Pump CFD Analysis
Theory and Physics
Overview
What does CFD analysis of a centrifugal pump predict?
The three basics are Head, Efficiency, and Shaft Power. Creating the H-Q characteristic curve is the main purpose of CFD.
Definition of Head and Efficiency
Please tell me the head equation.
The pump head is the difference in total head between the inlet and outlet.
In CFD, it's convenient 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 CFD head 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, Frozen Rotor or Sliding Mesh is used. For a guide vane pump without a volute, Mixing Plane can also be used.
Specific Speed as a Compass – The Starting Point of Mixed-Flow Pump Design
The first step in turbo pump design is calculating the Specific Speed (Ns). This dimensionless number, defined by Ns = n√Q / H^(3/4) (n: rotational speed, Q: flow rate, H: head), determines the pump type (centrifugal, mixed-flow, axial). In the design domain for mixed-flow pumps (Ns = 400–1200), the standard two-step approach is theoretically to determine basic dimensions with 1D design (velocity triangles) and then verify 3D flow details with CFD. The theory of specific speed was systematized by American hydraulic engineers in the early 20th century, followed by confusion with different unit systems in Europe and Japan. Today, the IEC standard has internationalized the dimensionless specific speed in m³/s and m units.
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 spluttering and unstable, but after a while, it becomes a steady flow, right? This "during the change" is described by the temporal term. The pulsation of blood flow from a heartbeat, or the flow fluctuation each time an engine valve opens/closes—all are unsteady phenomena. So what is steady-state analysis? Looking only at "after sufficient time has passed and the flow has settled down"—meaning setting this term to zero. This significantly reduces computational cost, so trying a steady-state solution first 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 end of a room is also because the "carrier," air, transports heat by convection. Here's the interesting part—this term includes "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" → 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 easier? Obviously water, right? Honey has high viscosity ($\mu$), so it flows poorly. Higher viscosity strengthens the diffusion term, making the fluid move "sluggishly." 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 a syringe plunger, liquid shoots out forcefully from the needle tip, right? Why? Because the plunger side is high pressure, the needle tip is low pressure—this pressure difference becomes the force pushing the fluid. Dam discharge works on the same principle. On a weather map, where isobars are tightly packed? Right, strong winds blow. "Where there is a pressure difference, flow is generated"—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. When switching to compressible analysis, if results become strange, it might be due to mixing up absolute/gauge pressure.
- Source term $S_\phi$: Heated 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. Others include chemical reaction heat from 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 buoyancy means the fluid doesn't move at all—a physically impossible result where warm air doesn't rise in a heated winter room.
Assumptions and Applicability Limits
- Continuum assumption: Valid for Knudsen number Kn < 0.01 (mean free path ≪ 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 number 0.3 and above, 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, 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?
Pump Re is on the order of $10^6$, sufficiently high, so wall functions with y+ = 30–100 generally yield reasonable results. However, for higher accuracy, the Low-Re solution with y+ < 2 is recommended. Particularly for predicting blade surface separation at partial load, wall functions have limitations.
Boundary Conditions
What are typical pump boundary conditions?
- 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
Setting the outlet to fixed static pressure and varying the inlet flow rate is the most stable configuration.
Between Axial and Centrifugal – Numerical Difficulties in Mixed-Flow Pump CFD
Mixed-flow pumps lie in the intermediate specific speed (Ns) range between axial and centrifugal pumps (Ns = 400–1200), and because flow mechanisms from both types coexist, numerical analysis is difficult. The axial flow component is dominated by tip vortices and secondary flows, while the centrifugal component is affected by flow curvature due to Coriolis forces. In this mixed region, turbulence model selection directly impacts pump efficiency prediction, and many comparative studies show the k-ω SST model is typically several percent more accurate than standard k-ε. In mesh design, balancing resolution in the axial, circumferential, and radial directions is important; making one direction finer is not necessarily better.
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
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 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)
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 timestep.
Residual Monitoring
Convergence is judged when residuals for Continuity Equation, momentum, and energy drop by 3–4 orders of magnitude. The mass conservation residual is particularly important.
Relaxation Factors
Pressure: 0.2–0.3, Velocity: 0.5–0.7 are typical initial values. If diverging, lower the relaxation factors. After convergence, increase to accelerate.
Internal Iterations for Unsteady Calculations
Iterate within each timestep until the steady solution converges. Internal iteration count: 5–20 iterations is a guideline. If residuals fluctuate between timesteps, review the timestep size.
Analogy for the SIMPLE Method
The SIMPLE method is an "alternating adjustment" technique. First, velocity is tentatively determined (predictor step), then pressure is corrected so that mass conservation is satisfied with that velocity (corrector step), and velocity is revised with 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 looking downstream can't tell where the water comes from—it's a discretization method reflecting the physics that upstream information determines downstream. It's first-order accurate but highly stable because it correctly captures 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 design flow rate $Q_d$
2. Set 7–10 points in the flow rate 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, efficiency η at each point and plot
Why does convergence worsen on the low flow rate side?
At low flow rates, the incidence angle at the impeller inlet becomes large, causing large-scale separation on the blade surface. In steady-state calculations, trying to converge an unsteady separation structure into a single solution causes oscillations. Below about 0.3$Q_d$, unsteady calculations are often necessary.
Related Topics
なった
詳しく
報告