Solver name: rhoCfdemSolverPimple Compressible, Isothermal, CFDEM coupled solver, with PIMPLE algorithm

Testing Status

• Reproduces incompressible cfdemSolverPiso ErgunMPI tutorial, with constant properties (that is, incompressible, with particles)
• Reproduces rhoPimpleFoam tutorials (e.g., cavity, pitzDaly, sqBendLiq) without particles (that is, compressible, without particles)

Currently we do not have a benchmark for compressible, with particles

Solver name: rhoCfdemSolverPimpleScalar Compressible, Isothermal, CFDEM coupled solver, with PIMPLE algorithm and scalar transport

Note: A compressible radiation model has not been developed. Radiation is not enabled with rhoCfdemSolverPimpleScalar!

• CFDEM 3.8.0
• LIGGGHTS 3.8.0

• rhoCfdemSolverPimple: Combines cfdemSolverPiso with rhoPimpleFoam
• rhoCfdemSolverPimpleScalar: Combines CfdemSovlerPisoScalar with rhoPimpleFoam

• Place the contents of the solver directory in $CFDEM_SOLVER_DIR
• Ensure the compressible CFDEM library is installed.
• Within the rhoCfdemSolverPimple directory, type wclean then wmake
• Place the contents of the tutorial directory in $CFDEM_TUT_DIR
• Optionally, add rhoCfdemSolverPimple/dir to the last line of solver-list.txt, located in $CFDEM_SRC_DIR/lagrangian/cfdemParticle/etc. If this edit is made, then rhoCfdemSolverPimple will automatically compile with the cfdemCompCFDEMsol command
• Within the rhoCfdemSolverPimpleScalar directory, type wclean then wmake
• Place the contents of the tutorial directory in $CFDEM_TUT_DIR
• Optionally, add rhoCfdemSolverPimpleScalar/dir to the last line of solver-list.txt, located in $CFDEM_SRC_DIR/lagrangian/cfdemParticle/etc. If this edit is made, then rhoCfdemSolverPimpleScalar will automatically compile with the cfdemCompCFDEMsol command

• These solvers have ONLY been tested with OpenFOAM 5.x
• The units for 0/p in the CFDEM ErgunMPI & packedBedTemp tutorials are changed relative to cfdemSolverPiso/cfdemSolverPisoScalar: Because the new solvers are incompressible, the units for pressure is now in Pa
• LIGGGHTS coupling can be enabled or disabled with the "switch" found in caseDir/system/couplingParameters. An example is found in the ErgunMPI test case included here. To run standard OpenFOAM tutorials, LIGGGHTS coupling must be disabled, as described below.

To use the solver in rhoPimpleFoam (no particles) format, use the following setting in caseDir/system/couplingParameters

enableCoupling          off;

To use the solver in CFDEM mode (particles), use the following setting in caseDir/system/couplingParameters

enableCoupling          on;

• CFDEM Tutorial ErgunMPI returns a similar result to cfdemSolverPiso. See tutorials/rhoCfdemSolverPimple/ErgunMPI.

• OpenFOAM tutorial rhoPimpleFoam/cavity can be reproduced with rhoCfdemSolverPimple. See tutorials/rhoCdemSolverPimple/cavity tutorial.

• OpenFOAM tutorial rhoPimpleFoam/pitzDaly can be reproduced with rhoCfdemSolverPimple. See tutorials/rhoCdemSolverPimple/pitzDaly tutorial.
• Left video - rhoCfdemSolverPimple (but LIGGGHTS coupling is disabled)
• Right video - OpenFOAM 5.x rhoPimpleFoam

• OpenFOAM tutorial rhoPimpleFoam/sqBendLiq can be reproduced with rhoCfdemSolverPimple. See tutorials/rhoCdemSolverPimple/sqBendLiq tutorial.

• CFDEM tutorial settlingTestMPI returns a similar result to cfdemSolverPiso. See tutorials/rhoCfdemSolverPimple/settlingTestMPI.

• CFDEM Tutorial packedBed returns a similar result to cfdemSolverPiso. See tutorials/rhoCfdemSolverPimpleScalar/packedBedTemp.
• Results

1. 0 directory

• Convert 0/p from incompressible units to compressible units, and adjust for the difference between gauge and absolute pressure. For example, 0 pressure in an incompressible tutorial is ~1E5 Pa in a compressible tutorial.

• Add a file for temperature in 0/T.

• Create a file for rho and adjust to the value of rho in the incompressible tutorial. Often this is found in the octave file for post processing. For an incompressible tutorial, pressure = p/rho and viscosity is kinematic viscosity (mu/rho), so the value of rho must be found from the post processing of an incompressible case.

2. system directory

• Add a couplingProperties file to the system directory. This allows OpenFOAM tutorials, without any CFDEM interaction, to run in the event system/couplingParameters enableCoupling is set to off

3. constant directory

• In the constant directory, transportProperties is replaced by thermophysicalProperties. Be sure to set rho and mu accordingly. Often rho can be found in the octave file in an incompressible CFDEM tutorial. Meanwhile, viscosity, mu, is equal to nu * rho, where nu is the kinematic viscosity in the incompressible case.

4. Search for the solver name (e.g., grep -r cfdemSolverPiso) and replace all instances of the incompressible solver name with the name of the compressible solver (e.g., rhoCfdemSolverPimple)