[C-L]

Hi All,

I am currently experiencing a weird bug whereby my case is freezing after attempting to update the kinematic cloud, but only when decomposing my mesh in a certain way.

My case study models a particulate flow down a pipe, with cyclic boundary conditions placed at the ends and the LES-WALE turbulence model. When running in serial there are no errors and the solution seems reasonable. However, when decomposing the mesh (scotch or simple) in the z-direction the output file freezes at 'evolving kinematic cloud'. When decomposing the mesh in the (r,theta) directions the solver works again, but this seems like a very inefficient way to parallelise my pipe, especially when I start splitting it into 64 processors.

My case directory can be found on this dropbox link:

https://www.dropbox.com/s/qz9wpb5wt7...PM.tar.gz?dl=0

and I have attached the output file below.

I have changed the case file slightly so that it runs (with the same issues) on the standard DPMFoam solver rather than my altered one.

If someone could take a look at this I would be very grateful!

Thanks,
Charlie

[wyldckat]

Greetings Charlie,

The solution is simple, you need to use preservePatches in "system/decomposeParDict":

preservePatches (C1 C2);

numberOfSubdomains 4;
method          simple;

simpleCoeffs
{
    n    (4 1 1);
    delta    0.0001;
}

This way the two patches are in the same processor sub-domain, which allows for the algorithm to work properly.

For more details/examples, check the main example dictionary file, whose path is given by the following command:

echo $FOAM_UTILITIES/parallelProcessing/decomposePar/decomposeParDict

Best regards,
Bruno

[C-L]

Hi Bruno,

I had tried the preservePatch feature before but clearly I got the notation wrong because your fix worked straight away! Thanks for the help,
Charlie