Flow in Ducts
Theory and Physics
Overview
Teacher! The analysis of flow inside ducts is the one used for HVAC piping and plant piping, right? Please teach me from the basics.
CFD analysis of duct flow aims to predict pressure loss, flow distribution, and flow maldistribution in piping and duct systems. At the design stage, it visualizes local losses and secondary flows that cannot be fully captured by hand calculations using the Darcy-Weisbach equation alone.
Governing Equations
The basic formula for pressure loss is the Darcy-Weisbach equation, right?
Yes. Frictional loss in straight pipes is described by the Darcy-Weisbach equation.
Here, $f$ is the pipe friction factor, $L$ is the pipe length, $D_h$ is the hydraulic diameter, and $V$ is the cross-sectional average velocity. For laminar flow, $f = 64/Re$, and for turbulent flow, it is obtained from the Colebrook equation.
The Colebrook equation is implicit, so iterative calculation is needed. In practice, is the Swamee-Jain approximation often used?
Exactly. Swamee-Jain is explicit and has sufficient accuracy for practical use.
Local losses (elbows, branches, expansions/contractions) are expressed using a loss coefficient $K$.
| Element | Loss Coefficient K (Guideline) |
|---|---|
| 90° Elbow (R/D=1.5) | 0.2〜0.3 |
| 90° Miter (No Vanes) | 1.1〜1.3 |
| T-Junction (Straight Through) | 0.3〜0.5 |
| T-Junction (Branch) | 0.8〜1.3 |
| Sudden Expansion | $(1 - A_1/A_2)^2$ |
| Sudden Contraction | $0.5(1 - A_2/A_1)$ |
Loss coefficients in hand calculations are from literature values, but with CFD, you can get accurate values specific to the geometry, right?
Yes. Especially for rectangular duct corner pieces and complex branch pipes, literature values are often unavailable, so it's valuable to obtain them via CFD.
Turbulence Model Selection
What turbulence model is suitable for duct flow?
For pipe flow, the Realizable $k$-$\varepsilon$ model is standard. For wall functions, Enhanced Wall Treatment (y+ ≒ 1) is ideal, but even with Standard Wall Function (y+ = 30〜300), pressure loss prediction achieves practical accuracy.
| Turbulence Model | Recommended Application | Notes |
|---|---|---|
| Realizable k-epsilon | Straight pipes / Elbows | General purpose, fast calculation with wall functions |
| SST k-omega | Separation / Sudden expansion | Strong against adverse pressure gradients |
| RSM (Reynolds Stress) | Swirling flow / Secondary flow | High accuracy but high computational cost |
Secondary flow (corner vortices) occurs in rectangular ducts, can it be captured with k-epsilon?
Secondary flow in rectangular ducts originates from Reynolds stress anisotropy, so strictly speaking, RSM is needed. However, if the purpose is pressure loss prediction, k-epsilon can keep the error within about 5%.
The Theory of "Entry Length" — How Many D from the Duct Inlet Until Turbulent Flow is Fully Developed?
The first important concept learned in duct flow theory is the "hydrodynamic entry length." It refers to the distance from the inlet until the flow, influenced by the wall boundary layer, becomes a fully developed turbulent profile across the entire cross-section. For turbulent flow, approximately $x \approx 10 \sim 60 D$ (relative to diameter D) is required. A common mistake in practical CFD analysis is "setting the inlet condition as uniform flow while making the analysis domain just barely long enough." Unless sufficient entry length is secured or a measured velocity profile is set as the inlet condition, pressure loss downstream tends to be underestimated.
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 term describes that "state of change." The pulsation of blood flow from a 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 setting this term to zero. This significantly reduces computational cost, so trying a steady-state solution first is a basic CFD strategy.
- Convection Term $\nabla \cdot (\rho \mathbf{u} \phi)$: 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 end 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 misunderstanding: "Convection and conduction are similar things" → 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. 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 large, the diffusion term becomes strong, and the fluid moves in a "thick" manner. In low Reynolds number flow (slow, viscous), diffusion is dominant. 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? Because the plunger side is high pressure, the needle tip is low pressure—this pressure difference provides the force pushing the fluid. Dam discharge works on the same principle. On a weather map, where isobars are tightly packed? That's 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 you switch to compressible analysis and suddenly get strange results, it might be due to confusing absolute/gauge pressure.
- Source Term $S_\phi$: Heated 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 source terms. 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 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 (molecular 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 change only in the buoyancy term, use 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 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
When solving duct flow with CFD, what should I be careful about regarding mesh and boundary conditions?
Let's start by explaining the mesh.
Mesh Strategy
Does the mesh creation method change between circular pipes and rectangular ducts?
It changes significantly. For circular pipes, O-grid topology (bow-tie type) is recommended, as it easily ensures prism layers orthogonal to the wall. For rectangular ducts, use sweep mesh with prism layers.
The height of the first layer at the wall should match the wall model used.
| Wall Model | Required y+ | First Layer Height Guideline (Re=10⁵, D=300mm) |
|---|---|---|
| Enhanced Wall Treatment | ≒ 1 | Approx. 0.05 mm |
| Standard Wall Function | 30〜300 | 1〜10 mm |
| Scalable Wall Function | > 11.225 | > 0.4 mm |
Setting y+ = 1 increases the cell count considerably. From a pressure loss accuracy perspective, are wall functions sufficient?
For frictional loss in straight pipes alone, wall functions are sufficient. However, for sudden expansions with separation or behind valves, wall resolution (y+ ≒ 1) yields higher accuracy.
Boundary Condition Settings
How do you set the inlet/outlet boundary conditions?
Here are typical setting patterns.
| Boundary | Condition Type | Setting Value |
|---|---|---|
| Duct Inlet | Velocity Inlet | Design air velocity + Turbulence intensity 5%, Hydraulic diameter |
| Duct Outlet | Pressure Outlet | Gauge pressure 0 Pa |
| Fan Location | Fan BC (Pressure Jump) | Fan characteristic curve |
| Damper | Porous Jump | Resistance coefficient according to opening |
| Wall | No-Slip Wall | Roughness height (Steel pipe: 0.045 mm) |
So you input wall roughness into CFD. Where can I look up roughness height for each material?
Representative values are listed in ASHRAE Handbook Fundamentals and Crane TP-410.
| Material | Equivalent Roughness [mm] |
|---|---|
| Galvanized Sheet Metal Duct | 0.09〜0.15 |
| Steel Pipe | 0.045 |
| PVC Pipe | 0.0015 |
| Concrete Duct | 0.3〜3.0 |
| Flexible Duct | 1.0〜4.6 |
Inlet Entry Length Treatment
When assuming fully developed flow, how do you handle the entry length?
The turbulent entry length is roughly $L_{entry} \approx 10 D_h$. If the purpose is not to evaluate pressure loss immediately after the inlet, either provide sufficient entry length or give a Fully Developed Profile as the inlet condition. In Fluent, another method is to use the Mapped condition at the inlet (a periodic condition that maps the outlet velocity profile to the inlet).
Solver Settings
Please tell me the recommended specific solver settings.
| Parameter | Recommended Setting |
|---|---|
| Solver | Pressure-Based, Steady |
| Pressure-Velocity Coupling | SIMPLEC |
| Convection Scheme | Second Order Upwind |
| Pressure Interpolation | Second Order |
| Gradient | Least Squares Cell-Based |
| Convergence Criterion | Residual below 1e-4 + Inlet/Outlet Flow Rate Balance < 0.1% |
Using the inlet/outlet flow rate balance for convergence judgment is practical. Relying on residuals alone might overlook...
Related Topics
なった
詳しく
報告