restarting CFDEM simulations

Are you using the Allrun-Script provided in the tutorial? If I remember right, in a last step the simulation directory is cleaned if you do not quit with ctrl+C. Maybe this applies in your case.

There is an additional thing to do. Please refer to the example, "ErgunTestMPI_restart".
Check the liggghtsCommands file in CFD/constant to write write_file for restarting.
Without this, it will read the restart file written by the initial LIGGGHTS run.

One important observation to do here is that OpenFOAM will not reconstruct the lagrangian folder when reconstructing your case (one can check the lagrangian folder in a time directory inside a processor directory). OpenFOAM will complain about a ponctuation token.

The lagrangian folder contains the information about the particles positions for paraview. So even if you reconstruct your case, you will lose these informations. The correct way to restart a simulation, is by making a backup of your CFD and DEM results before restarting. This way you will prevent the loss of data.

Hello

I am facing exact same problem when I restart cfdem simulation from last time step, I get the processors (and the results) removed where my existing results are present. Reonstructing is not an option as it looses the lagrangian data. backing up the data and then starting from latest time step is quite time consuming and not an efficient way to do it.

I was thinking about modifying the source code and remove the section which removes the processors and the recompile cfdem again. But this is also very complicated and recompiling complete cfdem on super computer is a challange.

I was wondering if someone know any efficient method to do it.

Best Regards
Atul Jaiswal

I have managed to restart the CFDEM simulation from previous time step without being the previous time step data being removed from the processors folder. I am providing the solution here in case someone needs it.

Most important thing is to create a new liggghts restart script (e.g. in.liggghts_restart) where one need to read the previously written CFDEM restart file. Then we need to indicate the openfoam to read in.liggghts_restart script. This is done by modifying couplingProperties file (CFD/constant), where we just replace the file name in.liggghts_run with in.liggghts_restart in the section twoWayMPIProps and twoWayM2MProps. it is also betetr to change the name of the restart file written during this restart simulation, that is done by changing the name of restart file under writeName. Additionally the startTime should be changed to latestTime in CFD/system/controlDict. Now the case is ready to be started to from previous run. But usiing Allrun.sh (which calls the function parCFDEMrun) would remove all the processors then again decompose the case. This happens because, the funtion parCFDEMrun first executes decoposePar -force then calls cfdemSolverPiso in parallel. We just have to tell that we dont need again decoposition and use the existing decoposed case. The easiet way to do it is by calling directly cfdemSolverPiso in parallel instead of function parCFDEMrun. just modify the parCFDEMrun.sh, where we call cfdemSolverPiso in parallel as follows:

cd CFD
mpirun -np cfdemSolverPiso -parallel

Now, when you execute Allrun.sh, your simulation will start from last time step without removing previous data.
I hope, it will help others.

Best Regards
Atul Jaiswal

Hello

you should remove everything and just call the two commands mentioned below (after #- call function to run a parallel CFD-DEM case)

cd CFD
mpirun -np cfdemSolverPiso -parallel

As said no need to call parCFDEMrun