## 2 Materials and Methods
### Computational Model  
The computational domain is defined by the interior air inside the ventilated air chamber with one inlet and one outlet opening. Three phases are necessary for the simulation of the computational model: Phase 1 involves the geometry of the computational domain, using the DESIGN MODEL software program of Ansys 2021 [32]. Phase 2 involves the meshing of the computational domain using the Meshing program [32]. Phase 3 involves the adjustment of computational parameters of the computational model, where the input parameters and output results are defined using the program Fluent [32].  
In Phase 1, all the geometries of the cases to be studied are generated, starting from the base geometry of case 0. After the geometry phase, the cases to be studied go to Meshing Phase 2; in this phase, a validation of the meshing is performed by comparing the results with 3 different meshes according to the GCI [33] method, choosing the mesh with the best computational accuracy-cost balance. The mesh used in the simulation is constructed from tetrahedral elements and increases in size from the walls towards the center of the air chamber. This type of mesh produces better convergence because there is a higher density of elements within the thermal boundary layer where the heat transfer coefficient is solved. To ensure the correct solution within the boundary layer, the nodes must be located within the viscous sublayer. Thus, the first element should be located at a maximum distance of 1 mm from the wall, and the growth rate towards the center of the enclosure should be between 10% and 15%. The parameter that controls the correct solution of the viscous sublayer is y+. In Figure 3, 3 meshes (coarse, medium, and fine) are compared as indicated by the GCI method where the (\(\dot{Q}\)) exchanged on the three meshes is monitored for 3 inlet velocities (0.5, 1.0, and 1.5 m/s). This figure shows that the medium mesh size provides better computational cost-accuracy.  
Phase 3 includes the configuration of the Fluent setup. In this phase, the following hypotheses and configurations are considered: (a) For the ideal gas, properties do not change with temperature and pressure. (b) The stationary regime is due to the low viscosity of the air and the short time it takes to cross the air chamber. (c) The gravity air buoyancy phenomenon is neglected; therefore, the heat exchange phenomenon is forced convection. (d) The floor temperatures are imposed, and the ceiling is considered adiabatic; therefore, radiation phenomena are not considered. (e) The inlet air temperature and velocity are known in all cases. (f) The outlet opening is considered as free flow with atmospheric pressure. (g) The types of equations used are the Navier-Stokes mass, momentum, and energy equations using the SIMPLE (Semi-Implicit Method for Pressure Linked Equations) numerical algorithm developed in [34]. (h) Another important aspect is the choice of the turbulence model; in the case of air with low viscosity, the k-\(\epsilon\)-type models show better results and convergence. Figure 4 shows the different turbulence models, where k-\(\epsilon\) with the \"enhanced wall treatment\" activation, controlling the y+ parameter close to 1, obtains better convergence and accuracy results in all simulated cases.  
Finally, the mass, momentum, and energy equations are solved iteratively for the corresponding boundary conditions using numerical methods until convergence is reached for the variables of interest (velocities, temperature, pressure, and wall heat flux). During the simulations of the different cases, a number of parameters must be controlled, such as, first, the residuals of the equations, which must about \(10^{-6}\), and, second, the heat flux in the floor. Convergence is achieved when a constant value is maintained for at least 1000 iterations. The number of iterations required for convergence is usually around 10,000 for all models.