[DrFloyd]

Hello to everybody,
I just compiled openfoam 3.0.x in a machine with intel i7-6700hq. Everything went good, but when I use "foamToVtk" I received the follow error:

--> FOAM FATAL ERROR:
floatScalar and/or label are not 4 bytes in size
Hence cannot use binary VTK format. Please use -ascii

From function foamToVTK
in file foamToVTK.C at line 335.

FOAM exiting

Anyone has any idea of how solve this (different from "foamToVtk -ascii"?)
Thankyou for your attention

[wyldckat]

Quick answer: Apparently you built OpenFOAM 3.0.x with 64-bit labels, which the VTK legacy format does not support when using binary format. That's why the utility is advising you to use the "-ascii" option.

Do you really need 64-bit labels? Do any of your meshes have more than 2^31 elements in them?

PS: I've moved the thread to the OpenFOAM Paraview & paraFoam.

[DrFloyd]

Dear wyldckat,
thankyou for your very clear answer.

[wyldckat]

I did forget to mention a few details:

• If you do need 64-bit labels, e.g. to prepare cases to be executed in another machine that has more RAM, I guess that would be a valid scenario...
• I did look into enabling 64-bit integers in the VTK format, but sadly it wasn't possible... see the following wiki page for more details on my findings: https://github.com/wyldckat/wyldckat...VTK_FileFormat
• You can open the cases with 64-bit labels directly in ParaView, if you use OpenFOAM's reader for ParaView.

[sandeep.pandey]

Hey Bruno,

Thank you for explanation and now I understand this problem. It persists in OpenFOAM v5.x. I did my simulations at cluster with OpenFOAM v2.4 and now after the up-gradation to v5.x and I am having the same warning message. I don't have paraFOAM on the local system, therefore, I always use FoamToVTK and currently with ascii, the file size is very big (with ~20 Mio. cells). So do you have any idea with the existing compiled version of OpenFOAM on the cluster?
I tried to compile your commit from github but the output is was again in ascii.

Thanks,
Sandeep

[wyldckat]

Quick answer: You can try opening the case with the file extension ".foam". For example, create an empty file "case.foam" inside the case folder and then open that file in ParaView. This will make ParaView open the case with the internal ".foam" reader.

If you are going to do this, then try using the more recent versions of ParaView, either 5.4.1 or 5.5.0.

[sandeep.pandey]

Hi,

Thanks for the reply. Actually, I've tried it with Paraview 5.1.0 (64 bit) but it wasn't able to open the file. Maybe I should give it a try with the version you have mentioned.

Thanks again,
Sandeep

[wyldckat]

Quick answer:

• I can't remember which ParaView 5.? minor version, but there was one that didn't open the more recent OpenFOAM cases properly with the ".foam" file reader... but I can't remember which one... maybe it was 5.2? I can't remember...
• Make sure you bring the whole case into your machine, and if the case is not reconstructed, then use the reader option (shown in the UI) for loading the decomposed case.
• As of ParaView 5.3 or 5.4, the .foam reader will ignore the "0" time folder by default, unless you choose to also load it.

[sandeep.pandey]

Thank you for the prompt reply! I end up switching to Linux and start using ParaFOAM. It was an easier option than keep trying or fixing things