[agunhan]

Hello All,

For my study, I am running a porous media in OpenFoam v2306. To save some computational cost I want to run it in 2D.
I set my front and back as patch at the beginning then I run blockMesh> snappyHexMesh -overwrite > extrudeMesh (front/back) > createPatch (front/back as empty).
But after creating the mesh I can check it on paraview. When I try to do decomposition I get error.
Does decomposition work with empty boundary conditions?

The error looks like this;

--> FOAM FATAL IO ERROR: (openfoam-2306)
Size 179028 is not equal to the expected length 41418

file: 0/cellLevel.internalField at line 21.

From void Foam::Field<Type>::assign(const Foam::entry&, Foam::label) [with Type = double; Foam::label = int]
in file ./src/OpenFOAM/lnInclude/Field.C at line 253.

FOAM exiting

Hint: I set the front and back as patch and named them as front1/back1 then using the createpatchdict named them front/back.

Thank you in advance.



%------------------SOLVED-----------%
For those who encounter the same problem.
The issue was the created mesh files in "0" file.
After running all the steps I restored the "0" file and I was able to run the simulation without any error.
cp -r 0.orig/ 0

blockMesh

snappyHexMesh -overwrite

topoSet

extrudeMesh

createPatch -overwrite

# Restore initial conditions in the 0 directory
restore0Dir

# Decompose the domain for parallel processing
decomposePar

# Run the simulation in parallel
mpirun -n 14 pimpleFoam >> log.pimpleFoam -parallel

[Yann]

Hello,

you don't need createPatch in your case, changeDictionary will be enough. (you don't need to create new patches, just to update the patch type for front and back)

This being said, this is not the cause of your error.

--> FOAM FATAL IO ERROR: (openfoam-2306)
Size 179028 is not equal to the expected length 41418

file: 0/cellLevel.internalField at line 21.

This message indicates a size mismatch between your mesh and the variables contained in the 0 directory.

cellLevel is a variable written by snappyHexMesh when you have some writeFlags activated in snappyHexMeshDict.

After running snappy and writing cellLevel variable, you modified your mesh with extrudeMesh, this is why you get this error. (cellLevel size does not match the size of your mesh anymore)

Just remove the variables written by snappy before decomposing your case and you should be fine.

[agunhan]

Originally Posted by Yann

Hello,

you don't need createPatch in your case, changeDictionary will be enough. (you don't need to create new patches, just to update the patch type for front and back)

This being said, this is not the cause of your error.

--> FOAM FATAL IO ERROR: (openfoam-2306)
Size 179028 is not equal to the expected length 41418

file: 0/cellLevel.internalField at line 21.

This message indicates a size mismatch between your mesh and the variables contained in the 0 directory.

cellLevel is a variable written by snappyHexMesh when you have some writeFlags activated in snappyHexMeshDict.

After running snappy and writing cellLevel variable, you modified your mesh with extrudeMesh, this is why you get this error. (cellLevel size does not match the size of your mesh anymore)

Just remove the variables written by snappy before decomposing your case and you should be fine.

Thank you, I will try it also without creatingpatch!!