## 2 Materials and Methods
### Computational Fluid Dynamics (CFD) Simulation
\[U=U_{ref}\left(\frac{y}{H}\right)^{0.16} \tag{1}\]  
Another important thing is the modelling of the atmospheric turbulence caused by the urban canopy layer, which causes an increase in the fluid turbulence changing the airflow pattern. To model this in Fluent, a parameter named aerodynamic roughness length (z\({}_{0}\)) can be used [50] which is an empirical parameter proposed by some authors to mathematically model the roughness of typical landscape configurations for numerical studies. With this, the turbulence created by the city skyline can be modelled and used in CFD simulations. For this research, a value of z\({}_{0}\) = 0.1 m is considered enough to recreate the city roughness. Moreover, the boundary conditions used in the simulation are listed in Table 3.  
Finally, the configuration of Fluent environment is also very important, as it determines how the simulation is solved. The most suitable turbulent model is needed to obtain the most realistic solution. In this case, the RANS k-\(\epsilon\) equation using Re-Normalisation Groupt (RNG) closure scheme and standard wall function seems to be the most appropriate one when studying the fluid dynamics of flow across the urban canopy layer according to authors [51]. To solve these equations, some inherent parameters of Fluent environment must be chosen: \(\{C_{c1},\ C_{c2},\ C_{c},\
u_{0},\ \beta\}=\{1.42\,;1.68,\ 0.0845;4.38;\ 0.012\}\)[52]. Finishing the configuration, the SIMPLE scheme is used to solve the coupled equations of pressure and velocity, with least squares cell-based discretization scheme for the gradient. Additionally, a second-order discretization upwind is selected for all the magnitudes to achieve better accuracy. The convergence criterion used to stop the simulation is setting all the residuals value to \(1^{-5}\). When this condition is met, the iterative process finishes, and the result is considered converged. When the simulation is carried out, some results will be obtained. Firstly, the pressure coefficient is calculated in four points of the left-wing part of the dwelling and then the pressure difference between the windward and leeward part of the upper floor is obtained with (2), where \(\rho\) is the density of the fluid, \(\Delta Cp\) is the difference of pressure coefficients between the points mentioned before. This way is found the direction of the flow and the magnitude of the pressure difference which will cause the cross-ventilation inside the floor. \[\Delta P=\Delta Cp*0.5*\rho*V_{ref}^{2} \tag{2}\]  
Furthermore, the flow streamlines are represented and the mass flow rate entering the courtyard is calculated, which gives an illustrative numerical result for the air renewal inside the courtyard. When all the results have been obtained, the second part of the decoupled method begins. Firstly, the 2D geometry model of the left-wing upper floor is completed, including \begin{table}
\begin{tabular}{c c} \hline \hline
**Zone** & **Boundary Condition** \\ \hline Inlet & Velocity Inlet. \\  & x-Velocity \(U=V_{ref}\left(\frac{y}{H}\right)^{0.16}\) \\ Outlet & Pressure Outlet \\ Far Field & Symmetry \\ Upstream & Wall. Roughness: C\({}_{5}\) = 1; z\({}_{0}\) = 0.1 m \\ Downstream & Wall, no slip condition \\ Walls & Wall, no slip condition \\ \hline \hline \end{tabular}
\end{table} 
Table 3: Boundary conditions for full model simulation. both rooms which face towards the street and the corridor with windows connected to the courtyard. For this purpose, the dimensions of the walls, doors and windows are the same as in the floor plan provided (Figure 14). Regarding the meshing, in this case, every zone of the model is equally important, so a cell mesh size of 0.2 m is used everywhere. In this simulation, a distinction between types of walls is considered because of their thermal properties.