## 2 Materials and Methods
### Numerical Simulation  
The present study makes extensive use of the CFD method in the study of the flows generated by the general ventilation system, the PV system, and the thermal plumes of the heated manikins. Numerical study was carried out in Ansys Fluent. Calculations were performed using a double-precision pressure-based coupled solver. To solve the turbulent flow, a RANS approach was chosen. To simulate natural convection, a relatively large density of cells for the fluid domain mesh had to be used near solid surfaces and in the field. Additionally, the low velocities in the climatic chamber implied low values for \(y+\) when using a robust mesh in term of spent computational resources. These considerations imposed a low-Re turbulence model. Thus, the \(k\)-\(\omega\) SST was adopted for all performed numerical simulations [53; 54; 55; 56]. The gradients were computed using a least-square cell-based method. Second-order discretization schemes were used for pressure, momentum, and energy equations, while for turbulence quantities, first-order upwind schemes were chosen. To initialize the flow field, a standard method was set. To ensure better convergence in the first steps, the whole fluid domain was patched using a low-velocity value along the Y axis (in the opposite direction of the gravity force) and a temperature value close to the equilibrium value measured during the experimental tests. The mesh consists of 8 million mixed 3D poly-hexcore cells with polygonal 2D cells on the solid surfaces. Near the solid surfaces, to correctly capture the velocity and temperature variation in the boundary layer, 10 layers of prismatic cells were grown using a constant aspect ratio equal to 10 for the first cells near the walls. To ensure an optimal distribution of cells in the fluid domain, different characteristic lengths were used for different zones. The characteristic dimensions of the cells are detailed in Table 1. Values were chosen considering a previous study [57] so that the grid would correctly capture the experimentally determined temperature and velocity fields and satisfy the requirements imposed by the numerical model with respect to \(y+\) values near the solid surfaces. To avoid large leaps between cells, a growth rate of 1.1 was used, except in the boundary layer zone, where a growth rate of 1.2 was applied. Additionally, in the hexcore zone, to avoid 1:8 cell jumps, the transition regions from hex cells with different characteristic lengths were filled with polyhedral cells. For simulations in which a PV system was considered, a rectangular zone with dimensions of \(5D_{e}\times 2D_{e}\times 2D_{e}\) was refined so that the influence of the PV jet could be better captured. The maximum characteristic length in this region was equal to 0.5 cm. Within this zone, another rectangular region was defined, wherein the mesh was refined so that the cell length was equal to 0.25 cm. Figure 6 presents details of the mesh, and Figure 7 illustrates the distributions of \(y+\) values on the manikins and seats surfaces. The maximum wall \(y+\) value was 2, ranging from 0.29 to 2 on the surface of the manikins and seats [58]. Temperature-boundary conditions on solid surfaces and inlets are detailed in Table 2. A schematic related to the surface-temperature values of the virtual manikins is presented in Figure 8.