Euler-Euler Two-Fluid Model
Theory and Physics
Overview
Professor, what is the Euler-Euler two-fluid model? From the name, does it handle two fluids simultaneously?
Exactly. The Euler-Euler method treats both the gas and liquid phases (or solid and gas phases) as continua and solves independent conservation equations for each phase. It excels in systems with high volume fractions of dispersed phases, such as bubble columns, slurry reactors, and vapor-liquid two-phase flow piping.
How is it different from the VOF method?
The VOF method is an "interface capturing method" that sharply tracks interfaces and is suitable for free-surface flows with large interface structures. On the other hand, the Euler-Euler method is a "dispersed flow model" that handles systems with numerous dispersed bubbles or droplets. It treats them statistically as local volume fractions rather than resolving individual bubbles.
Governing Equations
Please tell me the specific equations.
It solves the continuity equation and momentum equation for each phase $k$. The continuity equation is as follows.
Here, $\alpha_k$ is the volume fraction of phase $k$, and $\dot{m}_{lk}$ is the mass transfer rate from phase $l$ to phase $k$. The volume fraction constraint $\sum_k \alpha_k = 1$ holds.
What about the momentum equation?
The momentum equation for phase $k$ becomes as follows.
$\mathbf{M}_k$ is the sum of interfacial forces, and this is the core part of the two-fluid model. The pressure $p$ is shared among all phases (shared pressure model), which is the standard approach.
Interfacial Force Models
What kinds of interfacial forces are there?
Taking bubble flow as an example, the main forces acting on the dispersed phase (bubbles) are as follows.
| Force | Representative Model | Physical Meaning |
|---|---|---|
| Drag Force | Schiller-Naumann, Ishii-Zuber, Grace | Resistance to relative velocity |
| Lift Force | Tomiyama, Legendre-Magnaudet | Lateral force due to velocity gradient |
| Wall Lubrication Force | Antal, Tomiyama | Repulsive force near walls |
| Virtual Mass Force | $C_{VM} = 0.5$ | Added mass accompanying acceleration |
| Turbulent Dispersion Force | Lopez de Bertodano, Burns | Dispersion due to turbulent fluctuations |
How should I choose a drag model?
For spherical bubbles, Schiller-Naumann is suitable; for deformed bubbles (high Eotvos number), the Ishii-Zuber or Grace model is appropriate. The Ishii-Zuber model automatically switches the drag coefficient according to the bubble regime (spherical, ellipsoidal, cap), making it highly versatile.
The Philosophy of the Two-Fluid Model – What is Lost by "Averaging"
The Euler-Euler (two-fluid) model treats gas and liquid phases as independent continua, undergoing a "double averaging" process of volume and time averaging for each phase. This operation eliminates the positional information of individual bubbles/droplets, requiring closure models such as "interfacial area density" and "drag coefficient" instead. Ishii & Hibiki's textbook on the two-fluid model remains essential reading for multiphase flow CFD, but the authors themselves repeatedly state that "the uncertainty of closure models is the greatest challenge." Predictions of bubble column height can vary by over 50% depending on the chosen drag model, and the gap between the "philosophical correctness" and "practical accuracy" of models has been a source of long-standing debate.
Physical Meaning of Each Term
- Temporal Term $\partial(\rho\phi)/\partial t$: Imagine the moment you turn on a faucet. At first, water comes out in an unstable, spluttering manner, but after a while, the flow becomes steady, right? This "period of change" is described by the temporal term. The pulsation of blood flow due to heartbeats, or flow fluctuations each time an engine valve opens and closes—all are unsteady phenomena. So what is steady-state analysis? It looks only at "after sufficient time has passed and the flow has settled down"—meaning setting this term to zero. Since computational cost is significantly reduced, starting with a steady-state solution is a basic CFD strategy.
- Convection Term $\nabla \cdot (\rho \mathbf{u} \phi)$: If you drop a leaf into a river, what happens? It gets carried downstream by the flow, right? This is "convection"—the effect where fluid motion transports things. Warm air from a heater reaching the far corner of a room is also because the "carrier," air, transports heat via convection. Here's the interesting part—this term contains "velocity × velocity," making it nonlinear. That is, as flow speed increases, this term rapidly strengthens, making control difficult. This is the root cause of turbulence. A common misconception: "Convection and conduction are similar" → They are completely different! Convection is carried by flow, conduction is transmitted by molecules. There is an order-of-magnitude difference in efficiency.
- Diffusion Term $\nabla \cdot (\Gamma \nabla \phi)$: Have you ever added milk to coffee and left it? Even without stirring, after a while, they naturally mix. That's molecular diffusion. Now, a question—honey and water, which flows more easily? Obviously water, right? Honey has high viscosity ($\mu$), so it flows poorly. Higher viscosity strengthens the diffusion term, making the fluid move in a "thick, sluggish" manner. In low Reynolds number flows (slow, viscous), diffusion dominates. Conversely, in high Re number flows, convection overwhelms, and diffusion plays a supporting role.
- Pressure Term $-\nabla p$: When you push the plunger of a syringe, liquid shoots out forcefully from the needle tip, right? Why? Because the plunger side is high pressure, and the needle tip is low pressure—this pressure difference provides the force that pushes the fluid. Dam discharge works on the same principle. On a weather map, where isobars are densely packed? That's right, strong winds blow. "Flow arises where there is a pressure difference"—this is the physical meaning of the pressure term in the Navier-Stokes equations. A point of confusion here: "Pressure" in CFD is often gauge pressure, not absolute pressure. If results become strange immediately after switching to compressible analysis, confusion between absolute/gauge pressure might be the cause.
- Source Term $S_\phi$: Heated air rises—why? Because it becomes lighter (lower density) than its surroundings, so it is pushed upward by buoyancy. This buoyancy is added to the equation as a source term. Other examples: chemical reaction heat generated by a gas stove flame, Lorentz force acting on molten metal in a factory's electromagnetic pump... These are all actions that "inject energy or force into the fluid from the outside," expressed by source terms. What happens if you forget a source term? In natural convection analysis, forgetting to include buoyancy means the fluid doesn't move at all—a physically impossible result, like turning on a heater in a winter room but the warm air doesn't rise.
Assumptions and Applicability Limits
- Continuum Assumption: Valid for Knudsen number Kn < 0.01 (mean free path ≪ characteristic length)
- Newtonian Fluid Assumption: Linear relationship between shear stress and strain rate (viscosity model needed for non-Newtonian fluids)
- Incompressibility Assumption (for Ma < 0.3): Treat density as constant. For Mach number ≥ 0.3, consider compressibility effects
- Boussinesq Approximation (Natural Convection): Consider density changes only in the buoyancy term, using constant density in other terms
- Non-applicable Cases: Rarefied gas (Kn > 0.1), supersonic/hypersonic flow (shock capturing required), free-surface flow (VOF/Level Set, etc., required)
Dimensional Analysis and Unit Systems
| Variable | SI Unit | Notes / Conversion Memo |
|---|---|---|
| Velocity $u$ | m/s | When converting from volumetric flow rate for inlet conditions, pay attention to cross-sectional area units |
| Pressure $p$ | Pa | Distinguish between gauge and absolute pressure. Use absolute pressure for compressible analysis |
| Density $\rho$ | kg/m³ | Air: approx. 1.225 kg/m³ @20°C, Water: approx. 998 kg/m³ @20°C |
| Viscosity Coefficient $\mu$ | Pa·s | Note confusion with kinematic viscosity coefficient $\nu = \mu/\rho$ [m²/s] |
| Reynolds Number $Re$ | Dimensionless | $Re = \rho u L / \mu$. Indicator for laminar/turbulent transition |
| CFL Number | Dimensionless | $CFL = u \Delta t / \Delta x$. Directly related to time step stability |
Numerical Methods and Implementation
Details of Numerical Methods
Please tell me how to solve the Euler-Euler method numerically.
Basically, an extended version of the SIMPLE-type algorithm is used. The basic flow is to solve the momentum equations for each phase sequentially and perform pressure correction from the shared pressure.
1. Solve each phase's momentum equation with a tentative velocity field
2. Update the volume fraction equation
3. Solve the pressure correction equation (summing the continuity equations of each phase)
4. Correct the velocity field
5. Update the turbulence equations
6. Repeat until convergence
The pressure is shared among all phases, right?
Yes. However, additional terms may be included in the pressure term for the dispersed phase. For example, in granular flow (Eulerian Granular), a solid pressure $p_s$ is added as a function of volume fraction.
Handling of Turbulence Models
What about turbulence models for two-phase flow?
There are three approaches.
| Method | Overview | Application |
|---|---|---|
| Mixture Turbulence Model | Solves one set of k-ε for the mixture | Low void fraction, simple calculation |
| Per-phase Turbulence Model | Solves k-ε for each phase separately | High accuracy but high computational cost |
| Dispersed Phase Turbulence | Derives dispersed phase turbulence from continuous phase k-ε | Standard for bubble flow |
In bubble column analysis, additional source terms for Bubble-Induced Turbulence (BIT) are important. The Sato & Sekoguchi model is most commonly used.
You mean bubbles create turbulence?
Exactly. The wake of bubbles additionally generates turbulent energy. At high void fractions, BIT can become dominant.
Solver Setting Points
Are there any tips for achieving convergence?
The Euler-Euler method has strong nonlinearity and can be difficult to converge.
| Parameter | Recommended Value | Reason |
|---|---|---|
| Volume Fraction Relaxation Factor | 0.2〜0.5 | Suppresses abrupt changes |
| Momentum Relaxation Factor | 0.3〜0.5 | Nonlinearity of interfacial forces |
| Pressure-Velocity Coupling | Phase Coupled SIMPLE | Pressure coupling between phases |
| Time Step | $10^{-3}$〜$10^{-2}$ s | Transient calculation is fundamental |
Steady-state calculations often fail to converge, so it is common to perform transient calculations and take time averages. For systems like bubble columns, run for tens of seconds of physical time before starting to collect statistics.
SIMPLE vs Coupled Solver – Convergence Strategy for Gas-Liquid Two-Fluid Calculations
For the pressure-velocity coupling solver in the Euler-Euler two-fluid model, simply using the single-phase SIMPLE algorithm causes the volume fractions of both phases to intertwine in the pressure equation, slowing convergence. The Coupled Solver adopted by ANSYS CFX (a fully implicit method solving pressure, velocity, and volume fraction simultaneously) offers high stability even when gas-liquid interfaces are steep, with proven results showing iteration counts reduced to 1/3 to 1/5 of SIMPLE. However, the computational cost per iteration is higher than SIMPLE, so overall computation time is case-dependent. OpenFOAM's twoPhaseEulerFoam tends to diverge at high void fractions (α_g > 0.7), requiring careful management of time steps.
Upwind Scheme
First-order upwind: Large numerical diffusion but stable. Second-order upwind: Improved accuracy but risk of oscillations. Essential for high Reynolds number flows.
Central Differencing
Second-order accurate, but numerical oscillations occur for Pe number > 2. Suitable for low Reynolds number diffusion-dominated flows.
TVD Scheme (MUSCL, QUICK, etc.)
Maintains high accuracy while suppressing numerical oscillations via limiter functions. Effective for capturing shock waves and steep gradients.
Finite Volume Method vs Finite Element Method
FVM: Naturally satisfies conservation laws. Mainstream in CFD. FEM: Advantageous for complex shapes and multiphysics. Mesh-free methods like SPH are also developing.
CFL Condition (Courant Number)
Explicit method: CFL ≤ 1 is the stability condition. Implicit method: Stable even for CFL > 1, but affects accuracy and iteration count. LES: CFL ≈ 1 recommended. Physical meaning: Information should not travel more than one cell per time step.
Residual Monitoring
Convergence is judged when residuals for continuity, momentum, and energy drop by 3-4 orders of magnitude. The mass conservation residual is particularly important.
Relaxation Factor
Pressure: 0.2〜0.3, Velocity: 0.5〜0.7 are typical initial values. If diverging, lower the relaxation factor. After convergence, increase to accelerate.
Internal Iterations for Transient Calculations
Iterate within each time step until a steady solution converges. Internal iteration count: 5〜20 times is a guideline. If residuals fluctuate between time steps, review the time step size.
Analogy for the SIMPLE Method
The SIMPLE method is an "alternating adjustment" technique. First, tentatively determine velocity (predictor step), then correct pressure so that mass conservation is satisfied with that velocity (corrector step), and then correct velocity with the corrected pressure—repeating this back-and-forth to approach the correct solution. It resembles two people leveling a shelf: one adjusts the height, the other balances it, and they repeat this alternately.
Analogy for the Upwind Scheme
The upwind scheme is a method that "stands in the river flow and prioritizes upstream information." A person in the river cannot tell where the water comes from by looking downstream—it reflects the physics that upstream information determines downstream. Although first-order accurate, it is highly stable because it correctly captures flow direction.
Numerical Methods and Implementation
Related Topics
なった
詳しく
報告