[Situla]

Hello!


So I have been struggling for a while now trying to open my vtu files in Paraview. The error I get is this:

ERROR: In C:\bbd\ecd3383f\build\superbuild\paraview\src\VTK\ IO\XML\vtkXMLUnstructuredDataReader.cxx, line 657 vtkXMLUnstructuredGridReader (0000024E05BE8EC0): Cannot read cell connectivity from Cells in piece 0 because the "offsets" array is not monotonically increasing or starts with a value other than 0.

I obtained this vtu file by running CFD_SOL on my solution_flow.dat, which I again obtained from renaming the restart_flow.dat that is written at the end of the simulation.
This is the second (and very small) of four vtu files of a multi-physics problem (gas flow past three warm cylinders).
Most sense I can make of the error is by opening the vtu file in Notepad++, where I found these three lines:
<Cells>
<DataArray type="Int32" Name="connectivity" NumberOfComponents= "1" offset="1816" format="appended"/>
<DataArray type="Int32" Name="offsets" NumberOfComponents= "1" offset="3452" format="appended"/>


I am not sure if this "offset" variable is the same as in the error message, but it is clearly not 0.
This is my first multi-physics SU2 simulation, so I am not very experienced with how to deal with this.

I have attached the entire vtu-file and the mesh file.


Thank you for your time!
Martin




Edit: Above error appears with Paraview 5.8.0. I have tried opening this same exact file in Paraview 5.6.1, where I find a similar yet different error:


ERROR: In C:\bbd\ecd3383f\build\superbuild\paraview\src\VTK\ IO\XML\vtkXMLUnstructuredDataReader.cxx, line 616 vtkXMLUnstructuredGridReader (000001D73D38B500): Cannot read cell connectivity from Cells in piece 0 because the "offsets" array is not monotonically increasing or starts with a value less than 1.



What strikes me as bizarre is that in this version, Paraview seems to expect an array starting value > 0, whereas in the newer version, it seems Paraview would accept ONLY 0 as starting value. Clearly, there is not a value that can satisfy both conditions, which raises two questions: What value does it really need to be, and what value does my file have?




Edit2: added MWE

[hdavidcogollo]

Hi Martin.

I have the same problem and I don´t know if you did resolve it, but if you run the same case in Linux generate a vtk file, I would appreciate that if you solve it, you would let me know. Thanks

[rn86j]

Same issues as Mr Martin and look forward to updates
Thanks

[TKatt]

Hi all,

can you please attach your cases including the conifg .cfg and mesh (e.g. .su2). Problem

I get the same error as OP when opening the .vtu.

It is generally a good idea to attach a reproducible setup when encountering a problem. Like that is much easier to get help

Cheers, Tobi

[ddubey01]

I've had this same problem in the past, and I solved by pasting the following into my configuration file: OUTPUT_FILES= PARAVIEW_ASCII

Upon adding this to your configuration file and running it, a working .vtk file should be outputted and ready for visualization on Paraview.

[Situla]

Hello ddubey01,


thank you very much for the suggestion. It does indeed create a processable output file!
You solved my problem, thank you!


Kind regards,
Martin

[rn86j]

Appreciated...
A neat engineering fix to use vtk rather than vtu… The issue then is the storage and time. I noted that vtu files are in, general, less than 30-40% of the size of the vtk files. For large meshes, this is a practical consideration.
I am sure there could be a small bug to be fixed eventually.
Thanks

[hdavidcogollo]

Hello ddubey01.

Thanks, it help me a lot, I also noticed that it can also be done with other output files like restart_flow and surface_flow.

[rn86j]

Very glad to see SU2-v7.0.6, (faster than v7.0.4)..
However....
As is the case with V7.0.5, the v7.0.6 vtu files generated also do not work with Paraview 5.8.0 (same issues). V7.0.4 vtu files work well
So, have to go back to v7.0.4 !
The vtk file ideas produce extremely long files.
So the question is do we await v7.0.7 ??

[pcg]

Hi,
Thank you for noticing also the good stuff.
.vtu files work for me with Paraview 5.4.1, I'll try to replicate the problem with 5.8.

Could you help us pinpoint when the problem was introduced by testing this snapshot of the code:
"git checkout a81b0acd9a57913da292ceb6f5c8da870ec5f14e"
(This was just before some fixes were introduced to allow support for grids with 200M+ nodes.)

Thanks,
Pedro

[pcg]

I downloaded 5.8.0 for Linux and I can open all my .vtu files.

I tried opening Martin's file and I see the same error with 5.4.1 and 5.8.0, I'll see if something can be done about the SU2 options.

[pcg]

I cannot replicate the problem, I ran Martin's case and I can open the .vtu files, either generated in parallel, serial, by SU2_CFD or by SU2_SOL.

Are y'all running Linux or Windows?

[rn86j]

Thanks Dr pcg for attempting to resolve the issue. Appreciated

Yes. I have tried running v7.0.6 in Windows with mpi with su2_cfd only

using latest Paraview 5.8.0, No such problems on vtu files generated by v7.0.4

Looks like sum small bug when SU2 was upgraded from v7.0.4 to v7.0.5, ie. from vtk files to vtu files (to reduce the file size)

[dadadan93]

Hello Could you please share which config file to edit? Is it in the VTK-Files or in generation of the .vtu file?


Thank you in advance !
Daniel

Originally Posted by ddubey01

I've had this same problem in the past, and I solved by pasting the following into my configuration file: OUTPUT_FILES= PARAVIEW_ASCII

Upon adding this to your configuration file and running it, a working .vtk file should be outputted and ready for visualization on Paraview.

[rn86j]

Trying to work with vtu files as they are very much smaller than vtk files. This makes a great difference for larger meshes.

The su2v7.0.6 is some 20% faster than Su2 v7.0.4 (both running in mpi mode). So we hope the next version of SU2 will work. After all v7.0.4 is fine and I have to use this version at present.

Noted that Paraview 5.8.1 is imminent (trial version exists already) and it may be a good idea to try that out.
Thanks

[pcg]

We (another developer and I) think we know what might be the issue on Windows:
https://github.com/su2code/SU2/pull/1055

If you build the code from source you can checkout this branch: https://github.com/su2code/SU2/tree/...ows_vtu_output
I do not have access to a Windows machine, so I would really appreciate if any of you could give it a try.

[hkim716]

I have the same problem, how can I solve this problem?

I think .vtu file is not compatible with Paraview, and I don't know we produce .vtk file from SU2.
Please let me know anyone solved this issue. T^T

[rn86j]

I can confirm that problem still exists with MPI/windows SU2 7.0.6 generated vtu files and the latest version of Paraview 7.8.1.


Vtu files from SU2 7.0.4 work with Paraview 7.8.1

We need the help of Windows/MPI experts as Dr Pedro Gomez mentioned,

Thank You

[pcg]

7.0.6 is not going to change... it will never work.

The aforementioned fix was reported as successful by one of the developers.
It will be included in 7.0.7, so you can either:
- Wait for 7.0.7;
- Build the develop branch from source;
- Download the "nightly" build https://github.com/su2code/SU2/actions/runs/203927718

[hkim716]

Thank you for quick reply guys.
Once I tried to run SU2 on Linux operating system, the problem solved.
I think .vtu file from Windows gave me the error. Thanks!