THREE-DIMENSIONAL SIMULATION OF A TURBULENT FLOW AROUND A TAPERED CUBE DUG IN THE MIDDLE

To analyze the influence of the tapered form of the two upper vertices of a rectangular cube placed in a channel and the impact of the insertion of hollow in the center of the obstacle, a three-dimensional study was executed using K-ω SST turbulence model. Different models of the form of the cube were presented to examine the features of the flow with a Reynolds number Re=4×104. The turbulence kinetic energy, 2D and 3D time-averaged streamlines, trace-lines, streamwise velocity profiles, pressure profiles were obtained using the ANSYS CFX calculation code and the finite volume method were employed for resolving the governing equations. The streamlines showed in the model of the tapered cube with hollow a formation of another vortex downstream of the cube at the outlet of the hollow. For the streamwise velocity, there are two recirculation zones: one logarithmic zone due to the main flow, the other is a lower parabolic return zone due to the recirculation vortex.


INTRODUCTION
The study of atmospheric pollution around buildings has become a necessity given the even increase in the rate of pollution in cities [1]. This pollution becomes very dangerous for the health of the inhabitants especially if it remains stagnated and blocked by the buildings. For several years now, many experimental and more recently numerical studies have concentrated on the understanding of complex flows around various more or less profiled models. This type of flow is generally found in many industrial applications, such as the cooling of electronic components [2], atmospheric flows around buildings [3], fins of turbomachines, etc. Several studies have been carried out on the application of flows around obstacles, Hussein and Martinuzzi [4] presented an experimental study of a three-dimensional circulation in the canal which contains a cube. The results show that the development of the turbulence dissipation rate from the recirculation zone to the asymptotic slip. Martunizzi and al. [5] studied the flow around obstacles prismatic with different aspect ratios using the techniques of crystal violet display, oil film, and laser. The results showed a nominally two-dimensional region exists behind the obstacle and upstream of the recirculation zone. Hwang and Yang [6] have carried out a numerical study on swirl (vortex) structures around a cube inside a canal. They found out that the number of vortices increased as the Reynolds number raised. Filippini et al. [7] investigated the instance of the current around cubes placed into a channel, using the Large Eddy Simulation (LES) model. The results obtained showed that when the ratio S/H increases, the average drag coefficient augments for the second cube while it remains approximately constant for the first one. Chang Lim et al. [8] and Krajnovi'c et al. [9] provide using the standard Large Eddy Simulation (LES) model a numerical simulation of the flow around an area contains cube, inside in a turbulent boundary layer, and comparing with experimentation. In the same approach, Dan Gu et al. [10] and Becker et al. [11] to study the structure of the flow around three-dimensional obstacles, an experimental simulation has been presented using different aspect ratios, in two different types of boundary layers. The experimental results showed that the flow structure around the obstacle depends on its aspect ratio, the angle of attack, Reynolds number, and type of boundary layer. Yakhot et al. [12] presented a study of flow around a cube mounted surface with Direct Numerical Simulation (DNS) for a Reynolds number Re=5160 by using the immersed boundary method. The results support to employ immersed-boundary methods for simulating complex turbulent flows. Rostane et al [13] studied the impact of the curvature of the below edge of a block inside in the canal on aerodynamic phenomena, in particular, the vortex behind the cube. The authors studied the influence of three radius of curvature R = 0.2H, R = 0.3H and R = 0.5H, for Re = 10 5 . They concluded that the dimensions of the vortex downstream of the obstacle decrease by decreasing the radius of curvature. Sari-hassoun et al [14] studied the influence of the curved shape of the lover's edge of a rectangular obstacle. They compared two obstacle models using a qualitative approach, where they analyzed the dimensions of the recirculation zones, the velocity field, and the kinetic energy and dissipation. Aliane et al. [15] Performed a numeric analysis of flow around a block placed in a rectangular channel, using two models of obstacles: a rectangular cube, and the other rectangular with upstream round edge. The turbulence model used was kε. Salim et al [16] studied an approach to treat turbulent flows on a surface-mounted cube using the y + wall as a guide to select the appropriate grid pattern and corresponding turbulence models. They used the Fluent calculation code. The study is divided into two parts: the first part and the second part, deal respectively with the low and high Reynolds number. Heguehoug et al [17] presented a study of turbulent flow, stationary, three-dimensional, incompressible, and without heat transfer around an isolated 3D profile and through a series of 60 blades constituting a fixed wheel similar to that of a turbo machine. Merahi et al. [18] have contributed to the study of stationary three-dimensional flow and incompressible through a cascade of dawn by a digital simulation based on the k-ε model, and it was concluded that losses due to the change in the angle of incidence are considered to be the main cause of the decline in of turbo machinery. Amraoui and Aliane [19] presented the study of fluid flow and heat transfer in a solar flat plate collector by using Computational Fluid Dynamics (CFD) which reduces time and cost. Sercan et al. [20] investigated the flow characteristics around a surface-mounted cube at Re=3700 in terms of Computational Fluid Dynamics (CFD) and then compared with experimental results using three different models of turbulence. Kanfoudi et al. [21] large eddy simulation (LES) have been employed to present a numerical analysis of the turbulent flow structure induced by the Cavitation Shedding. Djeddi et al [22], have simulated a viscous fluid flow on an unconventional diamond-shaped obstacle in a confined channel is simulated in low to moderate Reynolds numbers. The diamond-shaped obstacle is geometrically modified to represent different blocking coefficients depending on the height of the channel and different aspect ratios based on the length /height ratios of the obstacle. The simulations are divided into two stationary and unsteady flow groups. Liakos et al. [23] performed a Direct Numerical Simulation (DNS) of steady-state laminar flow over a cube at Reynolds numbers ranging from 1-2000 based on the cube height. In the same work, Diaz-Daniel et al. [24] presented a Direct Numerical Simulations (DNS) of a wall-attached cube immersed in laminar and turbulent boundary layers at various Reynolds numbers ReH ranging from 500 to 3000. Additionally, Sumner et al. ( [25], [26]) assessed the effect of the aspect ratio and the incidence angle of the flow above the free end of a surface-mounted finite cylinder and finite-height square prism and Siddhesh Shinde et al. [27] presented a large-eddy simulation of flow over a wall-mounted cube-shaped obstacle placed in a spatially evolving boundary layer in order to understanding how variations in the cube height h modify the flow dynamics for the situation where the cube is within the boundary layer. M. Ennouri et al. [28] studied the modeling and simulation of the flow inside a centrifugal pump through non-cavitation and cavitation conditions using an SST-SAS turbulence model. Sari-hassoun et al [29] affected an experimental study of flat plate air solar collector. The conclusion obtained was that the air temperature at the outlet was different from that inside the collector. M. Bayareh and A. Nourbakhsh [30] studied the effect of different geometries of inner and outer tube surfaces on heat transfer of a double pipe heat exchanger is studied. Two-equation standard κ-ε turbulence model is used to model the turbulent flow. Simulations are done for different cases include convex, concave and smooth surfaces for inner and outer tubes at different Reynolds numbers. Results show that the maximum heat transfer corresponds to the convex-concave case in comparison with the smoothsmooth one.
To examine the influence of the tapered form of the two upper peaks and the impact of the hollow in the middle of the obstacle to check the detachment length, the structures of the vortex, the recirculation zone, threedimensional simulation of flow around a cube inside a horizontal channel has been carried out. Three different models of the cube (simple cube, tapered cube, a tapered cube with hollow) were processed to execute this.

MATHEMATICAL MODEL
Averaged equations of conservation of mass, momentum, energy, and Reynolds are: • The mass conservation equation • Reynolds Equations (4) The turbulence model used in this study was the K-ω SST (Shear Stress Transport) model of Menter [31] is derived from the Standard k-ω model [32]. This model combines the robustness and accuracy of the formulation of the k-ω model in the near-wall region with the k-ε model [33] and all its types for the free flow away from the wall.
The definition of the turbulent viscosity is modified to take into account the transport of turbulent shear stresses.
The formulation of the two-equation model is: The blend function F1 is defined by: Here y is the distance to the nearest wall. In the near-wall region, 1=1, while it goes to zero in the outer region is given as: Eddy viscosity is given by The second blending function is defined by: To prevent the accumulation of turbulence stagnation regions, limited production was used: The model constants are calculated using the mixing function F1: The values of the model constants are: The k-w SST model is mainly recommended for applications such as fluids undergoing sudden changes in stress, flowing in curved surfaces or cases of boundary layer separation, so is the perfect model for our simulation.

MODEL DESCRIPTION AND COMPUTATIONAL DOMAIN
The obstacle used in our problem studied (Fig.1) represents a cube that has tapered upstream and downstream edges, mounted inside a horizontal channel of length (L) and height (h). (Fig. 2) To obtain a better precision of the results, it is necessary to generate a mesh well refined. It opted for a structured hexahedral mesh in our case using calculation code ANSYS CFX. Fig.4 shows the grid of the mesh used.

Boundary conditions
Since the flow is turbulent, the model of turbulence k-w SST was chosen to analyze the problem more precisely. All "walls" are adiabatic and have no-slip conditions. According to the models selected previously, equations had to be solved using the following factors: The incoming flow velocity U0 corresponds to Reynolds number Re=4×10 4 (Re=U0.h/ν) and the channel height (h). The height of the obstacle is H=25 mm and the channel height is h=2H. The velocity is zero u=0m/s near the lower and upper walls of the channel and above the obstacle. The pressure at the outlet Pout=0. The boundary conditions of the problem treated are given as follows, as shown in Fig.3:   Figure1. Model of the body (3D view)

RESULTS AND DISCUSSION
An initial study of the grid independence was executed by a serial of test simulation in the computational domain corresponds to the velocity. For this, Many meshing sizes were tested (Fig.5) to ensure the grid independence of results, including 685020, 865274 and 987100 hexahedral elements. The values in Table.1 indicate the properties at x /H= 0.5. This study proves that there are comparatively low differences between the three grids. The mesh size of (865274) was chosen as the best solution between precision and calculation time.    X/H=-0.5 X/H=0.5 X/H=1.5 X/H=1 Figure 5. The grid sensitivity The study of the influence of the tapered form of the two upper peaks and the insertion of a hollow in the middle of a rectangular cube has been examined. A three-dimensional study was carried out using the ANSYS CFX calculation code. Turbulence model K-ω SST has been employed to examine the features of the around the inclined cube at Reynolds number Re=4×10 4 . The turbulence kinetic energy, 2D and 3D time-averaged streamline on the symmetry plane (z=0) and at the floor of the channel, streamwise velocity profiles, trace-lines around the cube have been presented.
The variation of contours of the turbulent kinetic energy in the symmetry plane (z = 0) for various block models (simple cube, tapered cube and tapered cube with hollow) is illustrated in fig.7. It is observed that this energy is maximum and higher downstream of the simple cube, and at the outing of the hollow, it is minimal and almost zero at the tapered edges of the cube. It can be noted that the quantity of turbulent kinetic energy is stronger in the simple cube.  For accurate flow analysis and for a good vision of separations and re-attachments on the top of, at the lateral sides and behind the obstacle of the obstacle, the time-averaged streamlines on the symmetry plane and at the floor of the channel for various form of the cube (simple cube, tapered cube and tapered cube with hollow) at Reynolds number Re = 4×10 4 were presented in (Fig.8) and (Fig.9). In (Fig.8), in the three different configurations, there is a small vortex upstream of the obstacle. Downstream of the cube, we observe the formation of a wide vortex.
In the case of a tapered dug cube, the vortex emerging from the hollow forms a complex structure and is pen chanting down by the force of the jet. A part of the fluid remains blocked in the region between the tapered upstream edge and the bottom wall of the channel, and above it, the separation is triggered; it is caused by the upstream stopping point of the obstacle which is achieved. Figure.9 and 10 show the 2D and 3D streamlines at the floor of the channel, the blocking effect of the obstacle creates an unfavorable pressure gradient that separates the flow and moves away from the cube, forming a horseshoe vortex. For all forms of the cube, the horseshoe vortex appears upstream and bypasses the obstacle. On the other hand, there is two focus (F), one saddle (S), separation (S) and reattachment (R) point achieved for all configurations that are likewise appearing in the study of R. Martinuzzi and C. Tropea [5]. We note that for the horseshoe the width of the wake is greater in the case of a hollowed-out cube and smaller in the case of the tapered cube.     (12-16) illustrated the velocity profiles (streamwise) at the symmetry plane (z=0) and different line positions (x/H=-0.5, 0.5, 1, 1.5 and 2) respectively upstream, above and downstream the obstacle. The range y/H is the meantime 0≤y/H≤2 for all positions except for the position x/H=0.5 where 1≤y/H≤2. For the 5 configurations, there are two recirculation zones: one logarithmic zone due to the main flow, the other is a lower parabolic return zone due to the recirculation vortex. For the first position, upstream the cube (x/H=-0 .5), we observe that the 3 profiles are almost identical; except close to the wall, we note that of the tapered dug cube is larger than the others. In the case (x/H=0.5), the velocity profile for the simple cube is greater than the other cases which are uniform. In the middle of the block (x/H=1), the stream wises of the two forms (tapered cube and tapered cube with hollow) are identical from y/H=1, at the lower end of this value, there is a sharp increase in the axial velocity and this is because it is at the level of the flow inside the cube (in the hollow) and we note that the span of the curve for the tapered cube is larger. Downstream the cube (x/h=1.5), we can see two distinct zones, above and below y / H = 1. Above y / H = 1, we note that the velocity profiles for the tapered cube and the tapered cube with hollow are the same and their profiles are smaller than the simple cube, but below the value y / H = 1, we observe that the profile of the simple cube and the tapered cube are identical and are smaller than that of the tapered cube with hollow, and we note an abrupt increase in velocity, this is due to the injection at the level close to the hollow. For figure.16, the velocity profiles for the simple cube and the tapered cube are almost identical, so the profile of the tapered cube with hollow is wider. A presentation of the numerical results of pressure profiles in the direction of flow for three different cube models in the plane of symmetry is given in Figure 17 at the position x / H = 2 m (after the obstacle). The value of the pressure reaches the maximum value of 450 Pa for the simple cube model, and because of this, the pressure is higher in the simple cube than the others. Besides, the axial pressure decreases sharply because it is located at the level of the flow located behind the cube (exit of the hollow).
It is found that the loss of pressure is relatively low for the case of the obstacle models of the tapered cube and the tapered cube with hollow. On the other hand, this loss of pressure is quite important for the case of the simple cube model.

CONCLUSION
The problem treated in this work is a three-dimensional simulation using the ANSYS CFX calculation code to carry out a three-dimensional numerical simulation of turbulent flow around an obstacle with three different forms (simple cube, a cube with two upper vertices, and tapered dug cube). The flow characteristics of the surface-mounted cube as a function of the Reynolds number of Re = 4×10 4 have studied with k-ω SST turbulence model. This study has allowed a 3D simulation to analyze and understand some important physical aspects. In this type of flow, especially we tried to emphasize the role of the presence of obstacles in the channel, the distribution of dynamic and thermal exchanges. The analysis of simulation results confirms that: The quantity of turbulent kinetic energy is stronger in the simple cube. The streamline figures proved the texture of the vortices around the different forms of the block, there appeared three vortices upstream, above and downstream of the obstacle. In the model of the tapered cube with hollow; there was the formation of another vortex downstream of the cube at the outlet of the hollow. For the streamwise velocity, there are two recirculation zones: one logarithmic zone due to the main flow, the other is a lower parabolic return zone due to the recirculation vortex. We find that the loss of pressure is relatively low for the case of the obstacle models of the tapered cube and the tapered cube with hollow. On the other hand, this loss of pressure is quite important for the case of the simple cube model.