Pump CFD Analysis
Theory and Physics
Overview
What does CFD analysis of a centrifugal pump predict?
There are three basics: Head, Efficiency, and Shaft Power. The main purpose of CFD is to create the H-Q characteristic curve.
Head and Efficiency Definitions
Please tell me the head equation.
The pump head is the difference in total head between the inlet and outlet.
In CFD, it's simpler to calculate directly from the total pressure difference. $H = (p_{t2} - p_{t1})/(\rho g)$.
Efficiency is divided into hydraulic efficiency and overall efficiency.
$\tau$ is the impeller torque obtained from CFD, and $\omega$ is the angular velocity.
What's the difference between hydraulic efficiency and overall efficiency?
Hydraulic efficiency includes only hydrodynamic losses, excluding disc friction and leakage. Overall efficiency includes all: disc friction, leakage flow, and mechanical losses. What CFD directly yields is hydraulic efficiency; disc friction and leakage won't appear unless a gap model with the wear ring is included.
Euler Head (Theoretical Head)
The theoretical head can be derived from the Euler equation, right?
Assuming no swirl at the inlet for a centrifugal pump ($C_{\theta 1}=0$), it becomes $H_{Euler} = U_2 C_{\theta 2}/g$. The head considering the slip factor $\sigma_s$ is $H_{th} = \sigma_s \cdot H_{Euler}$. The head from CFD corresponds to this theoretical head plus hydraulic losses.
Steady-State Analysis with MRF Method
Is the MRF method common for pump CFD?
For obtaining the H-Q curve, the MRF method (steady-state) is standard. For cases with a volute, use Frozen Rotor or Sliding Mesh. For pumps with guide vanes but no volute, Mixing Plane can also be used.
The Foundation of Centrifugal Pump Theory—Euler's Pump Equation (1754) and Its Connection to the Modern Era
The fundamental theory of centrifugal pumps, Euler's "Turbo Machine Equation" (U1*Vtheta1 - U2*Vtheta2 = g*H), was derived by Leonard Euler in 1754. The principle that the energy imparted to a fluid by a rotating body is proportional to the difference between the circumferential and swirl velocity components at the inlet and outlet remains an immutable truth that appears in the first chapter of textbooks on pumps, turbines, and compressors even 270 years later. Euler was the greatest mathematician of the 18th century, leaving monumental achievements not only in fluid machinery but also in rigid body mechanics, mathematics, and optics. Remarkably, the origin of the modern CFD Navier-Stokes equations, the "Euler Equations (inviscid)," also bears his name—the fact that Euler's name is engraved in both the fundamental theory of turbomachinery and the numerical methods of CFD is proof of how much fluid mechanics is built upon his work.
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 from a heartbeat, the 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 drops significantly, starting with a steady-state solution is a basic CFD strategy.
- 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. 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 it difficult to control. This is the root cause of turbulence. A common misconception: "Convection and conduction are similar" → They're completely different! Convection is carried by flow, conduction is transmitted by molecules. There's 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 a 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 low Reynolds number flow (slow, viscous), diffusion dominates. Conversely, in high Re number flow, convection overwhelms, and diffusion becomes 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? The piston side is high pressure, the needle tip is low pressure—this pressure difference creates the force that pushes the fluid. Dam discharge works on the same principle. On a weather map, where isobars are tightly 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: "Pressure" in CFD is often gauge pressure, not absolute pressure. If results go wrong immediately after switching to compressible analysis, it might be due to mixing up absolute/gauge pressure.
- Source Term $S_\phi$: Warmed air rises—why? Because it becomes lighter (lower density) than its surroundings, so it's 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, forgetting to include buoyancy means the fluid doesn't move at all—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 (mean free path of molecules ≪ characteristic length)
- Newtonian Fluid Assumption: Shear stress and strain rate have a linear relationship (non-Newtonian fluids require viscosity models)
- Incompressibility Assumption (for Ma < 0.3): Treat density as constant. For Mach numbers above 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 (requires shock capturing), free surface flow (requires VOF/Level Set, etc.)
Dimensional Analysis and Unit Systems
| Variable | SI Unit | Notes / Conversion Memo |
|---|---|---|
| Velocity $u$ | m/s | When converting from volumetric flow rate for inlet conditions, be careful with 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 | Be careful not to confuse with kinematic viscosity $\nu = \mu/\rho$ [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
Mesh Generation
What should I be careful about with centrifugal pump meshing?
For the impeller, generating a structured grid with TurboGrid yields the highest quality. For the volute, use an unstructured tetra/polyhedral mesh.
Region Mesh Type Approx. Cell Count Tool Impeller Structured Grid (H/J/L+O-grid) 0.5～1.5 million/pitch TurboGrid Volute Unstructured Tetra+Prism 1～3 million Fluent Meshing, STAR-CCM+ Suction Pipe Structured or Unstructured 0.2～0.5 million Any Wear Ring Gap Structured (Hexahedral) 0.1～0.3 million Manual
Should the wear ring gap also be included in the model?
It's essential if you want to evaluate the effect of leakage flow. The gap is very narrow, 0.2～0.5mm, so a minimum of 10 cells radially and 50 cells axially is recommended.
Turbulence Model Selection
Which turbulence model is suitable for pumps?
SST k-omega is the standard. It excels at predicting adverse pressure gradients and separation on blade surfaces. For pumps, since the number of blades is small (5～7) and blade loading is high, k-epsilon tends to underpredict separation.
Should I use wall functions or Low-Re?
Since pump Re is on the order of $10^6$ and sufficiently high, wall functions with y+ = 30～100 generally yield reasonable results. However, for higher accuracy, the Low-Re approach with y+ < 2 is recommended. Particularly for predicting blade surface separation at partial load, the limitations of wall functions become apparent.
Boundary Conditions
What are typical boundary conditions for a pump?
- Inlet: Mass flow rate specified (varied from 0.2 to 1.4 times design flow rate)
- Outlet: Static pressure specified (atmospheric or actual system pressure)
- Blade surface, Hub, Shroud: No-slip wall
- Impeller-Volute Interface: Frozen Rotor or Sliding Mesh
The most stable setup is to fix the outlet static pressure and vary the inlet flow rate.
Coffee Break Yomoyama Talk
Practical Settings for Pump CFD—Choosing Between Rotating Reference Frames and MRF, and Mesh Requirements
The first setting to decide in centrifugal pump CFD analysis is "MRF (Moving Reference Frame) vs. Sliding Mesh (SM)." For confirming basic characteristics like total head and efficiency near the design point, MRF (steady-state) is overwhelmingly advantageous in terms of computation time, providing comparable accuracy at 1/10 to 1/50 the cost of sliding mesh. For pumps where blade passing frequency (BPF) vibration, noise, or fatigue are issues, unsteady SM is necessary. Mesh requirements are a practical guideline of at least 20-30 prism layers normal to the blade surface in the impeller passage (when using low-Re wall treatment with y+<1) and a minimum of 0.5 million cells per blade passage. For full model analysis including the volute and scroll, a total cell count of 3-5 million is typical.
Upwind Differencing (Upwind)
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 (Central Differencing)
Second-order accurate, but numerical oscillations occur for Peclet number > 2. Suitable for low Reynolds number, diffusion-dominated flows.
TVD Schemes (MUSCL, QUICK, etc.)
Maintain high accuracy while suppressing numerical oscillations via limiter functions. Effective for capturing shocks 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 methods: CFL ≤ 1 is the stability condition. Implicit methods: 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 timestep.
Residual Monitoring
Convergence is judged when the residuals for continuity, momentum, and energy drop by 3-4 orders of magnitude. The mass conservation residual is particularly important.
Relaxation Factors
Typical initial values: Pressure: 0.2～0.3, Velocity: 0.5～0.7. If diverging, lower the relaxation factors. After convergence, increase to accelerate.
Internal Iterations for Unsteady Calculations
Iterate within each timestep until a steady solution converges. Guideline for internal iteration count: 5～20 iterations. If residuals fluctuate between timesteps, review the timestep size.
Analogy for the SIMPLE Method
The SIMPLE method is an "alternating adjustment" technique. First, velocities are tentatively determined (predictor step), then pressure is corrected so that mass conservation is satisfied with those velocities (corrector step), and velocities are revised using the corrected pressure—this back-and-forth is repeated 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 Upwind Differencing
Upwind differencing 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's a discretization method reflecting the physics that upstream information determines downstream. Although first-order accurate, it is highly stable because it correctly captures the flow direction.
What should I be careful about with centrifugal pump meshing?
For the impeller, generating a structured grid with TurboGrid yields the highest quality. For the volute, use an unstructured tetra/polyhedral mesh.
| Region | Mesh Type | Approx. Cell Count | Tool |
|---|---|---|---|
| Impeller | Structured Grid (H/J/L+O-grid) | 0.5～1.5 million/pitch | TurboGrid |
| Volute | Unstructured Tetra+Prism | 1～3 million | Fluent Meshing, STAR-CCM+ |
| Suction Pipe | Structured or Unstructured | 0.2～0.5 million | Any |
| Wear Ring Gap | Structured (Hexahedral) | 0.1～0.3 million | Manual |
Should the wear ring gap also be included in the model?
It's essential if you want to evaluate the effect of leakage flow. The gap is very narrow, 0.2～0.5mm, so a minimum of 10 cells radially and 50 cells axially is recommended.
Which turbulence model is suitable for pumps?
SST k-omega is the standard. It excels at predicting adverse pressure gradients and separation on blade surfaces. For pumps, since the number of blades is small (5～7) and blade loading is high, k-epsilon tends to underpredict separation.
Should I use wall functions or Low-Re?
Since pump Re is on the order of $10^6$ and sufficiently high, wall functions with y+ = 30～100 generally yield reasonable results. However, for higher accuracy, the Low-Re approach with y+ < 2 is recommended. Particularly for predicting blade surface separation at partial load, the limitations of wall functions become apparent.
What are typical boundary conditions for a pump?
- Inlet: Mass flow rate specified (varied from 0.2 to 1.4 times design flow rate)
- Outlet: Static pressure specified (atmospheric or actual system pressure)
- Blade surface, Hub, Shroud: No-slip wall
- Impeller-Volute Interface: Frozen Rotor or Sliding Mesh
The most stable setup is to fix the outlet static pressure and vary the inlet flow rate.
Practical Settings for Pump CFD—Choosing Between Rotating Reference Frames and MRF, and Mesh Requirements
The first setting to decide in centrifugal pump CFD analysis is "MRF (Moving Reference Frame) vs. Sliding Mesh (SM)." For confirming basic characteristics like total head and efficiency near the design point, MRF (steady-state) is overwhelmingly advantageous in terms of computation time, providing comparable accuracy at 1/10 to 1/50 the cost of sliding mesh. For pumps where blade passing frequency (BPF) vibration, noise, or fatigue are issues, unsteady SM is necessary. Mesh requirements are a practical guideline of at least 20-30 prism layers normal to the blade surface in the impeller passage (when using low-Re wall treatment with y+<1) and a minimum of 0.5 million cells per blade passage. For full model analysis including the volute and scroll, a total cell count of 3-5 million is typical.
Upwind Differencing (Upwind)
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 (Central Differencing)
Second-order accurate, but numerical oscillations occur for Peclet number > 2. Suitable for low Reynolds number, diffusion-dominated flows.
TVD Schemes (MUSCL, QUICK, etc.)
Maintain high accuracy while suppressing numerical oscillations via limiter functions. Effective for capturing shocks 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 methods: CFL ≤ 1 is the stability condition. Implicit methods: 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 timestep.
Residual Monitoring
Convergence is judged when the residuals for continuity, momentum, and energy drop by 3-4 orders of magnitude. The mass conservation residual is particularly important.
Relaxation Factors
Typical initial values: Pressure: 0.2～0.3, Velocity: 0.5～0.7. If diverging, lower the relaxation factors. After convergence, increase to accelerate.
Internal Iterations for Unsteady Calculations
Iterate within each timestep until a steady solution converges. Guideline for internal iteration count: 5～20 iterations. If residuals fluctuate between timesteps, review the timestep size.
Analogy for the SIMPLE Method
The SIMPLE method is an "alternating adjustment" technique. First, velocities are tentatively determined (predictor step), then pressure is corrected so that mass conservation is satisfied with those velocities (corrector step), and velocities are revised using the corrected pressure—this back-and-forth is repeated 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 Upwind Differencing
Upwind differencing 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's a discretization method reflecting the physics that upstream information determines downstream. Although first-order accurate, it is highly stable because it correctly captures the flow direction.
Practical Guide
H-Q Characteristic Calculation Procedure
How do you create the H-Q characteristic curve?
1. Converge a steady-state MRF (or Frozen Rotor) calculation at the design flow rate $Q_d$
2. Set 7～10 points in the range $0.2Q_d$ to $1.4Q_d$
3. Recalculate at each point by changing the inlet mass flow rate (using the previous point's result as the restart value)
4. Calculate head H, torque τ, and efficiency η at each point and plot
Why does convergence worsen on the low flow rate side?
Related Topics
なった
詳しく
報告