Multi-phase Flow in OpenFOAM
Multi-phase flows has wide applications in process, automotive, power generation and metal industries including phenemona like mixing, particle-laden flows, CSTR - Contunuously Stirred Tanks Reactor, fluidized bed, fuel injection in engines, bubble columns, mixer vessels. Some of the general characteristics and categories of multi-phase flow are described below before moving to actual application of OpenFOAM utilities.
Multiphase flow regimes are typically grouped into five categories: gas-liquid (which are naturally immiscible) flows and (immiscible) liquid-liquid flows, gas-solid flows, liquid-solid flows, three or more phase flows. As can be seen, the immiscibility is a important criteria. In a multi-phase flow, one of the phase is usually continuous and the other phase(s) are dispersed in it. Gas-liquid flows are further grouped into many categories depending upon the distribution and shape of gas parcels. Three such types are described below.
Bubbly Flows: it resensts a flow of discrete gaseous or fluid bubbles in a continuous phase.
Slug Flows: This is characterized by flow of large gas bubbles in liquid.
Annular Flows: Here one of the phase if confined to area near the wall forming an annular section.
Some other types of flows are particle-laden flow such as air carrying dust particles, slurry flow where particles are transported in a liquid, hydrotransport which describes densely-distributed solid particles in a continuous liquid such as cement concrete mix. Gas assisted mixing of solid such as fluidized-bed and settling tank where particles tend to sediment near the bottom of the tank forming thick sludge are some other examples of multi-phase flows.
The two dominant method of multi-phase simulations are listed below.
This page summarizes the multi-phase cases supplied with OpenFOAM 1606+.
Some of the resource from the web are listed below. IPR: the ownership and copyright of these documents lie with the author mentioned in the document.
Excerpts from "LPT for erosion modeling in OpenFOAM: Differences between solidParticle and kinematicParcel, and how to add erosion modeling by Alejandro Lopez" - When dealing with the movement of a group of particles inside a fluid, there are basically two different ways to approach the problem. In the Eulerian-Eulerian models, the particles are treated as a continuous phase and conservation equations are solved for the particulate phase. This method is suitable for large particle concentrations, where two-way coupling between the fluid and the particulate phases as well as particle-particle collisions are important. On the other hand, in the Eulerian-Lagrangian approach, the Eulerian continuum equations are solved for the fluid phase, while Newton’s equations for motion are solved for the particulate phase in order to determine the trajectories of the particles (or groups of particles).
Thus, if both or all the phases are to be modelled as continuous phases, Eulerian approach is used. When a discrete phase (spatially not continuous) is to be modeled, a Lagrangian frame of reference is used in which spherical particles of pre-defined size distribution is dispersed in the continuous phase (the spherical particles may represent parcels of droplets or bubbles). The fluid phase is modeled as a continuum where time-averaged Navier-Stokes equations are solved to get flow field while the discrete phase is solved by tracking a large number of particles (parcels, bubbles, or droplets) through this calculated flow field. Thus, a Lagrangain approach includes and requires:
DPMFoam: Discrete Phase Model - This is another multi-phase solver which includes the effect of the discrete phase particulate volume fraction on the continuous phase. This utility is recommended for dense particle flow simulation. Though there is no strict and standard definition of 'dense' particle-laden flow, a volume fraction of 10% or higher is usually considered 'dense'. The solver uses existing functionality for particle clouds and their collisions, which directly resolves particle-particle interactions. Official description is "Transient solver for the coupled transport of a single kinematic particle cloud including the effect of the volume fraction of particles on the continuous phase.".
The term 'cloud' represents the overall presence of all particles, whether they're active or not. Since, this is a transient solver, it is based on PIMPLE algorithm. Turbulence models available in this utility are [a] laminar, [b] k-ε RANS and [c] LES as shown in the header file of the source code.
The object 'particleProperties' defined in dictionary file 'kinematicCloudProperties' is the additional information required for Lagrangian-Eulerian simulations. It defines particle injection rate, particle size and distribution, the forces acting of the particle and empirical model to be used. A sample of kinematicCloudProperties file with comments to describe each of the variable and its significance in the simulation can be find in the this file.
MPPICFoam (MultiPhase Particle-In-Cell method):This is a "Lagrangian solver" having LPT (Lagrangian Particle Tracking) capabilities and can be used for modelling particles in continuum. This method simulates solid phase as parcels and is used to represent collisions without resolving particle-particle interactions. This solver is identical to DPMFoam, but without the collisions between particles.. Quote from a post by Bruno Santos on cfd-online.com: |The solvers DPMFoam and MPPICFoam are virtually identical, except that the first one uses "basicKinematicCollidingCloud" as the base cloud type and the second one uses "basicKinematicMPPICCloud"|.
Phase-coupling mechanisms strongly influences the behavior of the continous and dispersed phase. There are 3 different types of couplings present in particle-laden fluid flows.
Lagangian >> MPPICFoam >> injectionChannel - The computational geometry and animation of particle tracks in a mixing phenomena of two streams of particle-laden gas is described below.
For particle tracking in ParaView, [a] either the utility particleTracks can be used or [b] convert the case to VTK format using foamToVTK utility. Copy the particleTrackProperties dictionary into the /constant directory and execute the utility: particleTracks. This will generate necessary files to visualize the particle trajectories in ParaView. The location of the file particleTrackProperties is:
Both the particleTracks and foamToVTK utility will create a folder named VTK in the case directory which will have futher sub-level folders. The folder VTK/lagrangian/kinematicCloud will contain a file kinematicCloud_TTT.vtk files where TTT is the time step. For particle tracking visualization, one needs to open this file. Then, use Glyph utility to visualize the tracks - with various Gyph type options [Sphere, arrow, cone, box...] available.
Lagangian >> simpleReactingParcelFoam >> verticalChannel : a steady state Lagrangian - Eulerian solver for chemical reaction, combustion and particle clouds.
Two-phase flows are often broadly categorised by the physical states of the constituent components and by the topology of the interfaces. Thus, a two-phase flow can be classified as gas-solid, gas-liquid, solid-liquid and liquid-liquid in the case of two immiscible liquids . Similarly, a flow can be broadly classfied topologically as separated, dispersed or transitional.
The following video is an attempt to model air entrainment using multiphase flow. In the left video, you may notice how spherical bubbles are formed due air entrained by water stream entering into the bottle. The interface of the air bubble and water is sharp. This feature is not as prominent in the simulation primarily due to corse mesh. Capturing a sharp interface between gas and liquid will require a very fine mesh. Some improvements planned are:
multiPhase >> interFoam >> ras >> angledDuct - Flow of water in an empty angled duct: immiscible two phase flow - there are 3 three implementation with LAMINAR, LES and RAS turbulence as tutorial cases. One of the tutorial with RAS implementation is shown below where water enters into the inlet and fills the duct as it moves towards the outlet.
This is an Eulerian-Eulerian solver for two (including compressible) fluid phases where one phase is continuous say water and the other phase is dispersed say gas bubbles or solid particles. It may or may not involve heat transfer. Fluidised bed simulations can be performed using this solver. Note that the flow of solids (the particle bed is bubbling) is being modeled here though it is gas assisted and not the granular flow of solid by its own weight.
For two phase flows involving fluids, the thermophysicalProperties are specified by adding suffix after the dictionary 'thermophysicalProperties' such as thermophysicalProperties.air, thermophysicalProperties.water. Special variables for this solver:
Three or more phases, interface capturing capabilities configured to work with LES and not RANS. Phases can be segregated or dispersed. As per source code: "Solver for a system of many compressible fluid phases including heat-transfer". The application to 2D geometry of a mixing vessel is shown below. This is based on Multiple Reference Frame (MRF) method for sliding interfaces - set by dictionary constant/MRFProperties.
The simulation of this categories require following 5 files in 'constant' folder -  chemistryProperties - required to include chemical reactions when 'chemistry' is switched on,  environmentalProperties - specify gravity,  combustionProperties - to activate combustion models such as PaSR / XiFoam,  thermophysicalProperties - to specify type of mixtures and its properties, gas phase reaction scheme, presence of inert species and  phaseProperties - this dictionary file is specific to this solver and is used to describe interaction between the phases.
A sample 'phaseProperties' dictionary file with comments as per tutorials, online literatures and information available in approppriate *.C and *H file can be acccessed here.
The content on CFDyna.com is being constantly refined and improvised with on-the-job experience, testing, and training. Examples might be simplified to improve insight into the physics and basic understanding. Linked pages, articles, references, and examples are constantly reviewed to reduce errors, but we cannot warrant full correctness of all content.