Native ParaView Reader Bugs
 

I just wanted to created a post where we could keep a buglist/request for functionality list for the native openfoam reader in ParaView.

I have been away from developing the reader for sometime and would like to get it upto date.

Thanks,
Terry

Hi Terry! Thanks for your w
 

Hi Terry!

Thanks for your work.

I'm currently trying it (64Bit Linux Machine, Paraview 3, compiled from the CVS). OpenFOAM-functionality is enabled via a Client-Plugin (right now the OpenFile-Dialog doesn't know OF-files).

It works fine for some cases. The problems I can put my finger on so far are:

- it is not very tolerant about the files in the time-direcotries (it allocates memory if there are any gzipped-files until the machine is completely filled). Same thing happens if there are any backup-files from the texteditor (ending with a ~)
- For some geometries I only can see the grid but can not color it with data (although the data gets recognized) I'll try to find a minimal case where that happens.

If you got a new version of vtkOpenFOAMReader that you want to have tested, I'd be more than happy to do so.

Bernhard

*Gzipped data is not supported
 

*Gzipped data is not supported.

*You need to create a copy of the controlDict file named "controlDict.foam" -> Paraview doesnt support opening files without extensions.

*The newest version of the reader would be in the latest release of Paraview. I would however suggest using the Paraview 2.6.2 (which also has the newest reader) not the 3 branch. I havent tested it much on 3 and there were major changes to Paraview made between those two releases.

Thanks.

@Gzipped data: Any plans to su
 

@Gzipped data: Any plans to support that? Because having only non-zipped-data limits the usefullness for any real-life data (at least a more robust result than crashing would be cool)

Cool features (if you have too much time on your hands) would be:
- Support for Multi-region cases
- Lagrange particles

I don't have much time to inve
 

I don't have much time to invest in the reader currently. Hopefully in the future I will have sometime to add some functionality. For the time being I am looking for any bugs in the current functionality.

Hi, I'm now trying rather tho
 

Hi,
I'm now trying rather thorough bug hunting of the paraview native reader since I wrote paraFoam for Cygwin to use the native reader (afaik this is the only feasible way to realize paraFoam on Windows). Maybe I'll be posting a patch around early next week.

Although I well understand, and also would like what Bernhard suggests, the patch will exactly be focused on bugfix (most notably reported at this thread) and will include no feature enhancements, meant to serve as a basis for enhancements.

Takuya

Hi, Here's the patch for the
 

Hi,
Here's the patch for the reader included in the ParaView-2.6.2 distribution. To apply cd to ParaView-2.6.2/VTK/IO and run

patch < vtkOpenFOAMReader-20070813.diff.

If your mesh has any zones defined, extract group 0 (choose Filter->Extract Group and select group 0) to work on the dataset. Otherwise you'll see geometry but cannot colorize it (just as Bernhard pointed out above). Group 1 and above contain zone geometries.

Problems fixed:
* the reader should now work better and stably at least for most of the tutorial cases except for gzipped ones, and for other cases with relatively complex meshes/overall setups (especially ones with polyhedra/tetrahedra).

Problems not fixed:
* proper comment handling
* handling of tiny mesh/internalField/boundaryField datasets (< 10 elements), e. g. the solidEquilibriumDisplacementFoam/beamEndLoad case where some patches have only 6 faces

I figured that these remaining problems would be better fixed by rewriting the current line-based parser of the reader to token-based one that better emulates the one in libOpenFOAM, with gzipped stream support, as a longer-term work.

Hopefully Terry will be able to concentrate on new features,
Takuya
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif vtkOpenFOAMReader-20070813.diff

It may be quite a while before
 

It may be quite a while before I have time to add new features. I will try to get these changes in soon. If anyone wants to add new features feel free. You will have to commit the code through me.

Takuya, if I use your patch I will credit you in the source.

Thanks.

Thanks Terry, personally I thi
 

Thanks Terry, personally I think it's well worth investing some collaborative developments to improve the native reader since all VTK-based applications under all the supported platforms, not only paraview on Linux, could benefit from it, but I neither have enough time... I will post a patch again if I ever could implement those listed in my post above.

Takuya

Hi Terry and all, After a clo
 

Hi Terry and all,
After a close and intensive collaboration, Philippose Rajan and I are happy to announce the availability of OpenFOAM native reader for ParaView3-CVS.

New features are:

• Supports the ParaView 3.3 CVS development version (as of Oct. 22, 2007).
• The reader supports volScalarField, volVectorField, lagrangian (of class Cloud) scalarField, lagrangian vectorField. Currently no support for point/surface nor symmTensor/tensor fields (see Notes to use the lagrangian feature).
• The reader supports compressed(gzipped)/uncompressed-ascii/double precision binary data formats. Single precision binary format is not supported.
• Improved performance. You should find the reader a lot faster than the previous versions.
• Neat user interface. Patch and array selection lists are now offered.

Roles are:

• Philippose Rajan: user interface, extensive testing, many suggestions http://www.cfd-online.com/OpenFOAM_D...part/happy.gif.
• Takuya Oshima: implementation of token-based FoamFile parser, performance enhancements, gzipped file support, lagrangian field support.

Before using the reader, you might want to have a look at ReleaseNotes for installation procedure and notes (the same file is also included in the package):
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif ReleaseNotes

After reading ReleaseNotes if you think it's worth trying, here's the package:
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif vtkOpenFOAMReader-20071023.tar.bz2

To Terry:
We would like to make the reader code go into the source tree of ParaView3. Would it be possible?

Regards,
Takuya

Takuya, I have sent the reade
 

Takuya,
I have sent the reader updates to my contact at ParaView. I will let you know when the changes are available in the CVS.

Thanks Terry, thanks indeed!
 

Thanks Terry, thanks indeed!

Takuya

Hi Takuya, I'm currently us
 

Hi Takuya,

I'm currently using the OpenFOAM native reader together with the precompiled ParaView 3.3.0 you offered to download from your homepage (Thanks for that!). It runs fine, but I still have two small questions which may fit into this thread:

1.) I tried to use the ParaView filter "Surface Flow" but although I extracted the correct boundary surface the filter was not avaiable (stayed grey).
I doubt it's a bug, so maybe you can tell me whether it's simply not supported in the current version or a different procedure has to be used to make the filter available.

2.) It's an understanding question: When you refer to the performance of the reader, do you mean e. g. the playback speed of a timestep animation in ParaView? I noticed that the animation of the same case runs a bit faster and smoother when vtk-Files are used, do you know why?

Many thanks in advance.

Best regards,
Johannes

Hi Johannes, 1.) It looks l
 

Hi Johannes,

1.) It looks like it's because of an incompatibility between what the reader offers as output dataset and what the filter requires as input, i.e. the Surface Flow filter doesn't seem to support composite dataset types, one of which is the type of dataset reader outputs. Other possibly incompatible filters with the same reason are Append Attributes and Append Datasets (I still haven't confirmed though). Unfortunately no quick workaround come to me.

2.) Roughly yes, I mean performance by mainly the initial loading time of a case and the playback speed of an animation. However note that
a.) I meant "better performance" by comparison to the previous versions of the reader and by no means comparison to the VTK reader.
b.) even if we make some comparisons with the VTK reader, nothing can't be said for sure without the details of the comparison, i.e. what formats (single/double-precision, text/binary formats) are used, whether patch data are also read or not, what differences are observed etc. For example if you compared the OpenFOAM reader with an ascii format case reading all internal mesh/patches and the VTK reader with single-precision binary format reading only internal mesh, and observed "only" a bit faster result with the VTK reader (which is quite a likely situation), in my view the OpenFOAM reader is doing surprisingly and unexpectedly well.

Since

Takuya

Sorry I mistakenly pressed the
 

Sorry I mistakenly pressed the post button.

Since the OpenFOAM reader only supports double precision and foamToVTK only supports single precision as binary formats, a fair comparison will be in ascii formats (foamToVTK -ascii -noPointValues for VTK format).

Takuya

Hi Takuya, that's exactly w
 

Hi Takuya,

that's exactly what I wanted to know, thanks.

Regarding 1.): I can live with that; for cases where I need this filter I'll use VTK files.

Regarding 2.): I think the performance of the OpenFOAM reader is absolutely ok for watching the results. And for the rare times I record an animation via screen capturing I may use foamToVTK as well.

Best regards,
Johannes

Hi Takuya First thank you f
 

Hi Takuya

First thank you for your contribution this is good stuff and I really like the new Paraview3

I downloaded the paraview-3.3.0 svn-version by end November last year. Patched up and compiled this version all the way it was described by your beautiful Release Notes. Until now everything works marvelous!

Unfortunately this version has a feature (setting the resolution, when saving pictures "Save ScreenShot"), which is added in the most reason svn version (16.01.08). Now again I patched and compiled everything without any errors, but as soon as I try to read a controlDict.foam (OFcase) I get a crash with the following error:


./bin/paraview
ERROR: In /home/klosterm/OpenFOAM/linux64/ParaView3/Servers/Common/vtkProcessModule.cxx, line 1008
vtkProcessModule (0x6ff960): Object type: vtkOpenFOAMReader, could not find requested method: "SetKeepPatches"
or the method was called with incorrect arguments.

while processing
Message 0 = Invoke
Argument 0 = id_value {94
Argument 1 = string_value {SetKeepPatches}
Argument 2 = int32_value {1}



ERROR: In /home/klosterm/OpenFOAM/linux64/ParaView3/Servers/Common/vtkProcessModule.cxx, line 1009
vtkProcessModule (0x6ff960): Aborting execution for debugging purposes.}

Do you have any idea where to dig further?

Jens

Hello Jens, You downloaded
 

Hello Jens,

You downloaded the latest version of Paraview 3.3.0 from the anonymous CVS right? Or is there also a parallel SVN repository?

Anyway.... was just wondering.... if you downloaded a completely new version of paraview from CVS, then this also includes the original "vtkOpenFOAMReader.cxx" and "vtkOpenFOAMReader.h" files in the "<pv3_root>/VTK/IO" directory that comes with PV3.... this version of the reader is extremely old, and is not Takuya's version.

You need to replace these two files with the version written by Takuya, and then recompile paraview.

The error that you are obtaining basically says that the XML file which configures the graphical interface has been modified to use Takuya's version, but the openfoam reader compiled into Paraview does not contain those configuration settings.

Hope this helps :-)!

Have a nice day!

Philippose

Hi Philippose @You download
 

Hi Philippose

@You downloaded the latest version of Paraview 3.3.0 from the anonymous CVS right?

You are right it was anonymous CVS repository.

@Hope this helps :-)!

Yes it does I forgot to replace "vtkOpenFOAMReader.cxx" and "vtkOpenFOAMReader.h" files in the "<pv3_root>/VTK/IO" with the version written by Takuya.

Thanks

Jens

Hi paraview experts!, I hav
 

Hi paraview experts!,

I have a problem using the latest ParaView 3.3.0. When running paraview and loading a case.foam dir the following error pops up:

ERROR: In /home/frankl/OpenFOAM/linux/ParaView3/VTK/IO/vtkOpenFOAMReader.cxx, line 2424
vtkOpenFOAMReader (0x8b742a0): /home/frankl/OpenFOAM/frankl-1.4.1/run/tutorials/interFoam/damBreak/controlDict. foam contains no timestep data.

ERROR: In /home/frankl/OpenFOAM/linux/ParaView3/VTK/Filtering/vtkExecutive.cxx, line 757
vtkCompositeDataPipeline (0x8b75cf8): Algorithm vtkOpenFOAMReader(0x8b742a0) returned failure for request: vtkInformation (0x8b8b838

Let me describe the installation steps, which I followed:

1) Downloaded the latest ParaView 3.3.0 from the CVS repo.

2) I patched the reader using the 'patch -b -p0 < *.xml.diff' as described in the release notes of this new reader. I also replaced "vtkOpenFOAMReader.cxx" and "vtkOpenFOAMReader.h".

Then I did the following to compile paraview:

cd $HOME/OpenFOAM/linux/ParaView3
mkdir -p lib/paraview-3.3.0
cd $HOME/OpenFOAM/linux/ParaView3/lib/paraview-3.3.0
ccmake $HOME/OpenFOAM/linux/ParaView3
make
make install

In the case dir I created a sym link from /system/controlDict to controlDict.foam.

Is this the right way to compile and use the new paraview 3.3.0 ?? Using VTK files, my paraview installation seems to work correct....

Thanks and regards,
Frank

Hi Frank, Does it work with
 

Hi Frank,

Does it work with the /system/controlDict (without the controlDict.foam)?
Choose File -> Open -> Files of Type -> All Files (*)
and than OpenFoam. (all the way down!)

Jens

Hi Jens, That seems to wor
 

Hi Jens,

That seems to work! Apparently the compilation process was successful.

What does not work are the time dirs.....How do I visualise those ??

Regards, Frank

Never mind, it works! thanks J
 

Never mind, it works! thanks Jens,

Frank

ps: The time dirs are on a different tab compared to 2.4.

Hi Frank, so it look like y
 

Hi Frank,

so it look like your links "system/controlDict.foam" are at the wrong place or pointing to the wrong place?

Jens

PS. Paraview-3.3.0 rocks!!

Hi, Paraview 3.3.0 is real
 

Hi,

Paraview 3.3.0 is really fast !! It looks so much better, and more efficient (less clicks for same result).

The only thing what I miss is the interpolated point values to visualise smooth pressure and velocity. Now I use the "cell data to point data" filter, which works fine, but this is somewhat tedious when visualising different patches and different cell sets.....

Altogether it works very very well !!!

Regards, Frank

Hi Frank, Good Evening! And
 

Hi Frank,

Good Evening! And good to see you active again after a fairly long period of "apparent hibernation" :-)!

Could you expand a little on what you exactly meant, when you mentioned that its tedious to visualise different patches and cell sets using the "cell data to point data" filter in Paraview 3.3.0 ?

It would be great to get some feedback from everyone using the OpenFOAM reader for Paraview 3.x.x, to see what needs to be improved, what features need to be added, and which bugs need to be looked into.... :-)!

One question regarding Paraview 3.3.0 ... have you tried using the "Lookmark" feature in PV 3.3.0, with for example, the colour bar (legend) turned on, the data scaled to a specific range, and positioned at a specific view?

It seems to me, that the lookmarks generated by PV3 are much more primitive than the ones generated by the PV2 versions.... On loading a lookmark, I dont get back everything that was present in the scene when the lookmark was made.

Have you had the same problems too?

Regards,

Philippose

Hi Philippose! Concerning
 

Hi Philippose!

Concerning the hibernation period, I've been quit busy working on the improvement of the moving mesh methods. Right now, some nice results are within reach and the new paraview may be what I need.

What I mean by tedious is that, CellDataToPointData doesn't contain the patches. When visualising the data on a patch I need to use ExtractDataSets which only shows the blocks....It is a minor issue, everything (what I need) seems to work fine....

I'm not familiar with the lookmarks, but it seems to work fine with me. When I find any more problems, I'll post it here....

Furthermore, at first paraview 3.3.0 seems less responsive when the case is very large, I will test this in more detail....For extremely large cases, is there a way to run paraview in batch-mode to create the figures of each time separately. How to use the parallel paraview on a cluster with pbs queue-ing system ?

Regards, Frank

Hello again Frank, A quick
 

Hello again Frank,

A quick remark regarding your reply.....

In the latest reader from Takuya (which is posted in this thread), if you open an OpenFOAM case, and as the first operation if you run the "Cell Data to Point Data" filter on the mesh data, from then on, you should be able to view the patches as point data.

I havent had to use ExtractDataSets in Paraview 3.3.0 in order to view patches....

Anyway, here are a couple of screenshots....

http://www.cfd-online.com/OpenFOAM_D...ges/1/6481.jpg

http://www.cfd-online.com/OpenFOAM_D...ges/1/6482.jpg

http://www.cfd-online.com/OpenFOAM_D...ges/1/6483.jpg

http://www.cfd-online.com/OpenFOAM_D...ges/1/6484.jpg

Are we talking about the same thing :-)!? Or have I completely mis-understood you ??

Regards,

Philippose

Hi Philippose, I have some
 

Hi Philippose,

I have some problems with the lookmark tool:

If I create one I get an error message Source deleted with outputs attached. But this error is hard to reproduce.

I confirm that it is quite slow for larger cases but I think still faster than the paraview-2 versions.

improvements for me are:
-the Annotate Time filter
-Annotation "Show cube axes" they fit now with the geometry

some annoying thinks are:
-the color of the annotations is set to white per default, and I don't know where to change the default
-with "Show cube axes" per default the y- and z-axis are relative to the x-axis, This can't be changed at the moment. Right now I take the Transform Filter to solve this issue.
-the Offsets in the Slicing/Cutting Filter have no clear reference to the geometry Data. The frame of reference for the Slicing/Cutting Filter is not the same as for the geometry. So I have to transform it by hand which sucks.

But still I like the new paraview-3.3.x

Jens

Hi Philippose, In the prop
 

Hi Philippose,

In the properties tab from controlDict, all mesh regions (the patches) are available as well as the cell arrays for p and U.

When I create a "cellDataToPointData" filter on controlDict, I see nothing (only a button ("pass cell to data"), so I cannot select the patches of this "cellDataToPointData" filter.

Of course I should keep all patches and Inernal Mesh active in controlDict in order to visualise slices i.e.

Any ideas on how to active the patches in the "cellDataToPointData" filter ?

Regards, Frank

Hello again, Okkk... first
 

Hello again,

Okkk... first and foremost :-)! I was actually asking for feedback from users who use the "OpenFOAM reader in" paraview 3.x.x, and not the bugs and shortfalls of Paraview 3.x.x itself :-)! Though... no problems... if anyone involved in the development of Paraview is reading these posts, it would help.

And as for visualisation of the patches.... in Paraview 3.3.0, if you change the patch selection in the properties tab of "controlDict.foam", and press the "Accept" button, these changes are automatically carried down to all the downstream filters....

So... if you make the controlDict.foam tab (which contains the "cell" data) invisible (by clicking on the eye to the left of it), then change the patch selections, and finally press the "Accept" button, the "CellDatatoPointData" filter will only display the patches that are enabled in the "controlDict.foam" tab.

If you are still not clear, maybe I can try to come up with a short video using "Wink" :-)!

Have a nice day!

Philippose

Thanks for your time! In my op
 

Thanks for your time! In my opinion, paraview 3.3 is already very well suitable for the use with openfoam. Still I have a small problem when visualising a slice (cut) and the patches.

When I create a cut plane (i.e. to show contours) I need all patches selected in controlDict (especially Internal Mesh). Therefore, I have no success in generating a cut plane AND some patches (without the internal mesh).

Summarising:
1) For the patches: I need to switch off all patches in controlDict except the ones to visualise.
2) For the cut plane: I need to switch on all patches in controlDict, especially Internal Mesh.

I could be that I am not yet fully mastering the basic paraview features....any more ideas?

Good day to you too!!

Frank

Hi ParaView3 users, As a rece
 

Hi ParaView3 users,
As a recent overhaul in the dataset API of the ParaView 3.3 CVS head made the previous (20071023) version of the reader unusable, I made necessary changes to support the new API, in addition to some updates, to the reader, which resulted in a new release here.

The reader now supports the CVS head newer than Feb. 16, 2008 and the 3.2.1 released version. Major changes from the previous version are as follows.

Technical changes: The reader now

• has a builtin cell data to point data filter (not as accurate as the volPoint interpolator in paraFoam but better than the one in ParaView, see Notes).,
• decomposes polyhedral cells (so that you don't have to tetrahedralize).
• supports all combinations of vol/point/lagrangian-Scalar/Vector/SphericalTensor/SymmTensor/Tensor fields.
• handles all fields and point coordinates in single precision for performance and memory footprint reasons.
• has several Mac OS X Leopard specific (but should somewhat work for other OSes too) performance improvements for mid-large cases (> 2-3 million cells).
• outputs empty patches as zero-sized datasets. So you have to have a valid patch definition for every patch even e. g. for defaultFaces with nFaces 0. This change was made to keep the behavior of Extract Block filter as consistent as possible for topo-change cases.

Usability changes: Now you

• can open either an empty stub file <casename>.foam right under the case directory, where <casename> is an arbitrary string other than the strings that starts with "controlDict," or the symbolic link system/controlDict.foam (to system/controlDict) to load an OpenFOAM case. So if you use the stub files you can distinguish the cases in the Pipeline Browser when multiple cases are loaded simultaneously.
• no longer have to create the lagrangian/ subdirectory under the initial timestep directory to load a case with Lagrangians.
• won't see a blank white geometry after loading a case, since the reader now colorize with an appropriate scalar variable (typically CellToPoint/p).

Others:

• Lots of small fine tunings and bug fixes in many corner cases.

Please have a careful look through
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif ReleaseNotes
before proceeding, and try if you think it's worth trying.
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif vtkOpenFOAMReader-20080318.tar.bz2
I'd like to express my thanks again to Philippose Rajan for testing the code and having interesting and important discussions.

Regards,
Takuya

And here's a paraFoam-like scr
 

And here's a paraFoam-like script, pvFoam, to launch ParaView and load a case with the reader. You have to adjust the paraviewPath variable at line 34 to the path to ParaView. http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif pvFoam Takuya

Hi again ParaView3 Users, I
 

Hi again ParaView3 Users,

I noticed a rather silly compatibility problem with the Calculator filter, the detail of which is described here, after the release of the 20080318 version. I believe this is a bug in ParaView but anyway the confusing "CellToPoint/" and "Lagrangian/" prefixes had to be changed. Apologies for this frequent update.

Technical change:

• The naming schemes of point filtered arrays and Lagrangian arrays have been changed from CellToPoint/arrayName and Lagrangian/arrayName to CellToPoint[arrayName] and Lagrangian:arrayName so that the array names don't confuse the Calculator filter.

Usability change:

• Now you don't have to create a time directory only for viewing mesh under the constant subdirectory.

Other:

• Added a simple Python scripting example (pythonExample.py).

Here are and.

Takuya

Hi again ParaView3 Users, I
 

Hi again ParaView3 Users,

I noticed a rather silly compatibility problem with the Calculator filter, the detail of which is described here, after the release of the 20080318 version. I believe this is a bug in ParaView but anyway the confusing "CellToPoint/" and "Lagrangian/" prefixes had to be changed. Apologies for this frequent update.

Technical change:

• The naming schemes of point filtered arrays and Lagrangian arrays have been changed from CellToPoint/arrayName and Lagrangian/arrayName to CellToPoint[arrayName] and Lagrangian:arrayName so that the array names don't confuse the Calculator filter.

Usability change:

• Now you don't have to create a time directory only for viewing mesh under the constant subdirectory.

Other:

• Added a simple Python scripting example (pythonExample.py).

Here are http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif ReleaseNotes and http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif vtkOpenFOAMReader-20080324.tar.bz2 .

Takuya

Hi, at first thanks for thi
 

Hi,

at first thanks for this great reader!!!
i experienced some trouble visualizing lagrangian data. maybe somebody might explain how to do this with the new reader - is this working for binary lagr. data too?
thanx in advance
regards
stephan

hi, i am actually asking si
 

hi,

i am actually asking since i get errors like this:

ERROR: In /home/foam13/OpenFOAM/linux/ParaView3/VTK/IO/vtkOpenFOAMReader.cxx, line 5736
vtkOpenFOAMReader (0x871e620): Error reading line 28 of /home/foam13/OpenFOAM/foam13-1.4.1/run/reaktor/1/lagrangian/positions: Expected punctuation token ')', found ���Mb`?���R!��?0
so i am not sure if i do something wrong or if the reader cant handle binaries?
thanks
stephan

Hi Stephan, With which OF ver
 

Hi Stephan,
With which OF version did you run the case? The reader only supports lagrangian data created by OF version 1.4 or later (maybe I should have written that in the ReleaseNotes).

If the case is run with OF 1.4 or later, would it be possible to send me the problematic positions file? (just a single file will be fine)

Takuya

Hi Takuya, the file should
 

Hi Takuya,

the file should reach you in second. actually every binary position file seems to show the same problem?!
thanks for helping me!
best regards
stephan