Effect of turbulent boundary layer on the surface ...

Journal of Mechanical Science and Technology 27 (9) (2013) 2673~2681 www.springerlink.com/content/1738-494x

DOI 10.1007/s12206-013-0711-9

Effect of turbulent boundary layer on the surface pressure around trench cavities† Young-Tae Lee and Hee-Chang Lim* School of Mechanical Engineering, Pusan Nat’l University, San 30, Jangjeon-Dong, Geumjeong-Gu, Busan, 609-735, Korea (Manuscript Received January 17, 2013; Revised April 13, 2013; Accepted April 17, 2013) ----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------

Abstract This paper presents a parametric study on steady incompressible flow past cavities. Numerical calculations were performed around two- and three-dimensional trench cavities. Numerical and experimental results were compared to understand the fluid dynamics mechanism of vortex generation and diffusion in shear and mixing layers around cavities. Using the commercial computational fluid dynamics software FLUENT, the standard k-ε and k-ω shear stress transport (SST) models were applied to solve the Reynolds-averaged Navier– Stokes (RANS) equation of turbulent wind flow. The calculations were performed using a Reynolds number of 1.6 × 104 based on the free-stream velocity U∞ and the length of the cavity L. Computational meshes were carefully designed to be dense on the cavity surface and to be coarse in far-field to obtain an appropriate solution for the RANS equation for cavity flow because these measures result in decreased computational cost and more rapid convergence. The standard k-ε model produces an almost similar distribution regardless of whether the grid is two- or three-dimensional, whereas the k-ω SST model has different values of velocity, surface pressure, and Reynolds stress. The three-dimensional grid shows better prediction of surface pressure around the cavity compared with the twodimensional grid. Keywords: Trench cavity; Cavity flow; Surface pressure; Shear flow ----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------

1. Introduction Over the past 50 years, numerous studies have focused on numerical calculations and experimental measurements of flow around a cavity under a turbulent boundary layer. Shear flow in the cavity generates intense, self-sustained oscillations arising from a feedback loop consisting of the following chain of events. The growth and convection of instability waves in the shear layer induce large-amplitude pressure disturbances as vertical perturbations impinge on the downstream corner of the cavity. The wind tunnel experiments of Refs. [1] and [2] on flow in a rectangular cavity or slot are some of the first to demonstrate the importance of modeling intense, selfsustained oscillations from the flow past a cavity in connection maintaining a comfortable environment despite noise and vibration. Examples of cavities in high-speed flow include flows over weapon bays, wheel wells, aircraft hulls for an external case, and flow inside intake/exhaust manifolds in engines for an internal case, and even wind flow over complex terrains. (e.g., Refs. [3-6]). Low-speed examples include flows over surfaces with ribbing in heat exchangers and microelectronic chips, as well as electronic devices on printed circuit boards. Ref. [7] experimentally and analytically analyzed the *

Corresponding author. Tel.: +82 51 510 2302, Fax.: +82 51 512 5236 E-mail address: [email protected] † Recommended by Associate Editor Cheolung Cheong © KSME & Springer 2013

physical mechanisms in cavities exposed to both subsonic and supersonic free-stream flows. They explained the mechanisms through which the shear layer and free-stream flow interact with the aft wall of the cavity, and they evaluated several concepts behind the suppression of discrete tones, such as slanting of the aft wall. Pressure oscillation inside the cavity induces aerodynamic instabilities and complicates three-dimensional (3D) turbulent flow [8]. Fig. 1 illustrates the cavity flow generating a selfsustained oscillation and complicated shear flow. As shown in the figure, vortex shedding from the mixing layer impinges the downstream corner of the cavity, resulting in high-pressure waves. Some of these waves return to the upstream corner and interact with the mixing layer. Meanwhile, other waves shatter and penetrate into the cavity or solid plate and thus shake the nearby air, resulting in radiated acoustic waves. Recent developments in numerical and experimental technologies have extended this type of research in the direction of capturing the more complicated 3D flows around cavities. Some advanced optical measurements have been performed in wind tunnels ([9-13]). Ref. [13] investigated the flow structure past rectangular, triangular, and semicircular cavities with a length-to-depth ratio of 2:1 using particle image velocimetry. They performed this technique at a large-scale tunnel with three Reynolds numbers (1,230, 1,460, and 1,700) based on inflow momentum thickness for each cavity type. Ref. [13]

2674

Y.-T. Lee and H.-C. Lim / Journal of Mechanical Science and Technology 27 (9) (2013) 2673~2681

Fig. 1. Flow characteristics around a cavity.

presented the average velocity, vorticity, Reynolds stress, and streamline plots for each cavity type; thus, their study could serve as a reference database for future comparisons with other modeling resources. However, their models did not find significant variation because of the limitations of optical measurements (i.e., the laser light beam must be illuminated). Ref. [14] used a numerical approach to analyze the unsteady flow past 3D cavities and to observe a complex interaction between the external flow and the recirculating flow inside the cavity. Most of the abovementioned studies, which are mainly experimental, analytical, and numerical in nature, focused on square or rectangular cavity flows, although cavities may be non-rectangular in applications. In addition, they addressed merely the strong self-sustained pressure oscillations that arise from the vorticity–pressure feedback loop encountered in this type of flow. The present study was motivated by the demand for detailed fundamental information about 2D and 3D trench cavities to understand the mechanism through which strong surface pressure can be generated from the downstream corner of cavities, as well as the need to describe the general flow characteristics around cavities. This study also aims to understand the self-sustainable oscillations inside the cavities by comparing the effects of 2D flow around cavities and 3D flow around trench cavities. To achieve the current objectives, we performed a numerical calculation based on two-equation turbulence models, namely, k-ε and k-ω shear stress transport (SST) models. The models were applied for the final Reynolds-averaged Navier–Stokes (RANS) equation of turbulent flow at a Reynolds number of 1.6 × 104. Large eddy simulation (LES) and direct numerical simulation (DNS) are expected to serve as alternative tools for solving such a problem because these can directly compute the flow structures around cavities (i.e., wind engineering and fluid dynamic field). However, from the engineering point of view, the current study solved the Navier–Stokes equation based on the two-equation turbulence models ([15-18]). Fluid flow simulations are carried out on 2D and 3D trench cavities placed in a turbulent boundary layer at a Reynolds number of 1.6 × 104 based on the free-stream velocity U and the length of the cavity L, which are the velocity at the top of the cavity and the depth height, respectively. This paper is organized as follows. Section 2 outlines basic configuration and numerical parameters. Section 3 describes the RANS numerical method in detail. Section 4 analyzes the velocity

Fig. 2. Computational domain of 2D (up) and 3D trench (down) cavities.

and pressure distribution of 2D and 3D trench cavities. Finally, section 5 presents the major conclusions.

2. Numerical method 2.1 Configuration of 2D and 3D trench cavities Fig. 2 displays the 2D and 3D trench cavities describing the size and the geometric configuration used for the current computation. The nondimensional size (L × D) of the cavities used in this study is 0.1length × 0.1depth, which is located in the bottom center of the entire computational domain. The typical size of the cavities is all the same as defined (0.1), whereas the full size of the computational domain requires more space to create stress-free boundaries and to avoid disturbing the wake flow behind the cavity. Therefore, the full length of the streamwise domain is set to 2.1 in the flow direction (x direction) and 0.5 in the vertical direction (z direction). As a base approach, a simplified 2D cavity is created to compare with references. The cavity is then examined using turbulence models. A turbulent flow past a 3D trench cavity with sharp edges is also modeled on a Cartesian coordinate system. The case of a trench with smoothed edges is presented in Ref. [19]. Fig. 3 displays the typical grid structures of 2D and 3D trench cavities for the current numerical simulation. Computa-


2675

(2) where x j , u1 , ui' , p, v, and f i indicate Cartesian coordinates, mean velocity, fluctuating velocity, pressure, kinematic viscosity, and “other” body forces, respectively. Transport equations for the standard k-ε model: The standard k-ε model solves two additional equations. One is the kinetic energy (k) and the other is the dissipation rate (ε). The transport equations for k and ε are written as (3)

(4)

(5)

Fig. 3. Grid structures of 2D (up) and 3D trench (down) cavities for numerical calculation.

tional meshes are carefully designed to be densely attracted to the cavity surface and coarsely far-field to obtain an appropriate solution for the RANS equation for cavity flows. Such design helps reduce computational cost and ensures rapid convergence. The 2D and 3D meshes are numerically generated by quadrilateral and hexahedral cells, respectively, with 27,000 cells for the former and 400,000 cells for the latter.

where Cε 1 and Cε 2 are both constants, σ ( k ) and σ (ε ) are the turbulent Prandtl numbers for k and ε, respectively ( Cµ = 0.09, Cε 1 = 1.92, Cε 2 = 1.44, σ ( k ) = 1.0, σ ( ε ) = 1.3 ), and vt is eddy viscosity. Transport equations for the k-ω SST model: The k-ωSST model was developed by Menter to blend effectively the robust and accurate formulation of the k-ω model in the nearwall region with the free-stream independence of the k-ε model in the far-field. Turbulence kinetic energy k and specific dissipation rate ω are obtained from the transport equations:

(6) 2.2 Governing equations (standard k-ε and k-ω SST models) The fluid motion satisfies the Navier–Stokes equations, which are discretized using second-order finite volume methods in space. Simulations are carried out by assuming that no other thermal sources are present and that no stratification occurs, which equates to regarding the flow as a neutrally developed turbulent boundary layer. Flow characteristics are analyzed by using two two-equation turbulence models, namely, the standard k-ε and k-ω SST models. The problem is formulated using the computational fluid dynamics commercial software ANSYS FLUENT® [20], which is based on the finite volume method. The numerical models and methods used in the software are widely known. Nevertheless, several important points of the numerical computation are briefly introduced. The governing equations are modeled based on the 2D and 3D steady, incompressible Navier–Stokes equations. These equations can be written in non-dimensional form as (1)

(7)

(8)

where P% ( k ) represents the production of turbulence kinetic energy and is defined as P% ( k ) = min( P ( k ) , 10 ρβ *kω ) and P ( k ) = ρ ui' u j' / ∂xi . β *ω k and βω 2 represent the dissipation of k and ω, respectively. The k-ω SST model is based on both standard k-ω and k-ε models. To combine these two models, the standard k-ε model is transformed into equations based on k and ω, leading to the introduction of a cross-diffusion term. D (ω ) is defined as D (ω ) = 2(1 − F1 ) ρσ ω ,2 × 1/ ω × ∂k / ∂x j × ∂ω / ∂x j . The numerical simulation and the wind tunnel experiment are compared using statistical methods to evaluate the performance of the turbulence models. The comparison is based on salient parameters, including surface pressure, velocity, and shear stress.

2676


Fig. 4. Computational domain of a 2D cavity with a 3D domain.

2.3 Boundary conditions Fig. 4 displays the boundary conditions used in a channel flow with 2D and 3D trench cavities. The boundary conditions, that is, inlet velocity with a turbulent boundary layer, outflow, and periodic symmetry boundary conditions, are applied to the inlet, outlet, side, and top of the channel. The outflow conditions are assumed to be a zero diffusion flux for all flow variations. Especially, the zero diffusion flux condition implies that the conditions of the outflow plane are extrapolated from within the domain and have no impact on the upstream flow. This concept explains the physical aspect of the fully developed flows. Only diffusion fluxes in the direction normal to the exit plane are assumed to be zero. In addition, the wall boundary condition is applied to the bottom face of the channel to generate a turbulent boundary layer. The inlet boundary condition is assumed to follow the one-seventh power-law profile against height y:

.

(9) Fig. 5. k, ε and ω profiles at inlet and x/L = -1.

Symmetry is applied at the top of the channel to induce a fully developed profile when δ is at the top of the channel height. In this study, the mean streamwise velocity profile is prescribed, and the peak (free-stream) velocity is set to 2.5 m/s at the top of the channel. During numerical calculation, residuals based on the convergence criterion are less than 10-6 for all variables. Applying an available measurement result under similar conditions is often necessary to obtain reliable data based on numerical calculation. For example, a set of available wind tunnel experiments is performed for at least the inlet boundary condition and surrounding environments. In the present study, the k-profile (i.e., the turbulent kinetic energy indicator) and the mean velocity profile are both similarly imposed on the entire inlet face. These inlet conditions are properly tuned to obtain an appropriate solution with various turbulence-modeling standard k-ε and k-ω SST models. Fig. 5 shows the k , ε , ω profile at the inlet and further downstream at x/L=-1, which is from the leading edge of the cavity (i.e., originating from the top left corner of the cavity). As shown in the figure, fully developed k-profiles of turbulence-modeling standard k-ε and k-ω SST models show a clear difference close to the wall surface. As explained earlier,

the study undertakes this calculation based on two models, wall functions for k-ε and near-wall model for k-ω SST, to resolve the near-wall region. The y+ values at x/L = -1 for the k-ε and k-ω models are 30 and 0.8, respectively. These values are typically used in each model. The reason they have different shapes, especially close to the surface, is that the standard k-ε model uses the wall law in the viscous sublayer, whereas the k-ω SST model does not. The k-ω SST model is recently known to be more accurate than the k-ε model in near-wall layers. This model is also a reference for flows with wallbounded boundary layer and free shear, but not for flows with pressure-induced separation. In addition, this model depends highly on the values of ω in the freestream outside the boundary layer ([21, 22]), which is not considered in the current study. In the outlet boundary, the outflow condition is used to create the same flow rate as the inlet flow. That is, the outflow indicates that the outlet flow rate is equal to the inlet flow rate.


Fig. 6. Mean and turbulent intensities distribution used in the inlet condition of the 2D and 3D computational domains. Mean velocity profiles are compared with the corresponding wind tunnel experiment. Left figure: mean velocity profiles; right: turbulence intensity profiles. Figures are all non-dimensionalized by the velocity at the cavity height, UL.

2677

Fig. 7. Streamwise velocity profiles at equispace locations inside the cavity.

3. Results and discussion 3.1 Approaching flow Fig. 6 illustrates the typical characteristics of numerically generated turbulence boundary layer profiles produced in the upstream middle of the numerical domain. The figure compares the results with existing data measured in a wind tunnel. In the figure, the abscissa axis of the mean and the fluctuating velocity are non-dimensionalized by a characteristic velocity UL, and the ordinate axis of the vertical distance y is divided by the length scale of the cavity L. In addition, the mean velocity profile has the typical shape of the turbulent boundary layer, which has a minimum velocity value because of the wall friction and a gradual increase, resulting in a maximum velocity close to the top of the channel. As the proper turbulence models are provided, the overall comparison exhibits appropriate fit, and the numerical results are in agreement at x/L = -1. Conversely, turbulent intensity profiles close to the surface have different values that are estimated to be about 0.2 (k-ε model) and 0.13 (k-ω SST model). This difference in values may be caused by different wall models, such as the wall function for the standard k-ε model. That is, the k-ω SST model generally does not use the wall function, thereby producing a different shape. The turbulent intensity obtained from the solution to the RANS equation is defined as follows:

(10) . 3.2 Flow variation around the 2D and 3D cavities Fig. 7 shows the streamwise wind flow variation along several equispace locations of x/L = 0.0, 0.25, 0.5, 0.75, 1.0 in-

Fig. 8. Velocity distribution inside a cavity depending on the different turbulence models.

side and around the 2D and 3D trench cavities for the two turbulence models. The turbulent boundary layer flows from left to right, and the origin of the coordinate is located at x/L = 0.0 and y/L = 0.0. When it passes through the upper left edge of the cavities, wind flow experiences a rapid expansion around the corner such that it becomes highly unstable. The flow separation drives the free shear layer at the corner, propagates further downstream, and then reattaches at the other corner of the cavity. At this corner, the flow bifurcates in two paths, which is typical in flows passing through a channel with a cavity: one path for the entrainment and the other for the recirculation (also known as a feedback loop) inside the cavity. The velocity vector fields are displayed in Fig. 8, which illustrates the flow structure inside the cavity in detail. For a precise comparison between the turbulence models and the shapes of the cavity, all velocity vectors are given the same size to enable distinction of any unique flow. As discussed above, a separation flow that occurs in the left corner of the

2678


Fig. 10. Comparison of the pressure coefficient along the cavity with experimental results.

Fig. 9. Horizontal and vertical velocity distributions along vertical and horizontal centerlines.

cavity creates a large-scale recirculation flow in the middle. This flow also forms small wakes in each corner, which are technically called small-scale eddies. Depending on the turbulence model, these eddies have different strengths, and the corner vortex in the k-ω SST model appears at each corner. Meanwhile, the result using the k-ε model has relatively weak strength. In particular, the upper left part of the cavity has a range of flow separations. The separation in the sharp edge of the corner ought to be the physical phenomenon yielding the shear layer between the freestream and the cavity region. From the engineering perspective, such a separation in this sharp edge changes based on the Reynolds number. For example, no separation occurs at a low Reynolds number, whereas separation occurs at a critical Reynolds number. Previous scholars focused on flow instability around the upper left corner in a cavity ([23, 24]). Especially, Ref. [23] found a series of small-scale vortices depending on the Reynolds number. The implication of this finding is that the standard k-ε model would not be sufficient to calculate the small-scale vortex such as the flow around a corner. It would be a type of characteristic of turbulence modeling. However, the standard k-ε model is relatively unreliable for flows with a high mean shear rate or a rapid separation based on a high Reynolds number. Fig. 9 displays a simplified wind flow along a horizontal

and a vertical line in the middle of a cavity making a large clockwise circulation. In the figure, the horizontal line indicates a vertical wind velocity having a positive movement in the left part; negative values appear on the right. Similarly, the vertical line showing the streamwise velocity distorts to the reverse direction close to the bottom, but the wind speed of the upper region is increased substantially to become a wind speed in the outer region. In the figure, the streamwise velocity u and the vertical velocity v are non-dimensionalized by a characteristic streamwise velocity U0, where U0 is the horizontal velocity at x/L = 0.5 and y/L = 0. The shape of the profile is similar to that of a weather vane based on the center; the entrained flow from the main channel flow circulates inside the cavity. The standard k-ε model has an almost similar distribution regardless of whether the grids are 2D or 3D, whereas the k-ω SST model has a faster wind speed close to the wall surface in the 3D grid. Given the lack of experimental results, only a few related studies are available. One of the closest conditions is in the numerical simulation of Ref. [25]. They performed a lid-driven cavity flow via numerical simulation with the k-ω SST model. In most regions, the results are slightly different. However, the different Reynolds numbers (i.e., the Reynolds number in the current study is higher than that in Ref. [25]. by an order of 16) may imply a reasonable cause for the discrepancy. 3.3 Surface pressure distribution over cavities Fig. 10 displays a typical plot of a surface pressure coefficient (Cp) along the centerline with different turbulence models based on 2D and 3D trench cavities. In the figure, the geometric variable x’ of the abscissa denotes the parametric location along the centerline of cavities. For example, the leading edge is located at x’ = 0. Cp in this study is defined as (11)


where p0 is the reference pressure, ρ is the density, and uL is the flow velocity at the height of L from the wall. In the figure, the generated shear layer has its own flow instability and propagates downstream. As explained above, the separated flow from the leading edge of the cavity goes downstream and reaches the trailing edge in the corner (x/L = 1 and y/L = 0, i.e., downstream corner of the cavity). Thus, the region of the highest Cp occurs at the end of the downstream wall. The surface pressure along the centerline on the cavity has a wavy distribution. In the figure, the results are in generally strong agreement, but the surface pressure distribution around the corner and the bottom region is lower than that in the existing experiment. In addition, the 2D and 3D grid sizes of the standard k-ε model have a slight effect on the surface pressure variation. Meanwhile, the 3D grid of the k-ω SST model has a larger effect on the pressure around the corner of the cavity, showing small peaks in a local region that are not observed in the 2D case. In most of the regions, except for those downstream, the k-ε turbulence model underestimates the surface pressure but predicts a realizable distribution. Compared with the existing results, the predictions of the 3D k-ω SST model are better than those of the 2D k-ω SST model. Generally, the Cp from the k-ω SST model has a large discrepancy and a distorted shape around the corner. As described earlier, this section focuses on the observation of the small-scale vortex in the small confined region. This vortex is not usually observed in a RANS-type simulation, except for small-scale oriented calculations, such as LES and DNS. Therefore, the difference in surface pressure implies that a small-scale vortex exists around the corner under unsteady conditions. This vortex is not predictable by calculations under steady conditions. If the small-scale vortex stays in the corner, the surrounding pressure decreases as the local pressure inside the vortex drops. Therefore, the k-ω SST model has a higher pressure drop, which creates a wave shape. In addition, this effect causes more scattering and results in reduced predictability of the surface pressure. 3.4 Variation in turbulent kinetic energy and Reynolds stress The flow instability generated from the leading edge of the cavity propagates and magnifies downstream and finally creates a substantial change in energy after impinging on the trailing edge. Fig. 11 illustrates how the turbulent kinetic energy around the cavity is generated, propagated, and amplified. The top panel shows the propagation profiles of turbulent kinetic energy at equispace locations around the cavity. The middle panel shows the points of infection in each profile, which can indicate how energy would be propagated along the top region of the cavity. The width is defined as the distance of the inflection points between the upper and the lower range of y/L. The turbulent kinetic energy is initially the lowest; however, it gradually increases and then reaches a maximum value at around x/L = 0.9. When the flow hits the other edge of the cavity, the width decreases dramatically as the flow

2679

Fig. 11. Turbulent kinetic energy profile (top: overall profile, middle: inflection points) and non-dimensional width (bottom: Width/L).

becomes a type of impinging jet on the vertical wall. In the figure, the standard k-ε model predicts a larger energy distribution and an increase in the width of the inflection points. This difference is attributed to the energy of the k-ε model, which is almost twice as high as that from the k-ω SST model near the wall region. Reynolds stress ( u' v' ) represents the stress variation in a fluid caused by the random turbulent fluctuations in fluid momentum. It can be expressed as a combination of the strain rate of turbulent flow and turbulent viscosity νt and is described as follows:

.

(12)

Fig. 12 displays the contours of Reynolds stresses around 2D and 3D trench cavities depending on the turbulence models. The difference in turbulent kinetic energy creates substantial changes over the top region of the cavity. For the standard

2680


comparison with the experiments and the k-ω SST model, the 3D grid shows better results than the 2D grid on surface pressure around the cavity. (5) The difference in turbulent kinetic energy near the wall creates a substantial change over the top region of the cavity. The k-ε model predicts a larger energy distribution. In addition, the distribution of Reynolds stress is stable for the k-ε model, whereas the k-ω SST model shows an irregular distribution, and the location of the lowest Reynolds stress value is less distinct.

Acknowledgement

Fig. 12. Contour diagram of Reynolds stresses inside a cavity.

k-ε model, all distributions of Reynolds stress, depending on the 2D and 3D grids, appear stable, with the lowest being at the upper right (i.e., trailing edge). By contrast, the k-ω SST model shows an irregular distribution, and the location of the lowest Reynolds stress value is less distinct. A slight difference can be observed between the two turbulence models whereby the small-scale vortex stays in the corner. The k-ω SST model can predict this high Reynolds number flow effectively, whereas the k-ε model has a limited wall model, that is, wall function, such that the local pressure close to the corner increases.

4. Conclusions This paper presents the flow characteristics around 2D and 3D trench cavities using a typical two-equation-based numerical simulation. (1) Oncoming boundary layer profiles of mean velocity and turbulence quantities closely match the experimental data under a turbulent boundary layer. The inflow boundary conditions are sufficiently developed and similarly provided, but the turbulent intensity profiles close to the surface have a slight discrepancy depending on the turbulence models. (2) With a near-wall treatment, the k-ω SST model can simulate the small-scale flow around the corner of the cavity. In other words, the standard k-ε model would not be sufficient to calculate the small-scale vortex. (3) Surface pressure distribution around the cavity is generally in close agreement with existing experimental results, but the corner and bottom regions have lower values. The standard k-ε model has a slight effect on surface pressure variation, whereas the 3D grid of the k-ω SST model has a larger effect on the pressure around the corner of the cavity, showing small peaks in a local region that are not observed in the 2D case. (4) The standard k-ε model has an almost similar distribution regardless of whether the grid is 2D or 3D. Meanwhile, the k-ω SST model has different values of velocity, surface pressure, and Reynolds stress between 2D and 3D grinds. In a

This research was financially supported by the Ministry of Education, Science Technology and National Research Foundation of Korea through the Human Resource Training Project for Regional Innovation. This work was supported by Human Resources Development of the Korea Institute of Energy Technology Evaluation and Planning (grant funded by the Korea government Ministry of Knowledge Economy. (No. 20113020020010, 20114010203080).

References [1] A. Roshko, Some measurements of flow in a rectangular cutout, Naca Report No. TN-3488 (1955). [2] K. Krishnamurty, Acoustic radiation from two-dimensional rectangular cutouts in aerodynamic surfaces, NACA TN-3487 (1955). [3] H. G. Kim and V. C. Patel, Test of turbulence models for wind flow over terrain with separation and recirculation, Boundary-Layer Meteorology, 94 (2000) 5-21. [4] H. Kook and L. Mongeau, Analysis of the periodic pressure fluctuations induced by flow over a cavity, Journal of Sound and Vibration, 251 (5) (2002) 823-846. [5] E. S. P. So, A. T. Y. Chan and A. Y. T. Wong, Large-eddy simulations of wind flow and pollutant dispersion in a street canyon, Atmospheric environment, 39 (20) (2005) 35733582. [6] J. Summer, C. S. Watters and C. Masson, CFD in wind energy: the virtual, multiscale wind tunnel, Energies, 3 (5) (2010) 989-1013. [7] H. Heller and D. Bliss, Aerodynamically Induced Pressure Oscillationsin Cavities: Physical Mechanisms and Suppression Concepts, U.S AirForceFluid Dynamics Lab. AFFDLTR-73-133 (1975). [8] C. K. W. Tam and J. W. Block, On the tones and pressure oscillations induced by flow over rectangular cavities, J. Fluid Mech., 82 (2) (1978) 373-399. [9] N. Forestier, L. Jacquin and P. Geffoy, The mixing layer over a deepcavity at high-subsonic speed, J. Fluid Mech., 475 (2003) 101-145. [10] A. Y. D'yachenco, V. I. Terekhov and N. I. Yarygina,, Vortex formation and heat transfer in turbulent flow past a transverse cavity with inclined frontal and rear walls, Interna-


tional Journal of Heat and Mass Transfer, 51 (2008) 32753286. [11] W. Kang and H. J. Sung, Large-scale structures of turbulent flows over an open cavity, Journal of Fluids and Structures, 25 (2009) 1318-1333. [12] N. Murray, E. Sallstrom and L. Ukeiley, Properties of subsonic open cavity flow fields, Phys. Fluids, 21 (2009) 95-103. [13] C. Ozalp, A. Pinarbasi and B. Sahin, Experimental measurement of flow past cavities of different shapes, Exp. Therm. Fluid Sci., 34 (2010) 505-515. [14] H. Yao, R. K. Cooper and S. Raghunathan, Numerical simulation of incompressible Laminar flow over threedimensional rectangular cavities, J. Fluids Eng., 126 (2007) 919-927. [15] K. B. Shah and J. H. Ferziger, A fluid mechanicians view of wind engineering: Large eddy simulation of flow past a cubic obstacle, J. Wind Eng. and Ind. Aero. 67-68 (1997) 211-224. [16]E. Goncalves and R. F. Patella, Numerical simulation of cavitating flows with homogeneous models, Computers & Fluids, 38 (2009) 1682-1696. [17] H. C. Lim, T. G. Thomas and I. P. Castro, Flow around a cube in a turbulent boundary layer: LES and experiment, J. Wind Eng. Ind. Aero, 97 (2009) 96-109. [18] E. Goncalcves, Numerical study of unsteady turbulent cavitating flows, European Journal of Mechanics - B/Fluids, 30 (1) (2011) 26-40. [19] N. A. Kudryavtsev, Hydrodynamics and heat transfer of a transverse flow past a trench, in: Ext., Abstr. of Papers presented at VIII All-UnionSchool-Seminar Headed by Academician A. I. Leontev "Modern Problemsof Gas Dynamics and Heat and Mass Transfer and Ways of Improving ofthe Efficiency of Power Plants, Pt. 1, MGTU, Moscow (1991) 35-47. [20] ANSYS FLUENT Documentation version 12.1. (2009). [21] F. R. Menter, Influence of freestream values on k-ω turbulence model predictions, AIAA (1992). [22] F. R. Menter, Zonal two-equation k-ω turbulence model for

2681

aerodynamic flows, AIAA, (1993) 1993-2906. [23] E. Erturk, Discussions on driven cavity flow, International journal for Numerical Methods in Fluids, 60 (2009) 275-294. [24] E. Barragy and G. F. Carey, Stream function-vorticity driven cavity solutions using p finite elements, Computers and Fluids, 26 (1997) 453-468. [25] U. Ghia, K. N. Ghia and C. T. Shin, High-re solutions for incompressible flow using the Navier-Stokes equations and multigrid method, International journal for Numerical Methods in Fluids, 24 (1982) 477-492.

Young Tae Lee received his M.Sc. degree in 2009 and graduated from the School of Mechanical Engineering of Pu Kyong National University, Pusan, Korea, in 2009. He is currently a Ph.D. candidate at the School of Mechanical Engineering, Pusan National University. His major research field includes computational fluid dynamics development and energy prediction by wind turbines. Hee Chang Lim obtained his Bachelor of Science in Mechanical Engineering from the Department of Mechanical Engineering of Pusan National University. He completed his Msc and Ph.D. degrees in Thermo-Fluid Mechanics at the Department of Mechanical Engineering of Pohang University of Science and Technology. Since 2003, he has taken a Research Fellow position in the School of Engineering Sciences of the University of Southampton in the UK. In 2006, he returned to South Korea and took up a position of assistant professor in the School of Mechanical Engineering, Pusan National University, Pusan. He continues to develop his research interest in fluids dynamics, wind energy assessment, and wind turbine designs.