CFD-DEM coupled simulations with Yade and OpenFOAM

The FoamCoupling engine provides a framework for Euler-Lagrange fluid-particle simulation with the open source finite volume solver OpenFOAM. The coupling relies on the Message Passing Interface library (MPI), as OpenFOAM is a parallel solver, furthermore communication between the solvers are realised by MPI messages. The FoamCoupling engine must be enabled with the ENABLE_MPI flag during compilation:

cmake -DCMAKE_INSTALL_PREFIX=/path/to/install /path/to/source -DENABLE_MPI=1

Yade sends the particle information (particle position, velocity, etc. ) to all the OpenFOAM processes. Each OpenFOAM process searches the particle in the local mesh, if the particle is found, the hydrodynamic drag force and torque are calculated using the fluid velocity at the particle position (two interpolation methods are available) and the particle velocity. The hydroynamic force is sent to the Yade process and it is added to the force container. The negative of the particle hydrodynamic force (interpolated back to the fluid cell center) is set as source term in the Navier-Stokes equations. The OpenFOAM solver must also be installed to facilitate the MPI connection between Yade and OpenFOAM. Technical details on the coupling methodology can be found in [Kunhappan2017] and [Kunhappan2018].


In the standard Euler-Lagrange modelling of particle laden multiphase flows, the particles are treated as point masses. Two approaches are implemented in the present coupling:

  1. Point force coupling
  2. Volume fraction based force coupling.

In both of the approaches the flow at the particle scale is not resolved and analytical/empirical hydrodynamic force models are used to describe the fluid-particle interactions. For accurate resolution of the particle volume fraction and hydrodynamic forces on the fluid grid the particle size must be smaller than the fluid cell size.

Point force coupling (icoFoamYade)

In the point force coupling, the particles are assumed to be smaller than the smallest fluid length scales, such that the particle Reynolds Number is \(Re_{p} < 1.0\). The particle Reynolds number is defined as the ratio of inertial forces to viscous forces. For a sphere, the associated length-scale is the diameter, therefore:

(1)\[Re_{p} = \frac{\rho_{f}|\vec{U}_{r}|d_{p}}{\mu}\]

where in (1) \(\rho_{f}\) is the fluid density, \(|\vec{U}_{r}|\) is the norm of the relative velocity between the particle and the fluid, \(d_{p}\) is the particle diameter and \(\mu\) the fluid dynamic viscosity. In addition to the Reynolds number, another non-dimensional number that characterizes the particle inertia due to it’s mass called Stokes number is defined as:

(2)\[St_{k} = \frac{\tau_{p} \left| \vec{U}_{f} \right|}{d_{p}}\]

where in equation (2) \(\tau_{p}\) is the particle relaxation time defined as:

\[\tau_{p} = \frac{\rho_{p} d^{2}_{p}}{18 \mu}\]

For \(Re_{p} < 1\) and \(St_{k} < 1\), the hydrodynamic force on the particle can be represented as a point force. This force is calculated using the Stoke’s drag force formulation:

(3)\[\vec{F}_{h} = 3 \pi \mu d_{p} (U_{f} - U_{p})\]

The force obtained from (3) is applied on the particle and in the fluid side (in the cell where the particle resides), this hydrodynamic force is formulated as a body/volume force:

(4)\[\vec{f}_{h} = \frac{-\vec{F}_{h}}{V_{c} \rho_{f}}\]

where in equation (4) \(V_{c}\) is the volume of the cell and \(\rho_{f}\) is the fluid density. Hence the Navier-Stokes equations for the combined system is:

(5)\[\frac{\partial \vec{U}}{\partial t} + \nabla \cdot (\vec{U}\vec{U}) = -\frac{\nabla p}{\rho} + \nabla \bar{\bar \tau} + \vec{f}_{h}\]

Along with the continuity equation:

(6)\[\nabla \cdot \vec{U} = 0\]

Volume averaged coupling (pimpleFoamYade)

In the volume averaged coupling, the effect of the particle volume fraction is included. The Navier-Stokes equations take the following form:

(7)\[\frac{\partial (\epsilon_{f} \vec{U}_{f}) }{\partial t} + \nabla \cdot ( \epsilon_{f} \vec{U}_{f} \vec{U}_{f}) = -\frac{\nabla p}{\rho} + \epsilon_{f} \nabla \bar{\bar \tau} -K \left(U_{f}-U_{p} \right) + \vec{S}_{u} + \epsilon_{f} \vec{g}\]

Along with the continuity equation:

(8)\[\frac{\partial \epsilon_{f}}{\partial t} + \nabla \cdot (\epsilon_{f} \vec{U}_{f}) = 0\]

where in equations (7) and (8) \(\epsilon_{f}\) is the fluid volume fraction. Note that, we do not solve for \(\epsilon_{f}\) directly, but obtain it from the local particle volume fraction \(\epsilon_{s}\), \(\epsilon_{f} = 1 - \epsilon_{s}\) . \(K\) is the particle drag force parameter, \(\vec{U}_{f}\) and \(\vec{U}_{p}\) are the fluid and particle velocities respectively. \(\vec{S}_{u}\) denotes the explicit source term consisting the effect of other hydrodynamic forces such as the Archimedes/ambient force, added mass force etc. Details on the formulation of these forces are presented in the later parts of this section.

The interpolation and averaging of the Eulerean and Lagrangian quantities are based on a Gaussian envelope \(G_{\star}\). In this method, the the effect of the particle is ‘seen’ by the neighbouring cells of the cell in which it resides. Let \(\vec{x}_{c}\) and \(\vec{x}_{p}\) be the fluid cell center and particle position respectively, then the Gaussian filter \(G_{\star} \left(\vec{x}_{c}-\vec{x}_{p}\right)\) defined as:

(9)\[G_{\star} \left(\vec{x}_{c}-\vec{x}_{p}\right)=\left(2\pi\sigma^{2}\right)^{\frac{3}{2}}\exp\left(-\frac{\left|\left|\vec{x}_{c}-\vec{x}_{p}\right|\right|^{2}}{2\sigma^{2}}\right)\]

with \(\sigma\) being the standard deviation of the filter defined as:

(10)\[\sigma = \delta / \left(2\sqrt{2 \ln 2}\right)\]

where in equation (10) \(\delta\) is the cut-off range (at present it’s set to \(3 \Delta x\), with \(\Delta x\) being the fluid cell size.) and follows the rule:

\[G_{\star} \left(\left| \left| \vec{x}_{c} - \vec{x}_{p} \right| \right| = \delta/2 \right) = \frac{1}{2} G_{\star} \left( \left| \left| x_{c} -x_{p} \right| \right| = 0 \right)\]

The particle volume fraction \(\epsilon_{s,c}\) for a fluid cell \(c\) is calculated by:

(11)\[\epsilon_{s, c} = \frac{\sum_{i=1}^{N_{p}} V_{p,i} G_{\star (i,c)}}{V_{c}}\]

where in (11) \(N_{p}\) is the number of particle contributions on the cell \(c\), \(G_{\star (i,c)}\) is the Gaussian weight obtained from (9), \(V_{p,i}G_{\star (i,c)}\) forms the individual particle volume contribution. \(V_{c}\) is the fluid cell volume and \(\epsilon_{f}+\epsilon_{s}=1\)

The averaging and interpolation of an Eulerean quantity \(\phi\) from the grid (cells) to the particle position is performed using the following expression:

(12)\[\widetilde{\phi} = \sum_{i=1}^{N_{c}} \phi_{i} G_{\star (i,p)}\]

Hydrodynamic Force

In equation (7) the term \(K\) is the drag force parameter. In the present implementation, \(K\) is based on the Schiller Naumman drag law, which reads as:

(13)\[K = \frac{3}{4} C_{d} \frac{\rho_{f}}{d_{p}} \left| \left| \vec{\widetilde{U}}_{f} - \vec{U}_{p} \right| \right| \epsilon_{f}^{-h_{exp}}\]

In equation (13) \(\rho_{f}\) is the fluid density, \(d_{p}\) the particle diameter, \(h_{exp}\) is defined as the ‘hindrance coefficient’ with the value set as \(h_{exp}=2.65\). The drag force force coefficient \(C_{d}\) is valid for particle Reynolds numbers up to \(Re_{p} < 1000\). The expression for \(C_{d}\) reads as:

(14)\[C_{d} = \frac{24}{Re_{p}} \left(1+0.15Re^{0.687}_{p} \right)\]

The expression of hydrodynamic drag force on the particle is:

\[\vec{F}_{\textrm{drag}} = V_{p}K(\vec{\widetilde{U}}_{f} - {U}_{p})\]

In the fluid equations, negative of the drag parameter (\(-K\)) is distributed back to the grid based on equation (11). Since the drag force includes a non-linear dependency on the fluid velocity \(U_{f}\), this term is set as an implicit source term in the fluid solver.

The Archimedes/ambient force experienced by the particle is calculated as:

(15)\[\vec{F}_{by} = \left(\widetilde{-\nabla p} + \widetilde{\nabla \bar{\bar \tau}} \right) V_{p}\]

where in (15), \(\widetilde{\nabla p}\) is the averaged pressure gradient at the particle center and \(\widetilde{\nabla \bar{\bar \tau}}\) is the averaged divergence of the viscous stress at the particle position.

Added mass force:

(16)\[\vec{F}_{am} = C_{m}\left( \frac{D\widetilde{U_{f}}}{Dt} -\frac{dU_{p}}{dt} \right) V_{p}\]

where in eqaution (16), \(\frac{D\widetilde{U}_{f}}{Dt}\) is the material derivative of the fluid velocity.

Therefore the net hydrodynamic force on the particle reads as:

\[\vec{F}_{\textrm{hyd}} = \vec{F}_{\text{drag}} + \vec{F}_{\text{by}} + \vec{F}_{\text{am}}\]

And on the fluid side the explicit source term \(\vec{S}_{u, c}\) for a fluid cell \(c\) is expressed as :

\[\vec{S}_{u,c} = \frac{ \sum_{i=1}^{N_{p}} -\vec{F}_{\textrm{hyd,i}} \epsilon_{s,c} G_{\star (i,c)} } {\rho_{f} V_{c}}\]

Setting up a case

In Yade

Setting a case in the Yade side is fairly straight forward. The python script describing the scene in Yade is based on this method. Make sure the exact wall/periodic boundary conditions are set in Yade as well as in the OpenFOAM. The particles should not leave the fluid domain. In case a particle has ‘escaped’ the domain, a warning message would be printed/written to the log file and the simulation will break.

The example in examples/openfoam/ demonstrates the coupling. A symbolic link to Yade is created and it is imported in the script. The MPI environment is initialized by calling the initMPI() function before instantiating the coupling engine

fluidCoupling = FoamCoupling()

A list of the particle ids and number of particle is passed to the coupling engine

sphereIDs = [ for b in O.bodies if type(b.shape)==Sphere]
numparts = len(sphereIDs);

fluidCoupling.isGaussianInterp = False

The type of force/velocity interpolation mode has to be set. For Gaussian envelope interpolation, the isGaussianInterp flag has to be set, also the solver pimpleFoamYade must be used. The engine is added to the O.engines after the timestepper

O.engines = [
fluidCoupling ...
newton ]

Substepping/data exchange interval is set automatically based on the ratio of timesteps as foamDt/yadeDt (see exchangeDeltaT for details).


There are two solvers available in this git repository. The solver icoFoamYade is based on the point force coupling method and the solver pimpleFoamYade is based on the volume averaged coupling. They are based on the existing icoFoam and pimpleFoam solvers respectively. Any OpenFOAM supported mesh can be used, for more details on the mesh options and meshing see here. In the present example, the mesh is generated using blockMesh utility of OpenFOAM. The case is set up in the usual OpenFOAM way with the directories 0, system and constant

  U                         ## velocity boundary conditions
  p                         ## pressure boundary conditions
  uSource                   ## source term bcs (usually set as calculated).

  controlDict               ## simulation settings : start time, end time, delta T, solution write control etc.
  blockMeshDict             ## mesh setup for using blockMesh utility : define coordinates of geometry and surfaces. (used for simple geometries -> cartesian mesh.)
  decomposeParDict          ## dictionary for setting domain decomposition, (in the present example scotch is used)
  fvSchemes                 ## selection of finite volume schemes for calculations of divergence, gradients and interpolations.
  fvSolution                ## linear solver selection, setting of relaxation factors and tolerance criterion,

  polymesh/                 ## mesh information, generated by blockMesh or other mesh utils.
  transportProperties       ## set the fluid and particle properties. (just density of the particle)

Note: Always set the timestep less than the particle relaxation time scale, this is not claculated automatically yet! Turbulence modelling based on the RANS equations have not been implemented yet. However it is possible to use the present formulations for fully resolved turbulent flow simulations via DNS. Dynamic/moving mesh problems are not supported yet. (Let me know if you’re interested in implementing any new features.)

To prepare a simulation, follow these steps:

blockMesh         ## generate the mesh
decomposePar      ## decompose the mesh

Any type of mesh that is supported by OpenFOAM can be used. Dynamic mesh is currently not supported.


The simulation is executed via the following command:

mpiexec -n 1 python3 : -n NUMPROCS icoFoamYade -parallel

The video below shows the steps involved in compiling and executing the coupled CFD-DEM simulation


Paraview can be used to visulaize both the Yade solution (use VTKRecorder) and OpenFOAM solution. To visulaize the fluid solution, create an empty file as name.foam , open this file in Paraview and in the properties section below the pipeline, change “Reconstructed case” to “Decomposed case” , or you can use the reconstructed case itself but after running the reconstructPar utility, but this is time consuming.

Using blockMeshDict

The blockMeshDict file (system/blockMeshDict) can be loaded as facets (utils.facet) using the py/ module’s ymport.blockMeshDict function:

from yade import ymport

facets = ymport.blockMeshDict("system/blockMeshDict")


The version of the blockMeshDict must be 2.0, see: py/tests/ymport-files/blockMeshDict.

Only the “boundary” section will be loaded, that is faces \(f\) consists of vertices \(v\) in a way that one face is defined by four vertices:

(17)\[f_{i} = (v_{i0}, v_{i1}, v_{i2}, v_{i3}),\]

where vertex \(v\) is a point in a three dimensional space:

(18)\[v_{ij} = (x_{ij}, y_{ij}, z_{ij}).\]

Two new facets \(f^{*}\) are generated from every face \(f\):

(19)\[f_{0i}^{*} = (v_{i0}, v_{i1}, v_{i2}),\]
(20)\[f_{1i}^{*} = (v_{i2}, v_{i3}, v_{i0}).\]

There are three types of faces: patch, wall and empty. All types are loaded by default, the patch and empty types can be discarded using the patchasWall and emptyasWall arguments of ymport.blockMeshDict.

Using polyMesh

The polyMesh directory (constant/polyMesh) can be loaded as facets (utils.facet) using the py/ module’s ymport.polyMesh function:

from yade import ymport

facets = ymport.polyMesh("constant/polyMesh")


The function scans the directory and loads the points, faces and boundary files. The files must be FoamFiles` with the correct header (version is 2.0, type is ascii, see: py/tests/ymport-files/polyMesh/points). It parses the files and builds the boundary mesh:

The boundary mesh consists of faces \(f\) consists of vertices \(v\) in a way that one face is defined by four vertices:

\[f_{i} = (v_{i0}, v_{i1}, v_{i2}, v_{i3}),\]

where vertex \(v\) is a point in a three dimensional space:

\[v_{ij} = (x_{ij}, y_{ij}, z_{ij}).\]

Two new facets \(f^{*}\) are generated from every face \(f\):

\[f_{0i}^{*} = (v_{i0}, v_{i1}, v_{i2}),\]
\[f_{1i}^{*} = (v_{i2}, v_{i3}, v_{i0}).\]

There are three types of faces: patch, wall and empty. All types are loaded by default, the patch and empty types can be discarded using the patchAsWall and emptyAsWall arguments of ymport.polyMesh.

Note: The polyMesh is typically more refined than blockMeshDict.