## 2 Materials and Methods
### CFD Model  
The CFD model is developed using Ansys Fluent 15.0 software package (provided by Ansys, Canonsburg, PA, USA). Theoretical and practical considerations regarding CFD modeling can be consulted in [35]. The main elements of the developed CFD model in this paper are presented as follows. * Geometry: based on the design plans, the three-dimensional (3D) geometry of the station was built, respecting all the details related to the interior construction elements (e.g., resistance pillars, interior stairs, railings, elevator, etc. ), as shown in Figure 9. It should be noted that the defined geometry represents a 1:1 full scale model. * Computational domain discretization: finite volumes--unstructured mesh, based on tetrahedral elements. The mesh was refined in the following regions (using local sizing discretization functions): near the circular diffusers of the station ventilation system (Figure 10), area close to the air exhaust devices of the UPE system, area adjacent to the fire outbreak, and nearby the subway rails. Figure 8: Ventilation emergency operating mode in the subway station. It is worth mentioning that thorough studies were performed in order to obtain the grid independent solutions, considering three meshes with 10 million, 14 million, and 18 million elements (obtained using different settings for local mesh controls, e.g., \"growth rate\" [36]: 1.20 for 10 million mesh, 1.18 for 14 million mesh, and 1.14 for 18 million mesh). These three meshes were analyzed by comparing air velocity in a cross section through the fire outbreak (Figure 11). The results show that the velocity field for the coarser mesh is totally different (with much higher air velocities) from those for the other two (refined) meshes, while the differences between 14 million mesh and 18 million mesh are minimal. Consequently, the discretization with 14 million elements (exact number: 14,164,713 cells) was employed to perform the study. * Turbulence modeling: \"standard k-\(\varepsilon\) two-equation model\" [37], with values for the model constants according to [PERSON] and [PERSON] [37]. This approach was successfully used in analogous numerical studies [38; 39; 40; 31]. In addition, [PERSON] et al. [41], in a review article covering over 50 CFD numerical studies, concluded that the k-\(\varepsilon\) turbulence model is the most widely used for air flow modeling in subway networks (stations and tunnels). Moreover, the need for computational resources is reduced for the standard k-\(\varepsilon\) two-equation model compared to other turbulence models with two or more additional equations. This is even more important in the case of our configuration, with a very large computational domain and unsteady simulations. * Near wall treatment of the flow: \"standard wall functions\" [37], as the aim of this study is not to predict in detail the air flow in the boundary layers. In addition, the choice of a more complex model (which would better capture the influences of the walls on the air flow) would have required a denser discretization, which would also have led to higher Central Processing Unit (CPU) usage [42]. On the other hand, the approach based on \"standard wall functions\" requires specific conditions concerning the discretization near the solid borders, related to the distance between the near-wall cell centroid and the wall. The acceptable distance for the valid use of \"standard wall functions\" in the case of wall-bounded turbulent flows is judged by means of y+,  
Figure 10: Refined mesh near the circular diffusers of the station ventilation system. Figure 9: Subway station geometry in the numerical model. which represents a non-dimensional distance, defined in the same manner as the local Reynolds number:  
\[y^{+}=\frac{U_{\tau}y}{\
u} \tag{1}\]  
where U\({}_{\tau}\)--friction velocity at the nearest wall, y--distance to the nearest wall, and \(\
u\)--local kinematic viscosity of the fluid.