Eulerian Multiphase Model in ANSYS Fluent (Euler-Euler)

The Eulerian multiphase model in ANSYS Fluent is the standard method to simulate dense flows where two or more phases move together. Engineers also refer to this as the Euler-Euler model, because it treats every phase as its own continuous fluid. You will see it used for industrial equipment like bubble columns, fluidized beds, stirred tanks, and slurry lines.

This guide explains what the model does, when you should pick it instead of VOF, Mixture, or DPM, and how to define your phases correctly. If you want to practice setting up these physics with real project files, you can start with our Multiphase CFD Simulation tutorials.

Introduction to Multiphase Flows

Multiphase flow occurs when two or more states of matter move together in the same physical space. You can divide these flows into four main categories based on the interacting materials:

• Gas-Liquid Flows: Air bubbles rising in water, or liquid droplets sprayed into a gas stream.
• Gas-Solid Flows: Solid particles carried by air, such as sandstorms or pneumatic conveying.
• Liquid-Solid Flows: Solid particles suspended in a liquid, like mud or chemical slurries.
• Three-Phase Flows: A mix of gas, liquid, and solid, such as gas bubbles rising through a liquid-solid slurry.

Engineers simulate these interactions to design industrial equipment like bubble columns, fluidized beds, stirred tanks, and cyclone separators. Setting up an accurate CFD simulation is the only way to predict how these phases mix and separate before building the actual hardware.

 

 

Figure 1: Real-world applications of the Eulerian multiphase model in ANSYS Fluent, including particle mixing and fluidized beds.

What is the Eulerian Model?

When setting up a multiphase flow simulation, you should define how the software handles the secondary phases (like bubbles or sand) moving through the primary continuous phase (like water or air). ANSYS Fluent offers two main mathematical approaches: the Euler-Lagrangian method and the Euler-Euler method.

• The Euler-Lagrangian Method (DPM): The software solves the main fluid as a continuous space, but explicitly tracks the exact physical path of every single particle. Fluent calls this the Discrete Phase Model (DPM). You use this for dilute flows with a low particle count, which you can see in action in our DPM CFD Simulation tutorials. However, if your system contains millions of particles, tracking them individually becomes computationally impossible.
• The Euler-Euler Method: This is the foundation of the Eulerian multiphase model. Instead of tracking single particles, it calculates the flow by treating both the continuous phase and the dispersed phase as interpenetrating continua.

What does “interpenetrating continua” actually mean? It means the software assumes multiple phases can occupy the same computational cell at the same time. It calculates a volume fraction for each phase and treats them as separate, continuous fluids. Because it skips individual particle tracking, the Eulerian model in ANSYS Fluent easily handles extremely dense flows, regardless of how many millions of bubbles exist in the domain.

 

 Figure 2: Comparing the discrete Euler-Lagrangian particle tracking method with the Euler-Euler multiphase model approach in ANSYS Fluent.

When to Choose the Eulerian Model vs. Other Models

ANSYS Fluent provides several multiphase frameworks. Before committing to the high computational cost of the Euler-Euler approach, you should verify it is the right mathematical tool for your physics. For a side-by-side comparison of all four ANSYS Fluent multiphase models, see our full guide on choosing the right multiphase model.

When comparing these models directly, keep these technical boundaries in mind:

• Eulerian vs VOF: Choose VOF when you have clear, sharp borders between fluids. You only switch to the Eulerian model when the phases thoroughly mix and interpenetrate. In case you need to know more about this model, read our guide on VOF multiphase model in full.
• Eulerian vs Mixture model: The Mixture model works well for dense flows where particles are tiny and travel at the same velocity as the background fluid. You must switch to the Eulerian method when the phases move at significantly different speeds and experience strong drag or lift forces.
• Eulerian vs DPM: DPM gives you exact physical trajectories for dilute flows. Once your secondary phase volume fraction exceeds 10%, you must transition to the Eulerian approach to prevent solver overload and memory limits.

 Figure 3: Available multiphase models provided in the ANSYS Fluent setup tree.

Conservation Equations in the Eulerian Model

To simulate fluid dynamics accurately, the solver have to calculate the motion and interaction of each phase. Because the Euler-Euler approach treats phases as interpenetrating continua, it solves a distinct set of conservation equations—mass, momentum, and energy—for every individual phase.

Before analyzing the equations, you must define the phases within your multiphase flow CFD setup:

• Primary Phase: The continuous background fluid (e.g., water in a bubble column).
• Secondary Phase: The dispersed phase moving inside the primary fluid (e.g., air bubbles or solid particles). You can define multiple secondary phases.

The Volume Fraction Concept

Because the Eulerian model skips individual particle tracking, it calculates the Volume Fraction (α) of each phase within every computational cell. This metric dictates how much space a phase occupies. The fundamental physical rule of this concept is that the sum of the volume fractions of all phases in a single cell must always equal exactly 1:

Let us look at the core governing equations solved for a specific phase (designated as phase q).

Figure 4: The governing continuity and momentum equations solved for each phase in the Eulerian multiphase model.

1. The Continuity Equation (Conservation of Mass)

This equation tracks the mass of phase q, ensuring mass is mathematically conserved. It balances four specific terms:

• Transient Term: How the mass of phase q changes over time ().
• Convection Term: The net flux of mass moving across the cell boundaries ( ).
• Mass Transfer: Mass actively transferred from phase p to phase q, which occurs during physics like evaporation or condensation.
• Source Term (Sq): Any external mass generation explicitly defined by the user.

2. The Momentum Equation (Conservation of Momentum)

Derived from Newton’s Second Law, this is the most critical equation in gas-liquid flow CFD and granular flows. It calculates the velocity vector (latex] \vec{v}_q [/latex]) of the phase by summing all physical forces acting upon it:

• Pressure Gradient (): Drives the fluid from high-pressure to low-pressure zones.
• Shear Stress (): Represents the viscous forces and internal friction of the fluid.
• Buoyancy & Gravity (): Body forces where gravity pulls heavy phases downward, forcing lighter phases to rise.
• Interphase Forces (): The momentum exchange between phases, including Drag, Lift, Virtual Mass, and Wall Lubrication.

The physical accuracy of your Eulerian model in ANSYS Fluent depends entirely on selecting the correct mathematical models for these interphase forces.

3. The Energy Equation

If your simulation involves thermodynamics, heating, cooling, or phase change (like boiling), the solver activates an energy equation for each phase. It tracks total energy and temperature changes by balancing the volumetric heat sources and the heat transfer between phases using established correlations (such as the Ranz-Marshall or Gunn models).

 

Phase Interaction Overview

Because the Euler-Euler approach assumes multiple phases occupy the same computational cell, those phases must physically push, pull, and transfer energy to each other. Engineers refer to this as Phase Interaction.

The most dominant type of interaction is Interphase Momentum Exchange. If water moves faster than a rising bubble, it pulls that bubble along. ANSYS Fluent calculates this physical behavior using specific models divided into two main categories: drag forces and non-drag forces.

The Role of Drag Force: Drag acts as hydrodynamic friction and serves as the primary force in any multiphase setup. When an air bubble rises, the surrounding water creates resistance that restricts its speed. The software calculates this drag based on the “slip velocity” which is simply the difference in speed between the primary and secondary phases multiplied by a momentum exchange coefficient.

The Role of Non-Drag Forces: While drag is sufficient for basic pipe flows, dense gas-liquid systems require non-drag forces to produce physically realistic results. You must activate these specific forces based on your geometry:

• Lift Force: Pushes bubbles sideways when the surrounding liquid changes speed (shear flow).
• Wall Lubrication Force: Prevents bubbles from artificially attaching to solid boundaries by gently pushing them away from walls.
• Virtual Mass Force: Accounts for the extra energy a light bubble needs to push heavy liquid out of its way during rapid acceleration.
• Turbulent Dispersion Force: Simulates turbulent eddies scattering the bubbles to create an even, realistic mixture. This parameter is largely discussed in our guide on turbulence modeling in Eulerian multiphase and in case you wanna know more, read it.

Figure 5: The Phase Interaction tab in the ANSYS Fluent setup window.

Note: Selecting the wrong drag or lift model will generate completely inaccurate flow fields. If you are unsure which specific forces dictate the physics of your fluid materials and bubble sizes, we highly recommend using our CFD consultation services to share your issue with an expert before you order a project.

 

Figure 6: Interphase momentum exchange forces in the Eulerian multiphase model, including drag and non-drag forces.

Secondary Phase Settings & Particle Size

When configuring the Eulerian multiphase model in ANSYS Fluent, you ought to explicitly define the physical state of your materials. The continuous background fluid (e.g., water) acts as the Primary Phase. The dispersed matter (e.g., air bubbles or sand) becomes the Secondary Phase.

For the solver to resolve interphase physics, there is one non-negotiable rule: you must assign a phase diameter for every secondary phase.

Figure 7: Diameter specification panel for the secondary phase in the ANSYS Fluent setup tree.

The solver relies on this diameter to compute the interfacial contact area. Without it, the software cannot accurately calculate drag forces, lift, or heat transfer in your multiphase flow simulation.

Fluent offers three primary methods to define this diameter:

• Constant Diameter: You input a single fixed value. Use this only if you can safely assume every dispersed particle in the domain is identical in size.
• Sauter Mean Diameter (SMD): Used for poly-dispersed flows where you still need a single average input. SMD mathematically preserves the correct volume-to-surface-area ratio of the actual physical mixture.
• User-Defined Function (UDF): You write custom C-code to dynamically alter the diameter based on local flow conditions (such as pressure changes or high turbulence).

The Importance of Particle Size Distribution (PSD)

In actual industrial systems, bubbles and solid particles never exist in just one uniform size. If you look inside a chemical reactor, you will see a wide Particle Size Distribution (PSD). Tiny, medium, and large bubbles constantly mix together. The size of these bubbles directly controls the total interfacial area, which is the physical boundary where two phases touch. For accurate heat or mass transfer calculations, the solver must know this area.

If you assume a constant diameter, your multiphase flow simulation will produce incorrect thermal and mass transfer results. To solve this issue, engineers couple the main Eulerian solver with the Population Balance Model (PBM). This mathematical framework tracks the population of bubbles over time. It calculates how they constantly break apart (breakage) and merge (coalescence).

You can see a practical example of this in our tutorial project: A Bubble Column CFD Simulation Using the Fluent Population Balance Model (PBM). In this specific project, we simulated a gas-liquid bubble column. Using a single constant bubble size would cause the design to fail because the internal flow is highly dynamic. Turbulence, buoyancy, and shear forces continuously force bubbles to merge (using models like Luo) and rip apart (using models like Lehr).

 Figure 8: Plot showing the volume fraction of a specific bubble size group (a “bin”) calculated.

By coupling the Eulerian model in ANSYS Fluent with the PBM, this setup successfully achieved three things:

• Tracked the Bubble Size Distribution (BSD): It calculated precise bubble sizes dynamically instead of relying on a guess.
• Found the Ideal Operating Zone: The simulation identified a “dominant sweet spot” where specific medium bubble diameters (such as 0.012 m to 0.03 m) reached high volume fractions. In this range, breakage and coalescence balance perfectly.
• Predicted Interfacial Area Accurately: By determining the exact size distribution in every cell, the software accurately calculated the gas holdup and interfacial area. This data is highly essential for real-world chemical manufacturing.

For dense flows where bubble sizes change rapidly, combining the Eulerian approach with the PBM provides the most scientifically accurate result.

Solver Overview and Solution Strategies

After configuring the phases and interphase forces, you must define how ANSYS Fluent resolves the governing equations. In an Eulerian model ANSYS Fluent simulation, the mathematical equations are strongly coupled. Physical phenomena like drag forces and mass transfer generate substantial source terms, which requires a highly capable numerical solver.

For pressure-velocity coupling in the Eulerian framework, ANSYS Fluent provides two primary algorithms:

• Phase Coupled SIMPLE (PC-SIMPLE): This segregated solver resolves the equations sequentially—first momentum, then pressure, and finally volume fraction. It offers excellent stability but often requires longer computational time. If convergence stalls while using PC-SIMPLE, you should decrease the Under-Relaxation Factors (URFs) specifically for the volume fraction and pressure.
• Full Multiphase Coupled Solver: This method calculates volume fraction, pressure, and momentum simultaneously. It is generally the preferred approach for resolving strong phase interactions.

When utilizing the Coupled solver, your setup strategy depends on the time dependency of the flow:

• For Steady-State Problems: The coupled solver operates much faster than PC-SIMPLE. Engineers typically recommend setting the Courant number around 20, paired with higher URFs (0.5 to 0.75).
• For Transient Problems: The efficiency advantage of the coupled solver diminishes at extremely small time steps. If you apply it to a transient multiphase flow simulation, you will achieve better performance using larger time steps combined with significantly high Courant numbers (such as 1E7).

Regardless of your chosen algorithm, Eulerian simulations are highly susceptible to numerical divergence during the initial iterations. You must always launch your simulation using conservative solution controls. Begin with first-order discretization schemes to prevent early instability. Once the flow field establishes a stable pattern, you can progressively increase the under-relaxation factors and transition to high-order schemes (such as QUICK) to minimize numerical diffusion and maximize physical accuracy.

Figure 9: Recommended conservative solver settings for pressure-velocity coupling in the Eulerian multiphase model.

Summary & What’s Next

The Eulerian framework serves as a core tool for resolving dense, heavily coupled interphase interactions in ANSYS Fluent. Throughout this introductory guide, we examined its mathematical foundation, from treating separate phases as interpenetrating continua to solving governing conservation equations. We also highlighted why interphase forces like drag and lift dictate physical accuracy, and how coupling the setup with the Population Balance Model (PBM) accurately resolves real-world Particle Size Distribution (PSD).

This foundation sets the stage for more detailed flow physics. Future articles in this series will cover advanced topics, including phase change dynamics like evaporation and condensation, hydrodynamic cavitation, and the Eulerian Granular model for dense solid-liquid or solid-gas mixtures.