Solver: MPPICInterFoam Description
mppicInterFoam is a solver designed to handle transient simulations of two incompressible, isothermal and immiscible fluids with a dispersed particle phase interacting with the fluid phases. The solver is a combination of [.external-solver]#interFoam and [.external-solver]#MPPICFoam solvers.
The solver employs a Volume of Fluid (VOF) approach for phase-fraction-based interface capturing, which is essential for tracking the interface between the two fluids.
In addition to the fluid dynamics, the soler incorporates a multiphase particle-in-cell (MPPIC) model. This model accounts for the interaction between a dispersed particle phase and the fluid phases, making it suitable for flows where solid particles are suspended in a liquid or gas. The solver includes a mixture model approach, solving a single momentum equation that represents the combined effects of both fluids.
The behavior of the dispersed phase in this solver is governed by a Liouville equation applied to the particle distribution function, which encapsulates particle characteristics such as position, velocity, and mass. To improve computational efficiency, particles are aggregated into parcels, significantly reducing the time required for calculations.
Unlike other solvers, such as DPMFoam, where particle collisions are handled explicitly, the solver models the collision force as a spatial gradient. This approach enables the use of a particle stress model to describe interactions, making it possible to simulate dense gas-solid flows near close-pack conditions with reduced computational demands, as explicit collision calculations are avoided.
To advance the solution in time, the solver employs the PIMPLE algorithm, applying under-relaxation techniques to enhance convergence stability throughout the iterative process. Furthermore, the solver can include optional features like Moving Reference Frame (MRF) to simulate rotating systems and handle turbulence modeling, allowing for laminar, Reynolds-Averaged Simulation (RAS), or Large Eddy Simulation (LES) as needed.
The solver finds the application in gas-liquid-solid three-phase flows (GLSTPF) which are common in chemical engineering (flotation buble column reactors), environmental engineering (wastewater treatment) or biochemical engineering (three-phase fluidized bed).
Solver: MPPICInterFoam Features
- Transient
- Incompressible
- Multiphase - Volume of Fluid (VoF)
- Multiphase - Lagrangian Particles
- Fluid and Particles
- Lagrangian Particles:
- Dense Cloud/Particle Bed
- MP-PIC method
- Laminar and Turbulent (RANS, LES - limited set)
- Newtonian and Non-Newtonian Fluid
- Pressure-Based Solver
- Rotating Objects:
- Multiple Reference Frames (MRF)
- Passive Scalar
- Porosity Modeling
- Buoyancy
- Source Term (explicit/implicit)
- Erosion
- PIMPLE Algorithm
- Solution Limiters:
- Velocity Damping
Solver: MPPICInterFoam Application
Industrial Chemistry
- Flotation Bubble Column Reactors
Biochemical Industry
- Three-Phase Fluidized Bed
Environmental Engineering
- Wastewater Treatment
Solver: MPPICInterFoam Multiphase - Dispersed Solvers
Dispersed Solvers In this group, we have included solvers implementing the Eulerian or Lagrangian approach to handle multiple fluids and particle clouds considering Dispersed Phases or Fluid-Particle interactions.
Dispersed - Euler
- multiphaseEulerFoam multiple miscible fluids, Euler-Euler approach
Dispersed - Lagrangian
- DPMFoam 1 fluid and particles, particle-particle interactions resolved explicitly (direct approach)
- MPPICFoam 1 fluid and particles, dense particle cloud using particle-particle interactions model (simplified approach, MP-PIC method)
- MPPICInterFoam 2 immiscible fluids and particles, dense particle cloud using particle-particle interactions model (simplified approach, MP-PIC method)
- DPMDyMFoam extension of DPMFoam with DyM
- MPPICDyMFoam extension of MPPICFoam with DyM
Dispersed - Drift-Flux
- driftFluxFoam 1 fluid and slurry or plastic dispersed phase, drift flux approximation for relative phase motion
- DPM - Discrete Phase Model
- MP-PIC - multiphase particle-in-cell method
- DyM - Dynamic Mesh
- MPPICFoam incompressible, solid particle clouds, without reactions
- DPMFoam incompressible, solid particle clouds, without reactions
- multiphaseEulerFoam incompressible, multiple miscible fluids, Euler-Euler approach
- interFoam base version of
MPPICInterFoam, 2 immiscible fluids
Solver: MPPICInterFoam Results Fields
This solver provides the following results fields:
- Primary Results Fields - quantities produced by the solver as default outputs
- Derivative Results - quantities that can be computed based on primary results and supplementary models. They are not initially produced by the solver as default outputs.
Primary Results Fields
Velocity | \(U\) [\(\frac{m}{s}\)] |
Kinematic Pressure \(p/\rho\) | \(p\) [\(\frac{m^{2}}{s^{2}}\)] |
Phase Volume Fraction | \(\alpha\) [\(-\)] |
Kinematic Pressure It is a pressure normalized by density. To obtain pressure in Pascals [Pa], multiply kinematic pressure by the fluid’s reference density. Read More: Kinematic Fluid Properties
Derivative Results
Pressure | \(P\) [\(Pa\)] |
Density | \(\rho\) [\(\frac{kg}{m^{3}}\)] |
Vorticity | \(\omega\) [\(\frac{1}{s}\)] |
Courant Number | \(Co\) [\(-\)] |
Peclet Number | \(Pe\) [\(-\)] |
Stream Function | \(\psi\) [\(\frac{m^2}{s}\)] |
Q Criterion | \(Q\) [\(-\)] |
Wall Functions (for RANS/LES turbulence) | \(y^+\) [\(-\)] |
Wall Shear Stress | \(WSS\) [\(Pa\)] |
Turbulent Fields (for RANS/LES turbulence) | \(k\) \(\epsilon\) \(\omega\) \(R\) \(L\) \(I\) \(\nu_t\) \(\alpha_t\) |
Volumetric Stream | \(\phi\) [\(\frac{m^{3}}{s}\)] |
Passive Scalar | \(scalar_i\) [\(-\)] |
Forces and Torque acting on the Boundary | \(F\) [\(N\)] \(M\) [\(-\)] |
Force Coefficients | \(C_l\) [\(-\)] \(C_d\) [\(-\)] \(C_m\) [\(-\)] |
Average, Minimum or Maximum in Volume from any Result Field | \(Avg\) \(Min\) \(Max\) |