Fig. 1: The computational grid contains approximately 270,000 computational cells, based on the surface mesh shown.

A recent study documents the ability of computational fluid dynamics (CFD) simulation to accurately predict fan performance over a wide range of flow rates. As HVAC suppliers increasingly rely on numerical simulation to optimize the design of equipment, the accuracy of tools such as CFD to be able to predict fan performance has become a subject of much discussion. To address this issue, results from a CFD analysis of a four-bladed fan have been compared with published experimental wind tunnel data over a wide range of flow rates. The results correlate closely, providing evidence that fan designers can rely on simulation to predict the performance characteristics of new and existing fan designs.

Until recently, fans were designed using essentially the same methods as those used 50 years ago. Typically, this involved hand calculations using airfoil design methods to estimate the performance of various blade design concepts. The problem with these calculations was that they required many simplifying assumptions, thus limiting their accuracy in practical applications. The result was that most real world designs relied upon building and testing prototypes. Prototypes, however, take a considerable period of time to build and test and are also expensive. Moreover, the point measurements used to evaluate a prototype provide little information as to why a particular design performed well or poorly.

Recently, fan designers have turned to CFD simulation, which provides fluid velocity, and pressure and temperature values throughout the solution domain with complex geometries and boundary conditions. As part of the analysis, a designer may change the geometry of the system or the boundary conditions such as inlet velocity, flow rate, rotational speed, etc. and view the effect on the flow. CFD is an effective tool for generating detailed parametric studies and provides more complete information than physical testing, including color-coded graphics that depict flow direction and velocity in all relevant locations.

In order for fan design engineers to have confidence in numerical results, it is essential to validate CFD results using well-documented test cases that are similar in performance range to the systems encountered in industry. This report documents one such case for a four-bladed axial flow or propeller fan. The objectives of the study were to: 1) calculate the performance characteristics of the fan over a range of flowrates, 2) compare the numerical results with experimental data to determine accuracy that can be expected for this type of flow, and 3) examine the predicted flow patterns to see if important flow features are reproduced in the simulation.

The propeller fan considered here is a design described in a recent paper by Oh and Kang [1]. This fan was tested in a wind tunnel over a range of flowrates at a rotational speed of 2,000 rpm and standard atmospheric conditions. The Reynolds number for the tests, based on fan diameter and blade tip speed, is 1.2 x 105. The fan is 110mm in diameter and contains four blades. The blades are thin cambered plates (with circular arc sections) attached to a 25 mm diameter cylindrical shaft, the shaft having a spherical spinner attached to the pressure side.

In tests performed by Kang et. al. [2], the fan was place at the inlet of a .9m x .9m x 3m rectangular chamber (plenum). In the numerical simulation, this chamber was replaced by a .9m diameter cylindrical chamber so that periodic conditions could be imposed. This allowed the calculation to be done on only one of the four blades because of the periodicity of the flowfield, thereby requiring one-fourth the computational effort.

Numerical model

Fig. 3: Pressure and velocity field for the high flow case.

A computational grid for the fan/wind tunnel domain was developed using the GAMBIT CFD preprocessor. A tetrahedral mesh was generated around the blade, with a wedge mesh introduced at the inlet for efficiency. The surface mesh shown in Fig. 1 was used to generate the volume mesh of 269,265 cells.

The rotation of the blade was modeled in FLUENT using the rotating reference frame approach. With this method, the flow equations are solved in the rotating frame of the fan blade. The blade and shaft have zero velocity in this frame, and the outer walls of the tunnel have an angular velocity that is opposite that of the fan when viewed from the lab (stationary) frame. Coriolis forces are included in the motion of the fluid, which in this simulation, is air with constant properties. The effects of turbulence were modeled using the Realizable k-e turbulence model.

Results

Solutions were obtained for a range of flowrates so that fan performance data could be generated and the results compared with the wind tunnel data of Kang et. al. [2]. The non-dimensional parameters used to characterize the fan performance are defined as follows:

Flow Coefficient: F = Q/ND3

Head Coefficient: y = DP/rN2D2

Power Coefficient: Q= Tv/N3D5

In the above, Q is the volume flow rate (m3/sec), N is the rotational speed in rev/sec, D is the fan diameter (m), r is the density (kg/m3), T is the torque (N-m), and is the rotational speed in radians/sec (v = 2pN).

Because of the multi-valued nature of the fan curve at 0.25 A comparison of the predicted head and power coefficient versus flowrate curves (Fig. 2) with the data of Kang show excellent agreement over the entire flowrate range. The computed power coefficients also show good agreement at the higher flow regime, but under-predict the data at low flowrates. This discrepancy is perhaps due to the sensitivity of the blade torque to the points of separation on the blade surface. Given that the flow is expected to be highly separated in the low-flow regime, it would be desirable to refine the mesh appropriately in order to improve the present results.

An important observation made during the course of the calculations was that the solutions can be sensitive to initial conditions for operating points near the multivalued regime of the fan curve.

Fig. 3 shows a contours plot of static pressure distribution on the pressure side of the blade surface along with velocity vectors on a cutting plane y = 0 for the case with a flow coefficient of 0.5. Overall, the velocity vector patterns show that as the flowrate through the fan decreases, the flow downstream of the fan face becomes highly radial.

Conclusions

The performance of a four-bladed axial fan has been computed using CFD software. The results have been compared with wind-tunnel data from the open literature. The predicted performance characteristics are in general found to show excellent agreement with the test data, although power coefficients are under-predicted at low flowrates. From these results, it can be concluded that the performance of this class of axial fan can be predicted with reasonable accuracy over a wide range of flowrates.

References

1. Oh, K-J, Kang, S-H. “A numerical investigation of dual performance characteristics of a small propeller fan using viscous flow calculations,” Computers & Fluids 28 (1999), pp. 815-823.

2. Kang, S-H, Kim, J., Lee, S. “Effects of back-plate on the performance of a small propeller fan,” Transactions of the KSME 1996;20(4), pp. 1491-1500.