Which Multiphase Flow Interface Should I Use?
Fabrice Schlegel January 27, 2015
If you are interested in using COMSOL Multiphysics software to solve multiphase flow problems, you may be wondering which multiphase flow interface to choose. This is your guide to the six interface options available to you and when you should use them.
Overview of Applications and Multiphase Flow Interfaces
The COMSOL Multiphysics software’s multiphase flow capabilities cover a wide range of applications, including:
- Bubbly flow
- Discrete gaseous bubbles in a continuous liquid
- Droplet flow
- Discrete fluid droplets in another fluid
- Particle-laden flow
- Discrete solid particles in a fluid
- Free-surface flow
- Immiscible fluids separated by a clearly defined interface
- Fluidized beds
- Vertical cylinder containing particles where gas is introduced through a distributor
These application areas are covered by six different physics interfaces, and it is not always trivial to determine which physics interface is better suited to solve your particular application.
Screenshot of the model tree displaying the six interfaces.
In this blog post, we describe these six multiphase flow physics interfaces to make it easier for you to choose. Very specific application areas, such as two-phase flow in porous media or cavitation problems, will be the object of future blog entries.
Interface Tracking vs. Disperse Methods
The six multiphase flow models can be split into two main categories, which we will refer to as the interface tracking methods and the disperse methods.
The interface tracking methods model the flow of two different immiscible fluids separated by a clearly defined interface. These methods are typically used to model bubble or droplet formation, sloshing tanks, or separated oil/water/gas flow. In the below example by the Philips® FluidFocus team, the meniscus between two immiscible liquids is used as an optical lens.
Image credit: Philips.
The shape of the meniscus in this device is controlled by changing the voltage applied to the conducting liquid, thus changing the focal point of the lens. The lens is then integrated within a miniature variable-focus camera. Because the exact location of the interface is of interest here, the FluidFocus team used an interface tracking method in their numerical model.
A tutorial showing how to reproduce this model can be found in our Model Gallery.
While the interface tracking methods are accurate and provide a clear picture of the flow field (velocity, pressure, and surface tension force), they are not always practical due to their high computational cost. Thus, the interface tracking methods are generally better suited to microfluidics problems in which only a few droplets or a few bubbles are tracked.
Larger-scale simulations involving a greater number of bubbles, droplets, or solid particles require computationally cheaper methods. Cue: the disperse methods.
This second category of methods does not explicitly track the position of the interface between the two fluids, but instead tracks the volume fraction of each phase, thus lowering the computational load. A circulated fluidized bed, which is a very common apparatus in the food, pharmaceutical, and chemical processing industries, can be modeled using a disperse method.
In this example, the dispersed phase, consisting of solid spherical particles, is fluidized by air and transported upwards through a vertical riser:
Tracking every single solid particle would not be computationally practical here. Instead, we compute the volume fraction of solid particles. The disperse methods are typically used to model particle-laden flow, bubbly flow, and mixtures.
In the next few sections of this blog post, I will discuss and compare the different tracking and homogeneous methods.
The disperse methods include the following:
- Euler-Euler model
- Bubbly flow model
- Mixture model
The Euler-Euler model simulates the flow of two continuous and fully interpenetrating incompressible phases. Typical applications are fluidized beds (solid particles in gas), sedimentation (solid particles in liquid), or transport of liquid droplets or bubbles in a liquid.
This model requires the resolution of two sets of Navier-Stokes equations, one for each phase, in order to calculate the velocity field for each phase. The volume fraction of the dispersed phase is tracked with an additional transport equation.
The Euler-Euler model is the correct two-phase flow method to model the fluidized bed that I presented earlier. The model relies on the assumption that the dispersed particles, bubbles, or droplets are much smaller than the grid size.
The Euler-Euler model is the most versatile of the three disperse models, but it comes at a high computational cost. The model solves for two sets of the Navier-Stokes equations, instead of one, which is the case for all other models presented here. Both the bubbly flow and mixture models are simplifications of the Euler-Euler model and rely on additional assumptions.
Bubbly Flow Model
The bubbly flow model is used to predict the flow of liquids with dispersed bubbles. It relies on the following assumptions:
- The dispersed bubbles are much smaller than the grid size
- The gas density is negligible compared to the liquid density
- The gas volume fraction does not exceed 10%
In this model of an airlift loop reactor, air bubbles are injected at the bottom of a reactor filled with water:
The bubbly model solves one set of Navier-Stokes equations for the flow momentum, a mixture-averaged continuity equation, and a transport equation for the gas phase. Although this model does not track individual bubbles, the distribution of the number density (i.e., the number of bubbles per unit volume) can still be recovered. This can be useful when simulating chemical reactions in the mixture.
The mixture model is used to simulate liquids or gases containing a dispersed phase. The dispersed phase can be bubbles, liquid droplets, or solid particles, which are assumed to always travel with their terminal velocity. While this model can be used for bubbles, it is recommended to use the bubbly flow model instead for gas bubbles in a liquid.
The mixture model solves one set of Navier-Stokes equations for the momentum of the mixture, a mixture-averaged continuity equation, and a transport equation for the volume fraction of the dispersed phase. Like the bubbly model, the mixture model can also recover the number of bubbles, droplets, or dispersed particles per unit volume.
The mixture model relies on the following assumptions:
- The density of each phase is constant
- The dispersed phase droplets or particles travel with their terminal velocity
This tutorial models the flow of a dense suspension consisting of light, solid particles in a liquid placed between two concentric cylinders.
Summary of the Disperse Models
I have summarized the disperse models for you in a table:
|Euler-Euler Model||Bubbly Flow Model||Mixture Model|
|Valid for these continuous phases:||
|Valid for these dispersed phases:||
|Equations solved for (laminar flow):||
|Available turbulence models:||
These three multiphase flow models require the CFD Module. The mixture model for rotating machinery problems also requires the Mixer Module. More details on the required COMSOL products can be found in our specification chart.
Interface Tracking Methods
The interface tracking methods include:
- Level set method
- Phase field method
- Two-phase flow moving mesh method
All these methods very accurately track the position of the interface between the two immiscible fluids. They account for differences in density and viscosity of the two fluids, as well as effects of surface tension and gravity.
The Level Set and the Phase Field Methods
With the level set and phase field methods, the interface is tracked using an auxiliary function, or color function, on a fixed mesh.
The Navier-Stokes equations and the continuity equation are solved for the conservation of momentum and mass, respectively. The color function, and therefore the interface position, is tracked by solving additional transport equations (one additional equation for the level set method and two additional transport equations for the phase field method). This color function varies between a low value (0 and -1 for the level set and phase field methods, respectively) in one phase and high value of 1 in the second phase.
The interface is diffuse and centered on the center value of these functions (0.5 and 0 for the level set and phase field methods, respectively). The material properties of both phases such as the density and viscosity are scaled according to the color function.
This plot shows the filling of a capillary channel using the level set or phase field method. The higher value of the color function (red region) shows the location of the fluid phase, while the lower value (blue region) represents the gas phase. The two phases are separated by a diffuse interface that is not aligned with the fixed mesh.
While the level set method solves for two phases, the phase field method can solve for up to three phases. Unlike the Level Set interface, the Phase Field interface also allows for fluid-structure interaction and phase separation models.
The phase field method, which is physically motivated, is formulated such that the mixing energy (the sum of the surface energy and bulk energy of the flow) is minimized. It includes more physics than the level set method and is more accurate as long as the interface is properly resolved by the mesh. On the other hand, it is computationally more expensive, adding two additional transport equations versus one transport equation for the level set method. The phase field method is recommended for microfluidic simulations where the surface shape is of primary importance.
While the phase field method is based on physical considerations, the level set method has been developed from a mathematical standpoint and corresponds to a color function that is convected by the fluid flow. The level set method includes less physics and is thus slightly more robust from a numerical point of view. Unlike the phase field method, the level set method includes stabilization for the level set variable. Therefore, it is recommended for larger scale simulations where the interface is not well resolved by the mesh and where the mean position of the interface is sought rather than the fine details.
Moving Mesh Method
Unlike the level set and phase field methods, which are solved on a fixed mesh, the two-phase flow moving mesh method tracks the interface position with a moving mesh using the ALE method.
Here, the same capillary filling simulation is implemented using the moving mesh method. This time, the interface is sharp and it follows the boundary between the fluid and the gas domain. Because the position of the interface is given by the boundary between the two meshes, it does not require any additional transport equations. Only one set of Navier-Stokes equations is solved on each mesh.
Since physical interfaces are usually much thinner than practical mesh resolutions, the two-phase flow moving mesh technique offers the most accurate representation of the interface. This method also accounts for mass transport across the interface, which is very difficult to implement using the two other interface tracking methods. Finally, the sharp interface also means that different physics can be solved in the domains on either side of the interface.
The main drawback of the moving mesh methods is the fact that the mesh must deform continuously, which means that problems involving topological changes cannot be solved. This drastically limits its applications. Problems such as droplet breakup or the transition from jetting to dripping of a liquid jet cannot be modeled using the moving mesh method and require the level set or phase field method. This jet instability simulation shows the break-up of a jet into droplets over time using the level set method.
Liquid regions (shown in black).
Comparison of the Interface Tracking Methods
As with the homogeneous models above, I have put the interfacing tracking methods in a table for an easy overview:
|Level Set||Phase Field||Moving Mesh|
Does not support topological changes
|Accurate representation of the interface:||Good||Better||Best|
|Equations solved for:||
|Available turbulence models:||
|Required COMSOL products for laminar flow:|
|Required COMSOL products for turbulent flow:|
In this blog post, we compared six different two-phase flow methods. The COMSOL Multiphysics simulation software does offer additional multiphase flow methods, including two-phase flow methods in porous media or cavitation in thin films, such as journal bearings. These topics will be the object of future blog entries.
If you have any multiphase flow modeling questions, feel free to contact our Technical Support team. If you are not yet a COMSOL Multiphysics user and would like to learn more about our software, please contact us via this form — we’d love to connect with you.
PHILIPS is a registered trademark of Koninklijke Philips N.V.
Editor’s note: This blog post was updated on 5/5/16.