CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Visualization & Post-Processing Software > ParaView

[OpenFOAM] paraFoam error message on interPhaseChangeDyFoam propeller tutrial

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

Like Tree4Likes
  • 1 Post By wyldckat
  • 1 Post By wyldckat
  • 2 Post By MaySea

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 22, 2018, 04:53
Default paraFoam error message on interPhaseChangeDyFoam propeller tutrial
  #1
jcw
New Member
 
Christian Wolf
Join Date: Mar 2009
Posts: 24
Rep Power: 13
jcw is on a distinguished road
Hello!


I am working with the following tutorial:
OpenFOAM-4.1/tutorials/multiphase/interPhaseChangeDyMFoam/propeller


The case runs with 'Allrun', but I face a problem showing the results in paraFoam. When clicking the button 'Apply' in paraFoam, I receive the following error message:


Quote:
ERROR: In /xxx/xxx/OpenFOAM/v410/OpenFOAM/ThirdParty-4.1/ParaView-5.0.1/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 4674
vtkOpenFOAMReaderPrivate (0x2fffca0): Error reading line 149 of /xxx/xxx/OpenFOAM/yyyy-2.0.x/run/OF41/propeller/constant/polyMesh/faces: Expected punctuation token ')', found




ERROR: In /xxx/xxx/OpenFOAM/v410/OpenFOAM/ThirdParty-4.1/ParaView-5.0.1/VTK/Common/ExecutionModel/vtkExecutive.cxx, line 784
vtkPVCompositeDataPipeline (0x2fda300): Algorithm vtkPOpenFOAMReader(0x2ffe3a0) returned failure for request: vtkInformation (0x10a1f50)
Debug: Off
Modified Time: 196057
Reference Count: 1
Registered Events: (none)
Request: REQUEST_DATA
ALGORITHM_AFTER_FORWARD: 1
FORWARD_DIRECTION: 0
FROM_OUTPUT_PORT: 0
It also fails when loading a different time step.

The mentioned file ./constant/polyMesh/faces looks like binary code:
Quote:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format binary;
class faceCompactList;
location "constant/polyMesh";
object faces;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


1639612
(^@^@^@^@^@^@^@^@^D^@^@^@^@^@^@^@^G^@^@^@^@^@^@^@^ K^@^@^@^@^@^@^@^O^@^@^@^@^@^@^@^S^@^@^@^@^@^@^@^W^ @^@^@^@^@^@^@^[^@^@^@^@^@^@^@^^^@^@^@^@^@^@^@"^@^@^@^@^@^@^@&^@^@ ^@^@^@^@^@*^@^@^@^@^@^@^@.^@^@^@^@^@^@^@2^@^@^@^@^ @^@^@6^@^@^@^@^@^@^@:$
^C^@^@^@^@^@^@^N^C^@^@^@^@^@^@^R^C^@^@^@^@^@^@^V^C ^@^@^@^@^@^@^Z^C^@^@^@^@^@^@^^^C^@^@^@^@^@^@"^C^@^ @^@^@^@^@&^C^@^@^@^@^@^@*^C^@^@^@^@^@^@.^C^@^@^@^@ ^@^@2^C^@^@^@^@^@^@6^C^@^@^@^@^@^@:^C^@^@^@^@^@^@> ^C^@^@^@^@^@^@C^C^@^@^@^@^@^@H^C^@^@$
^@^@^@^@^@^@^D
^@^@^@^@^@^@^H
^@^@^@^@^@^@
^@^@^@^@^@^@^Q
^@^@^@^@^@^@^U
^@^@^@^@^@^@^Y
^@^@^@^@^@^@^]
.
.
.
What is going wrong?
jcw is offline   Reply With Quote

Old   December 13, 2018, 08:57
Default
  #2
jcw
New Member
 
Christian Wolf
Join Date: Mar 2009
Posts: 24
Rep Power: 13
jcw is on a distinguished road
Really no idea?
jcw is offline   Reply With Quote

Old   December 22, 2018, 10:53
Default
  #3
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,958
Blog Entries: 45
Rep Power: 122
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answers:
  1. The thread was originally on the main ParaView forum and since is a question regarding paraFoam, there are fewer people there who could try and answer to this issue. And around this time of the year, those who have more knowledge, also have more responsibilities and are fighting to get things done before the holidays and the end of the year. Therefore you were challenging the odds of getting an answer
  2. ParaView 5.0.1 is being used with its internal reader, which was unable to open the case, likely due to a compatibility problem.
  3. My suspicion is that the OpenFOAM 4.1 version you are using is built with 64-bit labels (integers), instead of the more common 32-bit labels (integers). Therefore, the only workaround is to export the case data to VTK format with the utility foamToVTK, or download and install a more recent ParaView version that has a more recent internal reader.
mcfdma likes this.
__________________
wyldckat is offline   Reply With Quote

Old   July 17, 2019, 11:39
Default motorBike tutorial not working
  #4
New Member
 
Jan M
Join Date: Nov 2018
Posts: 25
Rep Power: 4
MaySea is on a distinguished road
Hello everyone,
I am new to OpenFOAM and CFD in general. I have watched and read multiple tutorials though, searched for a solution to the question below for many hours and could not find it.

I'm trying to run the motorBike tutorial in OpenFOAM 6. Firstly, I did it with Allrun, then tried "manually" doing each step. Both attempts ended up in this error, when trying to visualise the project in ParaView:

Code:
In C:\bbd\ecd3383f\build\superbuild\paraview\src\VTK\IO\Geometry\vtkOpenFOAMReader.cxx, line 5463
vtkOpenFOAMReaderPrivate (000002A31F00F6A0): Error reading line 24971 of D:\....\motorBike\constant/polyMesh/faces: Expected punctuation token ')', found 

ERROR: In C:\bbd\ecd3383f\build\superbuild\paraview\src\VTK\Common\ExecutionModel\vtkExecutive.cxx, line 782
vtkPVCompositeDataPipeline (000002A32F010C20): Algorithm vtkPOpenFOAMReader(000002A32F3B07C0) returned failure for request: vtkInformation (000002A330273980)
  Debug: Off
  Modified Time: 318329
  Reference Count: 1
  Registered Events: (none)
  Request: REQUEST_DATA
  FORWARD_DIRECTION: 0  ALGORITHM_AFTER_FORWARD: 1
  FROM_OUTPUT_PORT: 0
I checked polyMesh/faces file and it does not look healthy:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      binary;
    class       faceCompactList;
    location    "constant/polyMesh";
    object      faces;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


1103393
(                         "   '   +   0   4   8   <   A   F   J   O   S   W   [   `   d   i   m   q   u   z      ƒ   ‡   ‹      “   ˜                                                                                            !  %  )  .  3  8  <  @  D  H  L  Q  W  \  a  e  i  m  q  u  y  }    ‡  ‹    “  —  ›  Ÿ                                                            !  &  +  /  3  7  ;  @  D  H  L  P  T  X  \  `  d  h  l  p  t  x  |    †  Š    “  ˜  œ  *      *                                            
            "  &  +  0  4  9  >  B  F  J  N  R  V  Z  _  d  h  l  p  t  x  |  €  „  ‰  Ž  “  —  œ  *                                                  
            "  '  +  /  3  8  <  @  D  H  L  P  U  

[...]
motorBike.emesh file looks similarly. I also wasn't able to visualise mesh after applying blockMesh and snappyHexMesh.

This is the the sequence of commands I'm using, when performing everything manually:

Meshing:

Rename 0 folder 0.org
blockMesh
surfaceFeatures
decomposePar
mpirun -np (number of cores) snappyHexMesh -overwrite -parallel
reconstructParMesh -constant
delete all processor folders
delete folder 0
rename folder 0.org to 0

Simulation:

decomposePar
mpirun -n (number of cores) renumberMesh -overwrite -parallel
mpirun -np (number of cores) simpleFoam -parallel
reconstructPar -latestTime

I copied the motorbike.obj from the geometry resources in FOAM_TUTORIALS. Paraview does not have any issues with the visualization of the object and the file looks OK with all the regions defined inside.

Thank you for any help. Hope I targeted the forum properly.

Last edited by MaySea; July 18, 2019 at 06:49.
MaySea is offline   Reply With Quote

Old   July 18, 2019, 09:39
Default
  #5
New Member
 
Jan M
Join Date: Nov 2018
Posts: 25
Rep Power: 4
MaySea is on a distinguished road
Anybody? I feel like I'm missing something easy here.

----

@jcw did the answer provided by @wyldckat work for you?

I'm facing very similar issues, with the most recent version of ParaView and OpenFOAM 6 when executing Allrun for a motorBike tutorial. Did you find the solution?

Cheers.

Last edited by wyldckat; July 18, 2019 at 19:32. Reason: Merged posts a few minutes apart
MaySea is offline   Reply With Quote

Old   July 18, 2019, 19:39
Default
  #6
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,958
Blog Entries: 45
Rep Power: 122
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick questions @MaySea:
  1. Which installation instructions did you follow?
  2. In which operating(s) system(s) are you running OpenFOAM and ParaView?
Because from what I can deduce:
  1. Perhaps you built a version with 64-bit labels?
    • You can confirm which label (integer) type you are using with OpenFOAM by running this command:
      Code:
      echo $WM_LABEL_OPTION
  2. It looks like you might be running ParaView on Windows?
    • If you are, then you are likely using the file extension ".foam", then depending on the version of ParaView that you are using, there should be an option for using 64-bit labels, if you have that build of OpenFOAM. For example, see the attached image.
Attached Images
File Type: png Screenshot from 2019-07-18 23-38-40.png (26.6 KB, 24 views)
wyldckat is offline   Reply With Quote

Old   July 19, 2019, 06:59
Default
  #7
New Member
 
Jan M
Join Date: Nov 2018
Posts: 25
Rep Power: 4
MaySea is on a distinguished road
Hi @wyldckat

1. OpenFOAM was installed by an HPCC admin in my institution.
2. I am running OpenFOAM via HPC cluster with linux installed. The OpenFOAM is using 32-bit labels, as concluded by echoing like you suggested. I'm copying the cases from HPCC Linux to visualize them on a PC Windows, as ParaView can't be installed on HPCC. The ParaView is x64 bit. I am indeed creating the .foam file to visualize them.


I guess that if its the matter of labels like you suggest, the next step will be to consult the problem with the admin. Prob they had these issues before.

What's weird is that I performed other, basic simulations using simpleFoam on the same setup and they worked well. The only difference is that I used some downloaded .stl geometry, not .obj copied from the tutorials.

Thanks for the engagement.
MaySea is offline   Reply With Quote

Old   July 19, 2019, 08:21
Default
  #8
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,958
Blog Entries: 45
Rep Power: 122
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer: Oh, then this might be a problem with the Endianess... what I mean is that the HPC system you are using, might be ordering the values in one way, but on the workstation is uses the other order.


There is an old thread on this topic: Big-endian to little-endian conversion. How to do it in OpenFOAM?


You can check the type of Endianess the HPC system is using if you run:
Code:
uname -a
which will tell you the architecture and from there it's possible to look for what type of Endianess is uses.
MaySea likes this.
wyldckat is offline   Reply With Quote

Old   July 22, 2019, 04:50
Default
  #9
jcw
New Member
 
Christian Wolf
Join Date: Mar 2009
Posts: 24
Rep Power: 13
jcw is on a distinguished road
Quote:
Originally Posted by MaySea View Post
Anybody? I feel like I'm missing something easy here.

----

@jcw did the answer provided by @wyldckat work for you?

I'm facing very similar issues, with the most recent version of ParaView and OpenFOAM 6 when executing Allrun for a motorBike tutorial. Did you find the solution?

Cheers.

Sorry. I have not been sucessful. It is still not working.
jcw is offline   Reply With Quote

Old   July 24, 2019, 11:41
Default
  #10
New Member
 
Jan M
Join Date: Nov 2018
Posts: 25
Rep Power: 4
MaySea is on a distinguished road
I checked the endianess. Assuming by default that Windows runs on little endian bytes, there should not be any conflict, as the HPCC linux is little endian too:
Code:
[...] $ lscpu | grep "Byte Order"
Byte Order:            Little Endian
Looking for some other solutions. Will update in case of success...
MaySea is offline   Reply With Quote

Old   July 25, 2019, 19:42
Default
  #11
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,958
Blog Entries: 45
Rep Power: 122
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer @MaySea: Please try running OpenFOAM's tutorial case "incompressible/icoFoam/cavity/cavity" on the HPC system. You only need 1 core, but make sure you launch it in a job and not on the login node. I say this because the login node might be Little Endian, but the HPC nodes might be Big Endian...

But before running the case, check if the file "system/controlDict" has the "writeFormat" line set to "binary" and not "ascii".

You can run the case with this command:
Code:
foamRunTutorials
or with these two:
Code:
blockMesh
icoFoam
Then package the resulting case folder in a ZIP or tar.gz file and attach it to your next post. That way I can inspect the case and confirm what kind of binary data format it's being used.
wyldckat is offline   Reply With Quote

Old   July 29, 2019, 10:26
Default
  #12
New Member
 
Jan M
Join Date: Nov 2018
Posts: 25
Rep Power: 4
MaySea is on a distinguished road
@Wyldckat, so...

I just changed the writeFormat in controlDict to ascii from binary and it obviously worked well. When its set to binary its probably the endianess problem, as indeed its the login node which I checked to be little endian, not the batch job nodes.

I don't need a binary format, so changing to ascii solves the problem for me.

Thank you.
wyldckat and ashish.vinayak like this.
MaySea is offline   Reply With Quote

Reply

Tags
error, interphasechangedymfoam, parafoam, propeller, tutorial

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM.com] paraFoam cannot open due to Qt issues - [Solved/Information] u2berggeist OpenFOAM Installation 2 July 2, 2018 18:03
Error with snappyHexMesh when using another propeller in propeller tutorial quarkz OpenFOAM Running, Solving & CFD 3 March 28, 2018 03:54
how to run the propeller Tutrial immortality OpenFOAM Running, Solving & CFD 10 February 22, 2014 10:33
[OpenFOAM] OpenFoam (Ubuntu): paraFoam via Xming+PuTTY raketenmaid ParaView 4 February 5, 2013 06:20
Modelling a propeller tomg STAR-CCM+ 4 April 28, 2011 18:22


All times are GMT -4. The time now is 22:19.