撹拌槽CFD
Theory and Physics
Overview
Teacher! In what situations is CFD analysis of stirred tanks used?
It's a technology to predict the flow patterns, mixing time, and power consumption of stirred tanks used in chemical plants, pharmaceutical manufacturing, food processing, water treatment, etc., using CFD. It solves the complex three-dimensional flow created by the rotation of the impeller (stirring blade) using the Navier-Stokes equations.
Governing Equations
Please teach me the basic equations for stirred tanks.
First, dimensionless numbers are important. The impeller Reynolds number and the power number are fundamental.
$N$ is the rotational speed [rps], $D$ is the impeller diameter, and $P$ is the stirring power, right?
Correct. For $Re_{imp} > 10^4$, it's considered fully turbulent; for $Re_{imp} < 10$, it's laminar. The transition region (10 to 10,000) is the most difficult to analyze.
The mixing time $\theta_m$ is defined from the tracer response.
$T$ is the tank diameter, right? $\theta_m N$ is the dimensionless mixing time, and in fully turbulent flow, it becomes a constant (depending on impeller shape).
Exactly. For a 6-blade flat blade turbine (Rushton Turbine), $\theta_m N \approx 30$ to $50$ is a typical value.
Impeller Classification
| Impeller Shape | Np (Turbulent Region) | Flow Pattern | Application |
|---|---|---|---|
| Rushton Turbine (6 flat blades) | 5.0〜5.5 | Radial | Gas-liquid mixing, general reactions |
| Pitched Blade Turbine (45°) | 1.2〜1.7 | Axial-Radial | Solid-liquid suspension, mixing |
| Hydrofoil (A310, A320) | 0.3〜0.4 | Axial | Low shear mixing |
| Anchor | 0.4〜0.8 (Laminar Flow) | Tangential | High viscosity fluids |
| Helical Ribbon | 0.5〜1.0 (Laminar Flow) | Axial+Tangential | Very high viscosity |
The power number is completely different depending on the impeller shape. Rushton is over 5, and Hydrofoil is around 0.3, right?
Rushton creates a strong shear field, making it suitable for gas-liquid dispersion, but power consumption is high. Hydrofoil efficiently circulates liquid with axial flow but has low gas-liquid dispersion capability. They are used according to the application.
Practical Considerations
- When deformation of the free surface (liquid surface) is large, the VOF method is necessary.
- The flow pattern changes significantly depending on the presence of baffles.
- CFD is effective for verifying scale-up rules (constant Np/V, constant tip speed).
- For non-Newtonian fluids (power-law, Herschel-Bulkley), the distribution of apparent viscosity is important.
The Father of Agitation Engineering, Rushton—Establishment of the Rushton Turbine and the Dimensionless Power Number (1950)
The foundation of stirred tank engineering was laid by the American J. H. Rushton. In his 1950 paper "Power Characteristics of Mixing Impellers," he defined the dimensionless power number for impellers, Np = P/(ρN³D⁵), and experimentally proved that Np converges to a constant value in the high Re region (approximately 5 for disc turbine types in fully turbulent flow). This "Rushton turbine" and power number correlation became the de facto standard for agitation design for the next 70 years. In modern CFD, his experiments are used as benchmarks for validating turbulence models, and numerous validation papers have confirmed that the prediction error of the standard k-ε model for Np is around 10-15%. The value of classical experimental data for understanding the limits of CFD accuracy remains unchanged to this day.
Physical Meaning of Each Term
- Time Term $\partial(\rho\phi)/\partial t$: Imagine the moment you turn on a faucet. At first, the water comes out in an unstable, spluttering manner, but after a while, it becomes a steady flow, right? This "period of change" is described by the time term. The pulsation of blood flow due to the heartbeat, or the flow fluctuation 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 this term is set to zero. Since computational cost is significantly reduced, the basic CFD strategy is to first try solving it as steady-state.
- Convection Term $\nabla \cdot (\rho \mathbf{u} \phi)$: What happens if you drop a leaf into a river? It gets carried downstream by the flow, right? This is "convection"—the effect where fluid motion transports things. The 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 the flow becomes faster, 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 put milk in coffee and left it? Even without stirring, after a while, it naturally mixes, right? That's molecular diffusion. Now, next question—honey and water, which flows more easily? Obviously water, right? Honey has high viscosity ($\mu$), so it flows poorly. When viscosity is high, the diffusion term becomes strong, and the fluid moves in a "thick" manner. In flows with low Reynolds numbers (slow, viscous), diffusion is dominant. Conversely, in flows with high Re numbers, convection overwhelmingly dominates, and diffusion plays a supporting role.
- Pressure Term $-\nabla p$: When you push the plunger of a syringe, the liquid comes out forcefully from the needle tip, right? Why? Because the piston side is high pressure, and the needle tip is low pressure—this pressure difference is 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 is generated 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: The "pressure" in CFD is often gauge pressure, not absolute pressure. If results become strange immediately after switching to compressible analysis, it might be due to confusion between absolute/gauge pressure.
- Source Term $S_\phi$: Warmed air rises—why? Because it becomes lighter (lower density) than its surroundings, so it is pushed up 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 the source term. What happens if you forget the source term? In natural convection analysis, if you forget to include buoyancy, the fluid doesn't move at all—you get a physically impossible result where warm air doesn't rise in a room with the heater on in winter.
Assumptions and Applicability Limits
- Continuum Assumption: Valid for Knudsen number Kn < 0.01 (molecular mean free path ≪ characteristic length)
- Newtonian Fluid Assumption: Linear relationship between shear stress and strain rate (viscosity model required for non-Newtonian fluids)
- Incompressible Assumption (for Ma < 0.3): Treat density as constant. For Mach numbers above 0.3, compressibility effects must be considered.
- Boussinesq Approximation (Natural Convection): Density variation is considered only in the buoyancy term; constant density is used in other terms.
- Non-applicable Cases: Rarefied gases (Kn > 0.1), supersonic/hypersonic flow (shock wave 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 pressure 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 | Be careful not to confuse with kinematic viscosity coefficient $\nu = \mu/\rho$ [m²/s] |
| Reynolds Number $Re$ | Dimensionless | $Re = \rho u L / \mu$. Criterion 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
How do you solve the flow where the impeller rotates in a stirred tank?
There are mainly three methods to model impeller rotation in CFD.
Rotation Model Selection
| Method | Overview | Computational Cost | Accuracy |
|---|---|---|---|
| MRF (Multiple Reference Frame) | Treats the rotating region in a steady-state manner | Low (Steady) | Medium |
| Sliding Mesh (SM) | Actually rotates the mesh of the rotating region | High (Unsteady) | High |
| Overset Mesh | Rotates using overlapping meshes | High (Unsteady) | High |
How do you decide between MRF and Sliding Mesh?
MRF is a method to obtain a steady-state solution, used for predicting time-averaged flow patterns or power numbers. Sliding Mesh provides an unsteady solution and is necessary for periodic force fluctuations (torque fluctuations) due to interference between the impeller and baffles, or for tracer tracking to determine mixing time.
Practically, it's efficient to first check the general flow field with MRF, then perform a detailed evaluation with Sliding Mesh.
MRF Settings
Please teach me the steps to set up MRF in Fluent.
1. Create a cylindrical rotating zone around the impeller in the mesh.
2. Cell Zone Conditions → Set Frame Motion → Rotational Velocity for the rotating zone.
3. Connect the top and bottom surfaces of the rotating zone to the external zone using Interface.
4. Do not include baffles in the rotating zone (baffles are on the stationary side).
Guidelines for rotating zone dimensions:
- Diameter: 1.1 to 1.3 times the impeller diameter
- Height: 1.5 to 2.0 times the impeller height
- Distance between impeller and zone boundary: 5 to 15% of impeller diameter
What happens if the rotating zone boundary is too close to the impeller?
The wake generated by the impeller is unnaturally cut off at the rotating zone boundary, reducing the prediction accuracy for power number and pumping capacity. Ensure sufficient margin.
Mesh Strategy
Important points for stirred tank meshing:
| Region | Mesh Size | Remarks |
|---|---|---|
| Impeller blade surface | D/100〜D/50 | Resolve pressure difference on upper/lower blade surfaces |
| Impeller blade tip | D/100 | Vortex generation point |
| Around baffles | T/100 | Vortex behind baffles |
| Near tank wall | T/50〜T/20 | Wall boundary layer |
| Near liquid surface | Refine if free surface analysis | When using VOF |
What's a guideline for the total cell count?
For a standard single-stage impeller + 4 baffle stirred tank, 1 to 5 million cells is a guideline. For long-duration mixing simulations with Sliding Mesh, computation time requires several tens of impeller revolutions (hundreds to thousands of time steps).
Turbulence Model
For fully turbulent flow ($Re_{imp} > 10^4$), Realizable k-epsilon + Standard Wall Function is the standard for stirred tanks. Its high prediction accuracy for Np has been verified in many papers.
However, SST k-omega sometimes captures the vortex structure in the impeller wake better, and it may yield better results for predicting mixing time. LES is for research purposes and is used for detailed visualization of vortex structures.
Coffee Break Yomoyama Talk
MRF Method for Stirred Tank CFD—Numerical Treatment of Impeller Rotation and Its Accuracy Limits
The "MRF method (Multiple Reference Frame method)" most commonly used in stirred tank CFD solves the region around the impeller in a rotating coordinate system and the tank body in a stationary coordinate system. While it allows steady-state calculation and is fast, it cannot capture the unsteady interference between the impeller and baffles (Impeller-Baffle Interaction), reducing prediction accuracy for local flow immediately behind baffles. The more accurate "Sliding Mesh (SM) method" connects the rotating and stationary regions in real-time and performs unsteady calculation, so it is more accurate than MRF but computational cost is 5 to 10 times higher. A practical guideline for decision-making is: "For detailed flow around baffles, mixing time, gas dispersion behavior → SM method"; "For flow rate, pressure, overall flow patterns → MRF method."
Upwind Scheme (Upwind)
1st Order Upwind: Large numerical diffusion but stable. 2nd Order Upwind: Improved accuracy but risk of oscillations. Essential for high Reynolds number flows.
Central Differencing
2nd order accuracy, 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 or 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)
Related Topics
この記事の評価ご回答ありがとうございます！参考に
なったもっと
詳しく誤りを
報告
For fully turbulent flow ($Re_{imp} > 10^4$), Realizable k-epsilon + Standard Wall Function is the standard for stirred tanks. Its high prediction accuracy for Np has been verified in many papers.
However, SST k-omega sometimes captures the vortex structure in the impeller wake better, and it may yield better results for predicting mixing time. LES is for research purposes and is used for detailed visualization of vortex structures.
MRF Method for Stirred Tank CFD—Numerical Treatment of Impeller Rotation and Its Accuracy Limits
The "MRF method (Multiple Reference Frame method)" most commonly used in stirred tank CFD solves the region around the impeller in a rotating coordinate system and the tank body in a stationary coordinate system. While it allows steady-state calculation and is fast, it cannot capture the unsteady interference between the impeller and baffles (Impeller-Baffle Interaction), reducing prediction accuracy for local flow immediately behind baffles. The more accurate "Sliding Mesh (SM) method" connects the rotating and stationary regions in real-time and performs unsteady calculation, so it is more accurate than MRF but computational cost is 5 to 10 times higher. A practical guideline for decision-making is: "For detailed flow around baffles, mixing time, gas dispersion behavior → SM method"; "For flow rate, pressure, overall flow patterns → MRF method."
Upwind Scheme (Upwind)
1st Order Upwind: Large numerical diffusion but stable. 2nd Order Upwind: Improved accuracy but risk of oscillations. Essential for high Reynolds number flows.
Central Differencing
2nd order accuracy, 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 or 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)
Related Topics
なった
詳しく
報告