The simulation has the fan model in a 0.9-m diameter duct and calculates flow on only one of four blades to trim computing time. A surface mesh was used to generate a volume mesh of about 269,000 cells. The inlet mesh extends two fan diameters upstream, except for low flow rates studies. There, large fan-to-inlet pressure gradients required that inlet mesh extended upstream about two additional fan diameters.
 
Head-versus-flow-rate simulations show excellent agreement with experiments over the entire flow-rate range. Computed power coefficients also show good agreement at higher flow regime, but under-predict experimental data at low flow rates (though the trend of higher torque as flow decreases is correctly predicted). The discrepancy may be due to blade-torque sensitivity to the points of separation on the blade surface. Flow is expected to be highly separated in the low-flow regime, so a finer mesh could improve the results. A more sophisticated model, such as the Reynolds Stress Model, may also improve results at low flow rates.
 
Pressure and velocity field for low flow, φ = 0.1
 
Pressure and velocity field for high flow, φ = 0.5.

Designing a fan blade usually involves mounting a prototype in a plenum and measuring pressure and flow rates at different rotational speeds. Such point measurements provide little information as to why designs work well or poorly. Consequently, engineers often settle for less than ideal performance because they don't have tools to optimize designs.

But new computational-fluid-dynamics (CFD) models let fan designers rely less on guess work. Franklyn Kelecy, an application engineer with CFD software developer Fluent Inc., Lebanon, N.H., compared results from a CFD simulation of a four-bladed fan, with published experimental wind-tunnel data, over a wide range of flow rates. "Results correlate closely," he says.

CFD simulations estimate fluid velocity, pressure, and temperature throughout the solution domain with complex geometries and boundary conditions. Designers immediately see the effects of changes to CFD geometry or boundary conditions such as inlet velocity, flow rate, and rotational speed. In addition, simulations give more complete information than physical testing, such as color-coded graphics of flow direction, and velocity. These provide more insight as to why a design is performing as it is, which allows rapid design improvements.

Wind-tunnel tests in this case were done over a range of flow rates at a fan speed of 2,000 rpm and standard atmospheric conditions. The Reynolds number, based on a 110-mm fan diameter and blade tip speed, is 1.2 X 105. Blades are thin, cambered plates (with circular arc sections) attached to a 25-mm diameter shaft.

Kelecy developed a grid for the fan and wind-tunnel domain using the Gambit CFD preprocessor. He says recent developments in meshing simplify and speed what was once a tedious task. A tetrahedral mesh around the blade with a wedge mesh at the inlet solves slightly faster than an all-tetrahedral mesh. And postprocessors integrated with solvers also speed the operations.

Blade rotation was modeled in Fluent using a reference frame that rotates with the fan blades. Here, the blade and shaft have zero velocity while tunnel walls have an angular velocity opposite that of the fan when viewed from the lab (stationary) frame. The simulation included Coriolis forces and turbulence using the Realizable k-e turbulence model.

"The nondimensional parameters used to characterize fan performance include:

flow coefficient: Φ = Q/ND3
head coefficient: ψ = Δ P/ρN2D2
power coefficient: θ = Tω/ N3D5,

where Q = volume flow rate, (m3/sec); N = rotational speed (rps); D = fan diameter (m), ρ = density (kg/m3); T = torque (N-m); and ω = rotational speed (rad/sec).

The fan curve takes on multiple values at 0.25 D upstream of the fan face and plenum-outlet boundary.

"Solutions can be sensitive to initial conditions for operating points near the multivalued regime of the fan curve," he says. For example, when Φ = 0.35. "We found that if the calculation was started from an arbitrary initial guess, the pressure rise at convergence was significantly higher than the data. But when the calculation started from a previous solution, say Φ = 0.4, the predicted pressure rise agreed better with published data. We think separated flow on the blade surface is the culprit, which is triggered by initial conditions and cannot be fully eliminated from the numerical solution."

Contour plots show static pressure distribution on the pressure side of the blade surface along with velocity vectors on a cutting plane (y = 0) for the cases with flow coefficients of 0.1 and 0.5. "At Φ = 0.1, severe adverse pressure gradients on the pressure surface indicate separated flow," says Kelecy. "These are less pronounced when Φ = 0.35. The separated flow disappears when Φ = 0.5 and the pressure distribution becomes more uniform. Low pressure at the blade tip is from tip-clearance effects. Also, velocity-vector patterns show that flow downstream of the fan face becomes highly radial with decreasing fan flow rates. A large volume of fluid is drawn towards the fan at the hub and propelled radially, much like a centrifugal fan," he adds.