Engineers at Fluent conducted a CFD simulation of a low-speed propeller fan to determine its accuracy as compared to wind tunnel testing data. The goal was to prove that fan designers can rely on FLUENT to help them to optimize their designs at low cost. Wind tunnel tests of this fan were carried out in an instrumented test chamber at 2000 rpm and a Reynolds Number of 1.2x105. It was found that the fan exhibited an unusual S-shaped variation of pressure rise versus flow rate, and it was speculated that this was due to the large radial flow produced by the fan at lower flow rates.

A computational grid for the fan/wind-tunnel domain was developed using GAMBIT 1.1. Since FLUENT 5 can accommodate unstructured meshes, it was decided to generate a tetrahedral mesh around the blade with a wedge mesh introduced at the inlet for efficiency. The final mesh was composed of 269,265 cells. The inlet was placed two fan diameters upstream of the fan. At low flow rates, however, it was noticed that significant pressure gradients existed from the fan to the inlet. Therefore, for the low-flow-rate cases, the inlet mesh was extended approximately two fan diameters upstream of the original inlet. This mesh contained 11,000 additional cells in the extended inlet region.

The single moving reference frame model was used to model the rotation of the blade, with the absolute velocity formulation option selected. The effects of turbulence were modeled using the realizable k-e turbulence model. The air was assumed to have constant properties, with the viscosity being specified such that the desired Reynolds Number of 1.2x105 was obtained (density = 1.225 kg/m3, viscosity = 1.29351x10-5 Pa-s). Boundary conditions for the model were prescribed as follows: 1) Inlet – Uniform velocity corresponding to a desired flow rate; 2) Outlet – Uniform pressure at atmospheric conditions; 3) Plenum top wall, vertical wall, shroud wall – no slip in absolute frame; 4) Blade, hub/spinner walls – no slip in relative frame; 5) Periodic boundaries – rotationally periodic BCs.

The performance of a four-bladed axial fan was computed using FLUENT 5. The results were compared with wind tunnel data from the open literature. The predicted performance characteristics showed excellent agreement with the test data, although power coefficients were under-predicted at low flow rates. This shows that the performance of this class of axial fan can be predicted with reasonable accuracy over a wide range of flow rates. It provides further evidence that fan designers can rely on CFD analysis to predict the performance characteristics of new and existing fan designs, allowing systems to be optimized at much lower cost than traditional “cut and try” methods.

Head coefficient vs. flow coefficient: comparison of FLUENT 5 results with published data.

Power coefficient vs. flow coefficient: comparison of FLUENT 5 results with published data.

FluentNEWS