Mixture Model
Use the Mixture Model () multiphysics coupling to simulate the flow of liquids containing one or more dispersed phases. The dispersed phases can be bubbles, liquid droplets, or solid particles, which are assumed to travel always with their terminal velocity.
The Phase Transport and the single-phase flow interface, which are coupled by the Mixture Model multiphysics coupling, solve together for conservation of mass of the dispersed phases and conservation of total mass and momentum of the mixture.
The Mixture Model multiphysics coupling provides the mixture density and viscosity to the single-phase fluid flow interface. Since the density of the mixture depends on the volume fractions and densities of the different phases, which in turn may depend on pressure and temperature, it cannot be assumed that the density of the mixture is constant. Therefore the Incompressible flow option is not available in the single-phase flow interface that is coupled by the Mixture Model multiphysics coupling.
In the Phase Transport interface, it sets the Absolute pressure in the Model Input section and defines the densities in the Density section of the Fluid feature. In addition it determines and provides the velocity fields for the dispersed phases in the Velocity Field section.
Settings
The Label is the default multiphysics coupling feature name.
The Name is used primarily as a scope prefix for variables defined by the coupling node. Refer to such variables in expressions using the pattern <name>.<variable_name>. In order to distinguish between variables belonging to different coupling nodes or physics interfaces, the name string must be unique. Only letters, numbers, and underscores (_) are permitted in the Name field. The first character must be a letter.
The default Name (for the first multiphysics coupling feature in the model) is mfmm1.
Domain Selection
When nodes are added from the context menu, you can select Manual (the default) from the Selection list to choose specific domains to define the mixture model, or select All domains as needed.
Coupled Interfaces
This section defines the physics involved in the multiphysics coupling. The Phase transport and Fluid flow lists include all applicable physics interfaces.
The default values depend on how this coupling node is created.
•
If it is added from the Physics ribbon (Windows users), Physics contextual toolbar (Mac and Linux users), or context menu (all users), then the first physics interface of each type in the component is selected as the default.
•
If it is added automatically when a multiphysics interface is chosen in the Model Wizard or Add Physics window, then the two participating physics interfaces are selected.
You can also select None from either list to uncouple the node from a physics interface. If the physics interface is removed from the Model Builder, for example Phase Transport is deleted, then the Phase transport list defaults to None as there is nothing to couple to.
Model Inputs
The viscosity and density of each phase can be defined through user inputs, variables, or by selecting a material. For the latter option, additional inputs, for example temperature or pressure, may be required to define these properties.
Temperature
By default, the Temperature model input is set to User defined. Alternatively, the temperature field can be selected from another physics interface. All physics interfaces have their own tags (Name). For example, if a Heat Transfer in Fluids interface is included in the component, the Temperature (ht) option is available for T.
Absolute Pressure
This input appears when a material requires the absolute pressure as a model input. The absolute pressure is used to evaluate material properties, but it also relates to the value of the calculated pressure field. There are generally two ways to calculate the pressure when describing fluid flow: either to solve for the absolute pressure or for a pressure (often denoted gauge pressure) that relates to the absolute pressure through a reference pressure.
The default Absolute pressure pA is p+pref, where p is the dependent pressure variable from the Navier–Stokes or RANS equations, and pref is from the user input defined at the physics interface level. When pref is nonzero, the physics interface solves for a gauge pressure. If the pressure field instead is an absolute pressure field, pref should be set to 0.
Whenever the Compressibility in the coupled Fluid flow interface is set to Weakly compressible flow, the material properties are evaluated using the reference pressure level, pref, supplied in the coupled Fluid flow interface.
The Absolute pressure field can be edited by clicking Make All Model Inputs Editable () and entering the desired value in the input field.
Model Inputs and Multiphysics Couplings in the COMSOL Multiphysics Reference Manual
Physical Model
Specify the characteristics of the dispersed phase(s), the model for the slip velocity, and the mixture viscosity model.
Dispersed Phase
To characterize the Dispersed phase, select Solid particles (the default) or Liquid droplets/bubbles.
Slip Model
To compute the slip velocity uslip,i (SI unit: m/s), select a Slip model — Homogeneous flow (the default), Hadamard-Rybczynski, Schiller-Naumann, Haider-Levenspiel, or User defined.
•
The Homogeneous flow model assumes that the velocities of the continuous and dispersed phases are equal, that is, uslip,i = 0.
•
In most cases there is a significant difference in the velocity fields due to the buoyancy of the dispersed phase. Use one of the predefined slip models for such cases.
•
For User defined specify an arbitrary expression for the relative velocity. For example, give a constant velocity based on experimental data. Enter the Slip velocity field uslip,i (SI unit: m/s) in the Dispersed phase properties sections.
Mixture Viscosity Model
Select the Mixture viscosity model.
•
When Solid particles is the Dispersed phase, select either Krieger type (the default) or User defined.
•
When Liquid droplets/bubbles is the Dispersed phase, select Krieger type (the default), Volume averaged, or User defined.
For User defined enter a value or expression for the Dynamic viscosity, mixture μ (SI unit: Pa⋅s). The default expression is mfmm1.muc, which is the variable name for the viscosity of the continuous phase. When using this option to enter an expression, make sure to limit the viscosity to bounded positive values.
When Krieger type is selected, enter a value or expression for the Maximum packing concentration ϕmax (dimensionless). The default is 0.62.
Select Krieger type to model the most generally valid expression for the mixture viscosity:
where ϕmax is the maximum packing concentration, which for solid particles is approximately 0.62. The dimensionless parameter μ* = 1 for solid particles and
for droplets and bubbles. When applying the Krieger type viscosity model, ϕd is replaced by min(ϕd, 0.999ϕmax) for better robustness.
When there is more than one dispersed phase, the Krieger type viscosity model uses a more involved expression which is described in detail in the section Theory for the Phase Transport Mixture Model Interfaces
Select Volume averaged to model the mixture viscosity of liquid-liquid mixtures, which uses the following equation for the viscosity:
The Mixture Model interfaces always employ the mixture viscosity in the particle Reynolds number expression used to calculate the slip velocity, thereby accounting for the increase in viscous drag due to particle-particle interactions.
Include Diffusion Stress in Momentum Equation
When the Include diffusion stress in momentum equation checkbox is selected (default), the diffusion stress term is added to the momentum equation in the coupled fluid flow interface. Deselect the checkbox to disregard this term.
Low Dispersed Phase Concentration
When the Low dispersed phase concentration checkbox is selected, the mixture density in the continuity equation and in the inertial terms of the momentum equation is replaced by the density of the continuous phase (see Equation 6-138 and Equation 6-139 in the section Theory for the Phase Transport Mixture Model Interfaces). This approximation is valid if the volume fraction of the dispersed phases is small (less than a few percent) and if the density of the dispersed phases is not (much) larger than the density of the continuous phase.
Include Shear-Induced Migration
When the Include shear-induced migration checkbox is selected, shear-rate dependent diffusion and migration terms are added to the conservation equations for the volume fractions of the dispersed phases. Enter values for the parameters Kc and λ (the default values are 0.4 and 1.59, respectively).
Turbulence
This section is available whenever the coupled fluid flow interface is a turbulent flow interface using a RANS turbulence model.
Enter a value or expression for the Turbulent Schmidt number ScT. The default value is 0.35 (dimensionless).
See the section About Turbulent Mixing in the CFD Module User’s Guide (this link is available online or if you have the CFD Module documentation installed).
Whenever the coupled fluid flow interface is a turbulent flow interface using the k-ε, k-ω, SST, Low Re k-ε or Realizable k-ε turbulence model, and the Dispersed phase is set to Liquid droplets/bubbles, this section also contains an Include bubble-induced turbulence checkbox. When this checkbox is selected, bubble induced turbulence production terms are added to the turbulence model. In addition, the turbulence model parameters for these terms can be edited.
Continuous Phase Properties
Select the fluid materials to use for the material properties. The default material used for the Continuous phase is the Domain material.
The default Density, continuous phase ρc (SI unit: kg/m3) uses values From material (as selected in the Materials section). For User defined enter another value or expression. In this case the default is 1000 kg/m3.
The density in a material can depend on temperature and/or pressure and these dependencies are automatically replaced by pref and Tref, which are specified in the Model Input section.
The default Dynamic viscosity, continuous phase μc (SI unit: Pa·s), uses values From material. It describes the relationship between the shear stresses and the shear rate in a fluid. Intuitively, water and air have a low viscosity, and substances often described as thick, such as oil, have a higher viscosity. For User defined enter another value or expression. In this case, the default is 0.001 Pa·s.
Dispersed Phase Properties
The number of Dispersed Phase Properties sections depends on the number of phases defined in the coupled Phase Transport interface: the number of sections is equal to the number of dispersed phases, which is in turn equal to the number of phases defined in the coupled Phase Transport interface minus one.
The options in these sections are influenced by the selections made in the Physical Model section.
Select the fluid materials to use for the material properties. The default material used for the Phase is the Domain material.
The default Density, dispersed phase ρi (SI unit: kg/m3) uses values From material (as selected in the Materials section). For User defined enter another value or expression. In this case, the default is 1000 kg/m3.
The density in a material can depend on temperature and/or pressure and these dependencies are automatically replaced by pref and Tref, which are specified in the Model Input section.
If Liquid droplets/bubbles is selected from the Dispersed phase list in the Physical Model section, then Dynamic viscosity, dispersed phase μi (SI unit: Pa·s) is also available. The default uses values From material or select User defined to enter another value or expression. In this case, the default is 0.001 Pa·s.
If one of the predefined slip models (Hadamard-Rybczynski, Schiller-Naumann, or Haider-Levenspiel) is selected from the Slip model list in the Physical Model section, then Diameter of particles/droplets di (SI unit: m) is also available. The default is 10−3 m (1 mm). If Haider-Levenspiel is selected for the Slip model under Physical Model, enter a value between 0 and 1 for the Sphericity (dimensionless). The default is 1.
If a Schiller-Naumann or a Haider-Levenspiel slip model is selected from the Slip model list in the Physical Model section, enter an initial value for the Squared slip velocity slipvel0,i (SI unit: m2/s2). The default is 0 m2/s2.
When a User defined Slip model is selected in the Physical Model section, specify an arbitrary expression for the slip velocity uslip,i (SI unit: m/s). For example, give a constant velocity based on experimental data.
•
See Theory for the Phase Transport Mixture Model Interfaces
If a physics interface is deleted and then added to the model again, then in order to reestablish the coupling, you need to choose the physics interface again from the Phase transport or Fluid flow lists. This is applicable to all multiphysics coupling nodes that would normally default to the once present interface. See Multiphysics Modeling Workflow in the COMSOL Multiphysics Reference Manual.