Purpose

Advanced solver for coupled CFD-DEM simulations involving incompressible fluids. Supports dynamic meshes and transport of passive scalars.

Note

This model or solver is supported by CFDEMcoupling on GPU devices.

cfdemSolverPimple

Description

cfdemSolverPimple is a coupled CFD-DEM solver using CFDEMcoupling, an open source parallel coupled CFD-DEM framework. Based on pimpleFoam®(*), a finite volume based solver for Reynolds-Averaged (RANS) or filtered (LES) Navier-Stokes equations applying the PISO or PIMPLE algorithm, cfdemSolverPimple has additional functionality for a coupling to the DEM code “Aspherix”. The volume averaged Navier-Stokes Equations are solved accounting for momentum exchange and volume displacement of discrete particles whose trajectories are calculated in the DEM code Aspherix.

This solver can use a PIMPLE algorithm when specifying nOuterCorr greater than 1 in the PIMPLE sub-dictionary of CFD/system/fvSolution. Also, appropriate settings in relaxationFactors need to be specified in this case (see tutorials for all settings).

This solver is able to smoothen force coupling fields in order to allow for extreme particle (parcel) size to grid size ratios using a smoothing models.

Implicit force coupling will result in a typically small difference in the coupling force exerted on the particles and the fluid, i.e., Newton’s Third Law will be conflicted. This error can be calculated by TotalError(dU) = Ksl * (Uf_preStep-Uf_postStep), since CFD experiences new Uf values, while particles only experience drag with Uf_postStep. The expCorrDeltaUError can be included in CFD/constant/couplingProperties that will correct for this error in an explicit fashion. Typically, correcting for this error results in a less stable solution. The sum of this error normalized by the total implicit drag is displayed during the simulation.

This solver internally creates the following fields during the calculation of momentum exchange:

name

type

unit

default value

voidfraction

scalar

1

0

f

vector

kg/m²/s²

(0 0 0)

Ksl

scalar

kg/m³/s

0

Us

vector

m/s

(0 0 0)

rho

scalar

kg/m³

fluidDensity

Boundary conditions for these fields are set automatically on all patches to either zeroGradient or the appropriate geomeric constraint on the patch (e.g. cyclic, empty, etc.) depending on the patch type.

Note

This means that a user should only create files for these fields in the zero folder if different boundary conditions or initial values are desired. Most likely, this might occur for the voidfraction for which fixedValue boundary conditions might be desired at inlet and outlet if partcles cross these patches.

Literature

GONIVA, C., KLOSS, C., HAGER, A. and PIRKER, S. (2010): “An Open Source CFD-DEM Perspective”, Proc. of OpenFOAM Workshop, Göteborg, June 22.-24.

(*) This offering is not approved or endorsed by OpenCFD Limited, the producer of the OpenFOAM software and owner of the OPENFOAM® and OpenCFD® trade marks.