
 
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

david September 20, 2008 13:06

Hi all I tried to implement
 
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:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) 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:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream& Foam::operator<<>(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&, 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 September 20, 2008 13:08

Sorry, wrong tab & wrong threa
 
Sorry, wrong tab & wrong thread!!


All times are GMT -4. The time now is 03:59.