Modeling Multiple Flow Regimes

The Multiple Flow Regime Phase Interaction model is used for cases where both segregated and dispersed two-phase flows exist in the same domain. An example scenario is a flow of a liquid and gas under undulating motion.

In the example flow of liquid and gas, it is possible to have three concurrent regions of two-phase flow:

First dispersed regime—a region where the gas is dispersed in the liquid.
Intermediate regime—a region where, of the two phases, neither phase is dispersed in the other phase. Instead, the interface between the two phases can be modeled as either separated or blended.
Second dispersed regime—a region where the liquid is dispersed in the gas.

When there is no clear separation between the two phases in the intermediate regime, by default, a blended interface drag method, a standard blending weight function, and a TVD scheme for volume fraction convection are used to model the mixed flow in this regime. If separated flow is anticipated (two phases are clearly separated by a sharp interface), the intermediate regime can account for the Large Scale Interface (LSI). This is achieved through a combination of the Large Scale Interface Detection phase interaction model, the Strubelj-Tiselj drag method, the Gradient Corrected Standard weight function, and the Adaptive Interface Sharpening (ADIS) volume-fraction convection scheme.

The steps in this procedure are intended to follow on from Step 4 in Modeling Eulerian Multiphase Flow.

To model multiple flow regimes:

Create two Eulerian phases, typically one gas phase and one liquid phase. For each phase:

Right-click the Multiphase > Eulerian Phases node and select New.
Right-click [phase] > Models and click Select Models.

In the Phase Model Selection dialog, select the following models:


Group Box	Model
Material	Select one of the following: Gas Liquid Multi-Component Gas Multi-Component Liquid
Reaction Regime	Select one of the following: Non-reacting Reacting
Equation of State	Any See General Equation of State Models.
Reynolds Averaged Turbulence	Select one of the following: K-Epsilon K-Omega Reynolds Stress See Modeling Turbulence.
Energy	Select one of the following: Segregated Fluid Enthalpy Segregated Fluid Temperature
Optional Models	Select any number of the following: Passive Scalar Used for tracking the phase material within the simulation. See Modeling Passive Scalars. Particle Size Distribution Use to predict the size distribution of droplets and bubbles due to breakup and coalescence. Select the S-Gamma model. See Modeling S-Gamma Particle Size Distribution

Define the phase interaction between the primary phase and the secondary phase. When you create a multiple flow regime phase interaction, you select the primary phase first, and then the secondary phase. When you select the secondary phase, you also choose the phase interaction type.

Right-click the Models > Multiphase Interaction > Phase Interactions node and select New > [Primary Phase] > [Secondary Phase] (Multiple Flow Regime).
Right-click the [phase interaction] > Models node and select Select Models.

In the Phase Interaction Model Selection dialog, activate the following models:


Group Box	Model
Enabled Models	Drag Force (selected automatically) See Drag Force Model Reference. Interaction Length Scale (selected automatically) See Interaction Length Scale Model Reference. Interaction Area Density (selected automatically) See Interaction Area Density Model Reference. Multiphase Material (selected automatically)
Optional Models	Select any of the following: Interphase Energy Transfer Models energy transfer between the phases. See Interphase Energy Transfer Model Reference. Interphase Mass Transfer Models mass transfer between the phases, such as boiling, evaporation, and condensation. The Boiling/Condensation model is selected automatically. See Modeling Boiling. Large Scale Interface Detection Allows the detection of large interface cells within the multiple flow regime topology. This model enables the use Adaptive Interface Sharpening (ADIS) and HRIC schemes for volume fraction convection. See Large Scale Interface Detection Model Reference. Large Scale Interface Distance Available when the Large Scale Interface Detection model is selected. Large Scale Interface Turbulence Damping See Large Scale Interface Turbulence Damping Model Reference. Surface Tension Force See Surface Tension Force Model Reference. Turbulent Dispersion Force Models the interaction between the dispersed phase and the surrounding turbulent eddies. See Turbulent Dispersion Force Model Reference. Virtual Mass Force Accounts for resistance effects when the dispersed phase density is similar or smaller than the continuous phase density. See Virtual Mass Force Model Reference. Lift Force Models the effect of the lift force on the dispersed phase. See Lift Force Model Reference. Wall Lubrication Force Models the effect of walls on bubbly flow. See Wall Lubrication Force Model Reference.

Values such as drag and heat transfer are calculated with a weighted sum of the interaction of each flow topology regime. You specify the blending function that is used in the transition between flow regimes.

Select the Multiple Flow Regime Topology > Flow Regime Weight Function node and set the appropriate method:

Option	Description
Standard	The default method. The weight function for each flow topology regime is calculated as described in Standard Blending Function.
Gradient Corrected Standard	A gradient based modification that leads to a smoother field of blending weight function. The weight function for each flow topology regime is calculated as described in Gradient Based Blending Function.
User Specified	You specify the first dispersed regime and second dispersed regime blending weight functions using field functions.

See Flow Regime Weight Function Properties.

Edit the [phase interaction] > Models node and set the following properties:


Node	Property	Setting
Interaction Length Scale	First Dispersed Regime Interaction Length Scale Second Dispersed Regime Interaction Length Scale	The mean bubble or droplet size in the respective regimes. See Interaction Length Scale Properties.
Interaction Area Density	First Dispersed Regime Interaction Area Density Second Dispersed Regime Interaction Area Density	The interfacial area available for drag, heat, and mass transfer between the two phases in the respective regimes. See Interaction Area Density Properties.
Drag Force	First Dispersed Regime Drag Coefficient Intermediate Regime Drag Coefficient Second Dispersed Regime Drag Coefficient	If the two phases are to be modeled as separated in the intermediate regime, use the Strubelj and Tiselj interface drag method. You also set the appropriate relaxation time factor for this interface drag method. If there is no clear separation of the two phases in the intermediate regime, use the Blended interface drag method. See Drag Coefficient Reference.
Interphase Energy Transfer	First Dispersed Regime Nusselt Number Intermediate Regime Nusselt Number Second Dispersed Regime Nusselt Number	See Nusselt Number Properties.

If a clear separation of the two phases in the intermediate regime is modeled (that is, the Blended interface drag method is not selected) set the following properties:


Node	Property	Setting
Large Scale Interface Detection	Primary Criteria of Interface Detection Secondary Criteria of Interface Detection Number of Cell Layers for Interface Band	See Large Scale Interface Detection.
Large Scale Interface Turbulence Damping	Primary Phase Turbulence Damping Secondary Phase Turbulence Damping	For a phase that has the K-Omega turbulence model activated, you also choose the turbulence damping method and the interface distance specification. See Primary and Secondary Phase Turbulence Damping Properties.

If you are using the Large Scale Interface Detection model you can use Implicit Multi-Stepping for the Volume Fraction solver to reduce the run-time of your simulation without affecting quality. The implicit multi-stepping feature alleviates the CFL restriction near the interface by sub-stepping the volume fraction transport equation with a reduced time-step. This allows you to increase the global time-step to reduce computational costs.

If you want to activate the implicit multi-step solver, select the Solvers > Volume Fraction node and set Number of Steps to greater than 1.
When the specified fixed number of implicit sub-steps is set to more than 1, the Volume Fraction solver performs multiple steps per time-step. See Volume Fraction Solver.
Note Implicit multi-stepping is not compatible with the LSI Smoothed CFL time-step provider.

In a Multiple Flow Regimes simulation, you are advised to use high order convection for the volume fraction and the flow. This setting reduces numerical diffusion and helps to obtain a reasonably sharp interface. If you are modeling a mixed intermediate regime, the second-order scheme for volume fraction convection is recommended. For modeling the Large Scale Interface (LSI), the Adaptive Interface Sharpening (ADIS) scheme for volume fraction convection is recommend. Additionally, to improve the simulation's robustness, setting the minimum volume fraction to a value of 1.0E-12 could assist.

Return to Modeling Eulerian Multiphase Flow and continue with Step 5.