ParaView patch visualisation error in Development version
 

Hello there,
I have been using the development version of OpenFOAM 1.3 (11.09.2006 - Hrv from Frank Bos' site) for some time now.

Today for the first time, I tried viewing only the patches for a mesh by switching off the "internal mesh" in Paraview.... I wanted to check if the patches I had selected were right or not.

Unfortunately, when I switch off the Internal mesh, I get nothing on the display... the patches are not displayed, though paraview indicates that they are on.

Thinking it was a flaw in Paraview 2.4.4 (which I downloaded from Hrv's site some time back), I reverted back to Paraview 2.4.2 which comes with the original OpenFOAM 1.3 package.

This did not solve the problem. I suspect there might be a problem with the OpenFOAM part of the paraview conversion in the development version... maybe one of the libraries, or the code which does the preprocessing before starting paraview.

Has anyone else noticed this problem? It used to work without any problems with the original OpenFOAM 1.3 and paraview 2.4.2

Have a nice day!

Philippose

I've got the same problem usin
 

I've got the same problem using (all) versions of paraview in combination with the development version. A time ago I tried to recompile paraview and the openfoam libraries corresponding to it. I think that the recompilation went wrong somewhere.
When I want to visualize the patches I use the standard openfoam + paraview installation which I have still installed as a different user. Otherwise I use Tecplot 360 (but that's not free :-()

Cheers, Frank

Yes, that would be me. The bi
 

Yes, that would be me. The binary build was badly broken in quite a few places, including mesh motion and complete topological changes. After I have fixed the topo change module I've found out that when the topology change occurs, paraFoam fails with out-of-bounds array memory access. This is because in topo changes the size of patches changes all the time, which is not taken into account in the paraview reader.

This needed to be fixed and I have changed the reader to account for topo changes in the boundary. You can reproduce the error using -DFULL_DEBUG on any case where the number of faces works fine.

Unfortunately, this is one of those pieces of OpenFOAM that I didn't write personally and there are errors in what I have done. I'm not sure if paraview proxies bits of OpenFOAM mesh or it does not allow re-sizing, but ever since the display of boundary faces was broken. Incidentally, dxFoam works just fine + it does a much better job displaying polyhedral cells.

I don't know how to fix this properly - if someone has got ideas or a bug fix, it will come in immediately (+ a "thank you beer" in Zagreb).

Hrv

Hi Frank, Thanks for corrobor
 

Hi Frank,
Thanks for corroborating the phenomenon I am having with the development version.

Yesterday I compiled the CVS version of Paraview 2.6, but though it can read foam files natively, I found that the openFOAM libraries are much faster...and moreover, the CVS version handles only the internal field and doesnt extract patches yet.

I tried to recompile the paraview reader related libraries in openFOAM, but that didnt work because it looks for some include files from the Paraview 2.4.4 source code, and I guess some configuration files need to be modified since there are lot of absolute paths which existed on the original computer on which it was compiled (Prof Jasak's :-)).

Have a nice Sunday!

Philippose

If you look inot the developme
 

If you look inot the development version, there's a file called buildInstructions.txt. It shows you that you have to build paraview yourself, copy some files etc. in order to natively build paraFoam.

Here's the relevant section:

4.5 paraview
cd ~/OpenFOAM/linuxSrc
tar xvzf paraview-2.4.4.tgz
mkdir paraview-2.4.4-obj
cmake -i ../paraview-2.4.4

Change options:

enable shared library: YES
prefix: ~/OpenFOAM/linux/paraview-2.4.4

gmake
gmake install


cd ~/OpenFOAM/linuxSrc

mkdir ~/OpenFOAM/linux/paraview-2.4.4/include
cp ./paraview-2.4.4/VTK/Common/vtk* ~/OpenFOAM/linux/paraview-2.4.4/include/
cp ./paraview-2.4.4/VTK/Filtering/vtk* ~/OpenFOAM/linux/paraview-2.4.4/include/
cp ./paraview-2.4.4-obj/VTK/vtk* ~/OpenFOAM/linux/paraview-2.4.4/include/
cp ./paraview-2.4.4-obj/ParaViewConfig.cmake ~/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/


Enjoy,

Hrv

Hello again Hrv, I am just
 

Hello again Hrv,
I am just shooting in the dark here... could the error in paraview due to changing patch sizes be something to do with the "cache mesh" option in paraview?

I am assuming that when the mesh is cached internally by paraview (which is the default option when you start paraview), any changes in patch size would cause out-of-bounds errors.

And... wouldnt Terry Jordan be able to help out in this situation because he seems to be involved with paraview development?

Philippose

Hello Hrv, This is with reg
 

Hello Hrv,
This is with regard to the bug in the vtkFoam library module in the development version (Downloaded from Frank Bos' site), due to which one cannot visualise individual patches in ParaView...

I spent the day looking through the vtkFoam directory, and finally found that the error came from the function "convertMesh()" in the file vtkFoam.C

In the file "vtkFoam.C", line numbers 223 to 260, the entire patch data is reread from the boundary file in the case. Here, the error comes from line numbers 253 to 256.

In this region, redefinition of the grid in the "setNthOutput" on an already existent region ID seems the be the problem.

I commented out lines 248 to 255, leaving behind the line "reader_->GetOutput(regioni)->Initialize()" intact, since this line resets the grid to an empty state and frees the used memory (which would be needed if the patch sizes change).... after rebuilding the library, ParaView worked fine (i.e., I can visualise each individual patch, and not just the internal mesh).

Now I have modified the code so that the "AddArray" function and the "setNthOutput" is called only when a patch which does not already exist in the vtk data set is found.

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif vtkFoam_dev_Release_bugfix.tar.gz

Could you try the modified vtkFoam library, to see if it works with cases where there are topological changes to the mesh?

Is it normal for patches to be added or removed from an OpenFOAM case? I understand that patch sizes can change, but are there situations where new patches can be formed during simulation... or patches deleted during simulation ?

Have a nice day!

Philippose

Hello again, I just tested
 

Hello again,
I just tested the modified ParaView vtkFoam library with the icoDyMFoam tutorial case "movingCone", and it is workiing fine... I am able to visualise each patch, and there are no errors.

Moving cone uses topological changes right? And not just mesh motion?

Enjoy!

Philippose

Heya, Well, you did it: it
 

Heya,

Well, you did it: it works fine, with no errors and no access problems. However, I get some really weird visualisation, with the "non-existent patch" carrying no data. Try the mixer2D tutorial and you will see for yourself.

I have prepared a moving cone tutorial with topological changes a while ago - if you want to try it out, just run attached.

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif movingConeTopo.tgz

Please let me know if you see a problem with the visualisation - maybe it's the empty patches...

Hrv

Woops! Segmentation fault:
 

Woops! Segmentation fault:

Shall I pass you the case or you is it too complex for serious digging?

Hrv


Program received signal SIGSEGV, Segmentation fault.
[Switching to Thread 1145648320 (LWP 1356)]
0x42ec8d23 in vtkDataObject::NewInstance () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkGraphics.so.pv 2.4
(gdb) where
#0 0x42ec8d23 in vtkDataObject::NewInstance () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkGraphics.so.pv 2.4
#1 0x574c4d29 in vtkFoamReader::Execute () from /home/hjasak/OpenFOAM/OpenFOAM-1.3/lib/linuxGcc4DPDebug/libPVFoamReader.so
#2 0x43e985fe in vtkSource::ExecuteData () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#3 0x43e98005 in vtkSource::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#4 0x43d8beba in vtkExecutive::CallAlgorithm () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#5 0x43d86d2e in vtkDemandDrivenPipeline::ExecuteData () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#6 0x43d68631 in vtkCompositeDataPipeline::ExecuteData () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#7 0x43d8a24d in vtkDemandDrivenPipeline::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#8 0x43e9f9a2 in vtkStreamingDemandDrivenPipeline::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#9 0x43d69a21 in vtkCompositeDataPipeline::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#10 0x43d8e1d9 in vtkExecutive::ForwardUpstream () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#11 0x43d65f58 in vtkCompositeDataPipeline::ForwardUpstream () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#12 0x43d8a1a2 in vtkDemandDrivenPipeline::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#13 0x43e9f9a2 in vtkStreamingDemandDrivenPipeline::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#14 0x43d69a21 in vtkCompositeDataPipeline::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#15 0x43d8e1d9 in vtkExecutive::ForwardUpstream () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#16 0x43d65f58 in vtkCompositeDataPipeline::ForwardUpstream () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#17 0x43d8a1a2 in vtkDemandDrivenPipeline::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#18 0x43e9f9a2 in vtkStreamingDemandDrivenPipeline::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#19 0x43d69a21 in vtkCompositeDataPipeline::ProcessRequest () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#20 0x43d89a8c in vtkDemandDrivenPipeline::UpdateData () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#21 0x43e9e9e9 in vtkStreamingDemandDrivenPipeline::Update () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#22 0x43d74a14 in vtkDataObject::Update () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkFiltering.so.p v2.4
#23 0x41258873 in vtkPVUpdateSuppressor::ForceUpdate () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVFilters.so
#24 0x41258be5 in vtkPVUpdateSuppressor::CacheUpdate () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVFilters.so
#25 0x41111308 in vtkPVUpdateSuppressorCommand () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVFiltersCS.so
---Type <return> to continue, or q <return> to quit---
#26 0x40054bbc in vtkClientServerInterpreter::ProcessCommandInvoke () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkClientServer.s o
#27 0x40054eb0 in vtkClientServerInterpreter::ProcessOneMessage () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkClientServer.s o
#28 0x40055114 in vtkClientServerInterpreter::ProcessStream () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkClientServer.s o
#29 0x41b23e93 in vtkProcessModule::SendStreamToClient () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerCommon .so
#30 0x41b24bf7 in vtkProcessModule::SendStream () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerCommon .so
#31 0x40d9c0b9 in vtkSMProxy::UpdateVTKObjects () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerManage r.so
#32 0x40d9c114 in vtkSMProxy::UpdateVTKObjects () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerManage r.so
#33 0x40db91a8 in vtkSMRenderModuleProxy::CacheUpdate () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerManage r.so
#34 0x40d0a36a in vtkSMAnimationSceneProxy::CacheUpdate () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerManage r.so
#35 0x40d0c18c in vtkSMAnimationSceneProxy::TickInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerManage r.so
#36 0x40d060ce in vtkSMAnimationCueProxy::ExecuteEvent () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerManage r.so
#37 0x40d08629 in vtkSMAnimationCueProxyObserver::Execute () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerManage r.so
#38 0x4415cda5 in vtkSubjectHelper::InvokeEvent () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommon.so.pv2. 4
#39 0x4415ce55 in vtkObject::InvokeEvent () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommon.so.pv2. 4
#40 0x440c29c6 in vtkAnimationCue::TickInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommon.so.pv2. 4
#41 0x440c3ed4 in vtkAnimationScene::TickInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommon.so.pv2. 4
#42 0x440c26ed in vtkAnimationCue::Tick () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommon.so.pv2. 4
#43 0x440c448e in vtkAnimationScene::Play () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommon.so.pv2. 4
#44 0x40d0aad6 in vtkSMAnimationSceneProxy::Play () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerManage r.so
#45 0x402d53b1 in vtkPVAnimationScene::Play () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#46 0x401c7d28 in vtkPVAnimationSceneCppCommand () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#47 0x401ca788 in vtkPVAnimationSceneCommand () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#48 0x40f7f6af in TclInvokeStringCommand () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#49 0x40f80e1f in TclEvalObjvInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#50 0x40f81146 in Tcl_EvalEx () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#51 0x40f81d5f in Tcl_EvalObjEx () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
---Type <return> to continue, or q <return> to quit---
#52 0x40f885c9 in Tcl_EvalObjCmd () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#53 0x40f80e1f in TclEvalObjvInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#54 0x40f81146 in Tcl_EvalEx () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#55 0x40f81608 in Tcl_Eval () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#56 0x40f8168e in Tcl_GlobalEval () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#57 0x40a0145d in vtkKWTkUtilities::EvaluateSimpleStringInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libKWWidgets.so
#58 0x40a017be in vtkKWTkUtilities::EvaluateStringFromArgsInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libKWWidgets.so
#59 0x40a0187d in vtkKWTkUtilities::EvaluateStringFromArgs () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libKWWidgets.so
#60 0x4095ef66 in vtkKWObject::Script () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libKWWidgets.so
#61 0x40496c25 in vtkPVVCRControl::InvokeCommand () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#62 0x40496e06 in vtkPVVCRControl::PlayCallback () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#63 0x4027671b in vtkPVVCRControlCppCommand () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#64 0x402775ec in vtkPVVCRControlCommand () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#65 0x40f7f6af in TclInvokeStringCommand () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#66 0x40f80e1f in TclEvalObjvInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#67 0x40fa62a8 in TclExecuteByteCode () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#68 0x40fa548c in TclCompEvalObj () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#69 0x40f81d8d in Tcl_EvalObjEx () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#70 0x41011bd7 in TkInvokeButton () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#71 0x41013165 in ButtonWidgetObjCmd () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#72 0x40f80e1f in TclEvalObjvInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#73 0x40f81bd4 in Tcl_EvalObjv () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#74 0x40f81d2c in Tcl_EvalObjEx () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#75 0x40fd6b8c in Tcl_UplevelObjCmd () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#76 0x40f80e1f in TclEvalObjvInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#77 0x40fa62a8 in TclExecuteByteCode () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
---Type <return> to continue, or q <return> to quit---
#78 0x40fa548c in TclCompEvalObj () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#79 0x40fd65cd in TclObjInterpProc () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#80 0x40f80e1f in TclEvalObjvInternal () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#81 0x40f81146 in Tcl_EvalEx () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#82 0x40f81608 in Tcl_Eval () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#83 0x40f8168e in Tcl_GlobalEval () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#84 0x4106f960 in Tk_BindEvent () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#85 0x4107441b in TkBindEventProc () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#86 0x40ffd0e9 in Tk_HandleEvent () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#87 0x40ffd185 in WindowEventProc () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#88 0x40fccb91 in Tcl_ServiceEvent () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#89 0x40fccdfa in Tcl_DoOneEvent () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkCommonTCL.so
#90 0x408c3012 in vtkKWApplication::DoOneTclEvent () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libKWWidgets.so
#91 0x408bf2c1 in vtkKWApplication::Start () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libKWWidgets.so
#92 0x40292c89 in vtkPVApplication::Start () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#93 0x4050578b in vtkPVProcessModuleGUIHelper::ActualRun () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#94 0x40506365 in vtkPVProcessModuleGUIHelper::RunGUIStart () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkKWParaView.so
#95 0x41b1190d in vtkPVProcessModule::Start () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerCommon .so
#96 0x41b274a9 in vtkProcessModuleGUIHelper::Run () from /home/hjasak/OpenFOAM/linux/paraview-2.4.4/lib/paraview-2.4/libvtkPVServerCommon .so
#97 0x0804a027 in MyMain ()
#98 0x0804a08c in main ()

Hello and a Good Morning :-)!
 

Hello and a Good Morning :-)!

I have always had the feeling that nothing comes easy :-)! So here is more proof!

Did you get the segementation fault when running the case you have provided in the previous post? And could you also tell me what you did to produce the error?

I shall look deeper into this... this is why I wanted you to check it out, because I am not so conversant with moving meshes including topological changes :-)! It worked fine for my comparatively plain vanilla cases :-)!

I really didnt expect it to work flawlessly yet :-)! I guess I need to start looking into how VTK works.... but I am more or less sure the error is at that point in the code.

Do I have a time frame for this? Do you want to put it into the next release? In which case, what kind of time window do I have? Sometimes its nice to work with a time challenge :-)!

Have a nice day, and thanks for checking it out!

Philippose

Heya, The error happens on
 

Heya,

The error happens on another case, I've uploaded it here if you want to have a play. The error is somewhere in vtkFoam.C - when I reverted to the previous version, it worked fine. The case is quite complex with lots of topo changes so it will actually be a good test.

There's no time pressure on my part - either you do it or I have to :-)

Thanks again + keep in touch,

Hrv

Hi Hrv, Thanks a lot for th
 

Hi Hrv,
Thanks a lot for the case.... for me its like two birds with one stone.... I get to see a real working case containing topological changes other than the ones in the tutorial, and... as a by-product... I can test the paraview visualisation ;-)!!

Shall look into the bug.... and hope to solve it soon :-)!

Enjoy!

Philippose

Hello once again :-)! So...
 

Hello once again :-)!

So...here we go again... the case you gave me really helped see the actual requirements of the vtkFoam library... :-)!

I have made quite a bit of modification to the vtkFoam library now... specifically, the "convertMesh()" function, and I am happy to report, that your case seems to be working fine now... except for one small caveat... which I am yet to solve... :-) (Its late, and I need to go to work early morning !!)

When the "cache mesh" is enabled, and then if the "constant" time set is selected, the system quits with a segment fault. If "cache mesh" is turned off, this part works fine.

In all other situations (within my limited experience of ParaView), everything seems to work fine... and I even added a function to pad the name of the patch, because one cannot ensure that all patches have the same length in a scenario where patch names are removed and added from the list dynamically.

The only annoyance, which as far as I can understand is a general problem with ParaView, is the lack of automatic scaling of the colours used to display the data set during an animation.....

As for the error with the "cache mesh" and "constant" time, I will be looking into it in the next few days.....

Here is the latest version... it would be great if we can stress test the code to see in what other scenarios it fails :-)!

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif vtkFoam_bugfix2.tar.gz

Have a nice day!

Philippose

Once more before hitting the s
 

Once more before hitting the sack... :-)!

I just tested out the "movingConeTopo" case which you had uploaded earlier today.... thats working flawlessly :-)!! Including the "constant" time, with "cache mesh" on...

I think its something to do with the result of the "meshPtr->readUpdate()" part of the code which is tripping up in the case of the "simpleEngine" case...

Any ideas?

Philippose

Hello and a good day! Here
 

Hello and a good day!

Here it is... the final bugfix for the vtkFoam Library. Everything seems to be working now... My test cases have always been the "simpleEngine" case from Hrvoje and the cases I use for my work (which dont use topological changes but only moving meshes).

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif vtkFoam_bugfix_final.tar.gz

As of now, I havent seen any segmentation faults, or error / warning messages in the console, and visualisation of individual patches are working fine... even in cases where multiple patches disappear, appear or re-appear during an animation.

As usual, it would be great if people could stress test the new version, to see if something crops up in some special situation or scenario.

Though vtkFoam works fine now, there are some issues regarding the Paraview / VTK interface that came to light during my study of the code....

1. Display of the time and region selection lists in Paraview are allowed to grow, but later if the list size becomes smaller, the rest of the lines in the display remain and are not erased.

2. Changes to the regions list are only updated if one can trigger a situation where the "Accept" button needs to be pressed... In this particular case, if patches are added or removed, the changes can only be seen if you create a situation in which you need to press the "Accept" button... such as disabling and enabling an existent patch or something similar.

If these two small Paraview irritations can be solved, it would be great :-)!

Awaiting feedback!

Have a nice day!

Philippose

Works beautifully - great job!
 

Works beautifully - great job!

Hrv

Hi Hrv, Thanks a lot for chec
 

Hi Hrv,
Thanks a lot for checking out the library, and I am happy it is working fine :-)!

I have commented the code, and as far as I know, have also stuck to the coding conventions (naming, and indentation, etc..) used by OpenFoam. In case there is something amiss on this front too, please do not hesitate to let me know.

Enjoy!

Philippose