[Mahdi_Kh]

Hi everyone,

I am using icoUncoupledKinematicParcelFoam in OpenFoam 2.206 for tracking of particles. I am using simple method for parallel processing to run the simulations on 6 cores. When I am using decomposePar on my PC, everything is fine and simulations are run, but when I take the simulations to run on HPC with the same setting as that on pc, I get this error although it is being decomposed on 1 node with the same 6 cores using simple method:

--> FOAM FATAL ERROR: (openfoam-2206 patch=221104)
[5] Particle tracking across AMI patches is only currently supported for cases where the AMI patches reside on a single processor.

Does anyone have some ideas why this happens?
Thank you so much all.

[lxufeishi]

As shown in the error message, the AMI patches should be distributed to the same processor in parallel running. We can use "singleProcessorFaceSets" constraint for this:

1. Use topoSet to assemble the AMI patches (often in pairs) to FaceSets.

actions
(
    {
        name    AMI_faceSets1;
        type    faceSet;
        action  new;
        source  patchToFace;
        sourceInfo
        {
            name "(AMI-interface1-2|AMI-interface2-1)";
        }
)

2. Add the "singleProcessorFaceSets" constraint in the decomposeParDict:

singleProcessorFaceSets 
(
        (AMI_faceSets1 -1)
);

3. decomposePar and run in parallel.

For more details, check the attached test case, especially the decomposePar_annotated file. The case is run with OpenFOAM-2112 but is compatible for OpenFOAM-7. An example of the results:

[Mahdi_Kh]

Thank you so much for your detailed and exact description of the solution lxufeishi!!

It is interesting that you use icouncoupled with pimplefoam. I thought it is only for when you have the velocity field. I need actually for an unsteady solution. Can I use the same functions you have for my own problem?

Thank you,
Mahdi.

[lxufeishi]

Originally Posted by Mahdi_Kh

It is interesting that you use icouncoupled with pimplefoam. I thought it is only for when you have the velocity field. I need actually for an unsteady solution. Can I use the same functions you have for my own problem?

Yes, the function can run with the transient solvers so the particle will be driven by the unsteady velocity field.

[Mahdi_Kh]

Hi lxufeishi,
Thank you for your reply again. Can you please explain a bit what changes you have made in the solver to run it with pimpleFoam? Can the solver you have developed be used for any transient case? or it is case-specific?

Thank you.

[lxufeishi]

Originally Posted by Mahdi_Kh

Can you please explain a bit what changes you have made in the solver to run it with pimpleFoam? Can the solver you have developed be used for any transient case? or it is case-specific?

Actually, I didn't make any change to the solvers but just add a "icoUncoupledKinematicCloud" type function in the controlDict. If you set your case properly (e.g. kinematicCloudProperties), then you can run your solver (steady or transient) together with the lagrangian particle tracking function. It is a built-in feature of OpenFOAM.

You may find the following tutorial helpful.
https://www.cemf.ir/residence-time-d...ticle-tracing/

Cheers,