EFFECT OF THE TURBULENCE MODEL ON THE HEAT VENTILATION ANALYSIS IN A BOX PROTOTYPE

Investigations of the flow in a building system are crucial for understanding the fundamental basis of the aerodynamic structure characteristics. The CFD simulations were conducted using ANSYS Fluent 17.0 software, which solves the Navier-Stokes equations in conjunction with different turbulence models and by a finite volume discretization method. Particularly, a comparison between the experimental and standard k-ω, BSL k-ω, SST k-ω, standard k-ɛ, RNG k-ɛ and Realizable k-ɛ turbulence model has been developed. The comparison between the founded results affirms that the standard k-ω turbulence model is the most efficient to model the air flow in the present application. Indeed, the numerical results compared using the experimental data developed in the LASEM laboratory confirms the validity of the numerical method. The good agreements validate the considered computational method.


INTRODUCTION
Heat ventilation of buildings by solar energy is used for wide range applications, such as hospitals, residential and commercial buildings.
The mechanism of Heat ventilation has been investigated by many researchers.
In particular, Driss et al. [4] investigated thermal comfort evaluation and the heat ventilation in a living room. In others applications, Teodosiu et al. [7] presented experimental-numerical comparisons to give the precision of a CFD model. Du et al. [8] conducted experimental results measurements to present the characteristics of a Chinese house. Homod et al. [9] studied and proposed a new system by coupling reasons of internal conditions that are influenced by the outdoor environment. Terrados and Moreno [10] integrated the architectural concepts with energy efficient. Yasa [11] analysed the inside regions and the surrounding areas of education buildings and performed the microclimatic comfort. Premrov et al. [12] studied a single storey house wood frame case for objective to avoid the last energy. Johnston [13] predicted and measured performance of the building fabric in new build dwellings. Chan et al. [14] modeled a building of 21 floors by using Energy plus.
The results of simulations indicate that the apartments flat present satisfactory periods for the environment. Ibrahim et al. [15] planned technical coating projection. The proposed mathematical model was compared with experimental results. Nam and Chae [16] developed an optimal design of the grounding by using a numerical method. Alam et al. [17] improves a method of releasing heat from the building to reduce the energy demand of the building in a tropical environment. Rode [18] illustrated global relations to highlight the building performance. Han et al. [19] investigated hybrid solar energy system.
A general view of the architectural envelope designs and innovative system was presented. Watson [20] reviewed design quality research on buildings in relation to users. Sailor et al. [21] describe the system use implications that lead to building energy of green roof design decisions. From these different anterior works, it has been noted that the design of buildings based on the reduction of the energy consumed. For thus, we have involved the study of the heat ventilation in a box prototype (living room).
Particularly, we have considered the turbulence models effect to choose the most effective model.
The numerical results obtained in this work were validated via a living room realized in the LASEM laboratory.

BOX PROTOTYPE SYSTEM
Figure 1 depicts the physical domain of the box prototype (living room). The gravity direction in the system is gives as The box is characterized by a 0.22 m of height, 0.2 m of width and 0.3 m of length. Both square holes are localized at the same wall of the box.
It has the same edge which equal to 0.02 m, while it has different distance from the bottom wall of the box. The down hole is situated with a distance equal to h1=0.05 m from the bottom wall, which used to receive the air flow coming from the outside of the box prototype. However, the top hole is responsible to the evacuation of the air flow from the box to the surrounding air [1]. It is situated from the box base with a distance equal to h2=0.18 m.

Boundary conditions
The applied boundary conditions of the considered system are shown in figure 2.
In the first hole, the heat flow supplies the box prototype from the outside air heater, where the velocity inlet and the temperature are equal respectively to V=3.4 m.s -1 and T=310 K. After that, the air flow is evacuated from the second hole of the box prototypes, where the outlet pressure is equal to p=101325 Pa.
The others side surfaces of the box prototype are assumed as walls surrounding the computational domain.
In these surfaces, Dirichlet boundary conditions are imposed and admit these values V=0 m.s -1 and T=290 K.

Meshing
The meshing is an amportant step in the simulation procudure which affect directly the accuracy of the computantional findings. Then a meshing analysis is required to minimize the error calculation.
In the present study, the employed mesh density is taken from an aterior meshing analysis [22] which is compared different meshing cases with our experimental data.
The meshing choice is based on both accuracy and calculation time [23]. Figure 3 shows a view of the used optimal mesh with a tetrahedral volume cells. The 3D computantional domain is caractirezed by 167400 cells and 64312 nodes.

Numerical model
The considered governing equations are the momentum equations, the energy equation and finally the continuity equation [24][25][26].
Taking a time average yields in the instantaneous equations, the Reynolds-averaged Navier-Stokes (RANS) equations can be written as follows: To close equation (2), these Reynolds stresses ' ' j i u u  − must be modeled by using the Boussinesq hypothesis, written as follows: The energy equation is expressed as follows: Where k is the thermal conductivity and E is the total energy.
The standard model k- is modeling by both transport equations of the turbulent kinetic energy k and its dissipation rate . These equations are obtained from the following expressions: t  is the turbulent viscosity computed from the combination of k and  : In these conditions, we have to write: The difference between the RNG and the standard k- models consists in the addition of this term: Where: As other k- models, the turbulent viscosity is calculated as follows: The difference between the realizable k-, the standard k- and the RNG k- models consists on the calculation of  C , as  C is: Table 1.c illustrates the different constants employed in the realizable k-ɛ model. In the k-ω standard model, the transport equations of the specific dissipation rate ω and the turbulent kinetic energy k and are written as follows:

CHOICE OF THE TURBULENCE MODEL
The effect of the turbulence model on the numerical results have been studied in this section in order to achieve the adequate model.
In fact, different turbulence models were studied using the software " Ansys Fluent 17.0" for solving the governing equations.
Particularly, we have compared the BSL k-ω turbulence model, the standard k-ω turbulence model, the standard k-ɛ turbulence model, the SST k-ω turbulence model, the Realizable k-ɛ turbulence model and the RNG k-ɛ turbulence model.
We found that the numerical results are in good agreement with the experimental data (the velocity profile) which confirms the validity of the numerical method.
In the viewed direction, in the viewed direction, set by the intersection of the two planes x=0.06 m and z=-0.005 m, the superposition of the experimental results with the velocity profiles for the different turbulence models is presented in figure 4.
According to these results, that the same profiles of the velocity have been observed and the values take down of the turbulence model. Particularly, it has been observed that the value founded with the experimental data is nearest to the standard k-ω tubulence model results.
This study tends to show that the standard k-ω turbulence model is the most efficient to model the air flow in the present application. Therefore, the overall error designed between the numerical and the experimental data is equal to 5%.

RESULTS AND DISCUSSION
The distribution of the velocity fields, the temperature, the total pressure, the turbulent kinetic energy and the turbulent viscosity are studied in this section.
In the present study, the employed Reynolds number is equal to Re=5100.

Velocity fields
The distribution of the velocity fields in the plane defined by x=0.06 m is shown in figure 5 for the different studied turbulence models. results, it has been observed a discharge zone at the box inlet hole in all cases with average velocity equal to V=3.4 m.s -1 . The inlet flow barge into the reverse wall of the box and then it moves inside the box with a turbulent behavior to evacuate through the top hole. Otherwise, both axial directions of the airflow are seen inside the box. The recirculation zone appeared in the whole area of the box is created by the change of the flow direction, specially by the first ascending flow. Meanwhile, the weak zone showed in the down area of the box is created by the second descending flow.
In these conditions, the averaged velocity presents a very low value in the whole system when exclude the values in the discharge area which reached V=1.3 m.s -1 . The comparison between the different turbulence models affirms that the choice of the adequate model presents a straight effect on the velocity fields. Particularly, it is noticed that the recirculation zone has been involved by the turbulence model choice. In this situation, the maximum value of the averaged velocity is obtained for the SST k-ω turbulence model and it reachs V=4.75 m.s -1 . However, the minimum value is founded for the standard k-ɛ turbulence model and it reachs V=4.42 m.s -1 .

Temperature
The distribution of the air temperature at t=2 s and in the plane defined by x=0.06 m is shown in figure 6 for the considered turbulence models.
According to these results, it has been observed that the temperature at the hole inlet is equal to T=310 K while, it slightly decreases in the discharge area, at the hole inlet.
However, the temperature decreases above the discharge area due to the recirculation region appeared into the whole area of the box prototype.
Otherwise, the air temperature decreases gradually to reaches the minimum values at the system outlet with a value equal to T=290 K.
The comparison between the founded results affirms that the choice of the turbulence model presents a straight effect on the temperature distribution.
Particularly, it has been noted that the minimum value of the temperature is obtained in the hole outlet for the BSL k-ω turbulence model and it is equal to T=290.8 K. However, the maximum value of the temperature reaches T=291.5 K for the SST k-ω turbulence model. Figure 7 shows the distribution of the total pressure in the plane defined by x=0.06 m for all considered turbulence models. From these results, it is clear that a compression zone is appears in the down hole of the box prototype for all cases. In fact, the total pressure decreases delicately in the expulsion area, produced from the system inlet and attacked until the reverse wall of the box. This reality can be clarified by the recirculation zone showed at the whole area of the box prototype.

Total pressure
From that point onward, the total pressure increases to reaches the peak value at the opposite wall.
However, a depression zone is appearing at the top hole in the system outlet for all cases.
A comparison between the different turbulence models gives that the turbulence model presents a straight effect on the distribution of the total pressure. In fact, it has been noted that the maximum value of the total pressure is founded for the standard k-ω and the SST k-ω turbulence models and presents a value equal to p=101342 Pa.
This value decreases slightly for the other turbulence models and reaches the minimum value equal to p=101340 Pa, for the standard k-ɛ turbulence model.  Figure 8 depicts the distribution of the turbulent kinetic energy in the plane defined by x=0.06 m, for the considered turbulence models. From these results, it can be seen that the turbulent kinetic energy presents a small value at the system inlet. In mean time, the turbulent kinetic energy increases gradually in the expulsion area which created in the down hole of the box. Otherwise, it has been observed that the maximum turbulent kinetic energy appears at the discharge area near the reverse wall and at the top hole at the box outlet.

Turbulent kinetic energy
As causes the other air proprieties, this fact is owing to the recirculation zone in the whole area of the box. Comparatively, the distribution of the turbulent kinetic energy in the four considered turbulence models affirms that the turbulence model presents a straight effect on the distribution of the turbulent kinetic energy. In fact, it has been observed that the maximum value of the turbulent kinetic energy is obtained in the hole outlet for the BSL k-ω turbulence model and it reaches k=1.258 m 2 .s -2 . However, this value reaches a low value, which is about k=0.226 m 2 .s -2 , for the SST k-ω turbulence model.  Figure 9 shows the distribution of the turbulent viscosity in the plane defined by x=0.06 m and for the four turbulence models. According to these results, it can be seen that the turbulent viscosity presents a small value at the box inlet for all cases. However, the turbulent viscosity roses at the expulsion area which shown in the down hole of the system. The maximum values of the turbulent viscosity appear in the discharge area near the reverse wall. Otherwise, a peak values appear at the top hole of the box prototype due to the recirculation zone of the hot air in this region.

Turbulent viscosity
Comparatively, it has been observed a small effect of different studied models on the distribution of the turbulent viscosity. In fact, the extension of the wake zone distinctiveness of the maximum values of the turbulent viscosity, obtained in the discharge area near the reverse wall, is more developed for the BSL k-ω turbulence model. Using this model, the maximum value of the turbulent viscosity reaches t=0.00192 kg.m -1 .s -1 in the hole outlet. However, this parameter presents a low value equal to t=0.00032 kg.m -1 .s -1 for the RNG k-ɛ turbulence model in the discharge area. In this case, the turbulent viscosity continues to decrease immensely in the outlet hole.

CONCLUSION
The present paper aims to investigate the impact of the turbulent model on the heat ventilation was studied in a box prototype equipped with a solar system. Particularly, a computational study and an experimental validation have been developed to compare the standard k-ω, the SST k-ω, the BSL kω, the standard k-ɛ, the Realizable k-ɛ turbulence the RNG k-ɛ and the model. From the obtained results, it is noticed that the aerodynamic characteristics presents the same emergence nevertheless the maximum values depend on the turbulence model. Particularly, it has been noted that the value founded with the standard k-ω tubulence model is nearest to the experimental data. This study tends to show that the standard k-ω turbulence model is the most efficient model to analyze the air flow in the box prototype. In the prospect, we suggest to extend this application with others geometrical arrangements.