# Preliminary Flutter Stability Assessment of the Double-Deck George Washington Bridge
## Appendix A RANS Simulations  
The finite element package ANSYS FLUENT was chosen both for meshing and simulating the fluid flow around the rigid body, with the aim of integrating the pressure distribution and finally obtain the steady-state aerodynamic coefficients. For each deck cross-section model, a 2D RANS simulation was performed. The \(k-\omega\)\(SST\) turbulence model, developed by [48], was adopted. This method consists in a sort of combination of the two simpler, widely used \(k-\varepsilon\) and \(k-\omega\) models, whose weighting is controlled by the wall distance. Both are two-equation models, whose differences can be summarized as follows: the \(k-\varepsilon\) model does not allow for a direct integration of the field equations through the boundary layer because the \(\varepsilon\) parameter tends to zero close to the wall. Conversely, the \(k-\omega\) model allows for directly integrating through the boundary layer, thus permitting to improve the goodness of the wall boundary layer unsteady-state solution, as demonstrated in [49]. As a drawback, the \(k-\omega\) model has proved to be highly sensitive to inlet turbulence boundary conditions: this can sensibly affect the solution even in large computational domains [48]. To overcome this drawback, the \(k-\omega\)\(SST\) model can conveniently be used. It preserves the main advantages of the classical \(k-\omega\) model, but it has proved to be less sensitive to the inlet conditions. After several tests regarding the turbulence model, the mesh sizing, the extension of the computational domain, and the boundary conditions, the following settings were adopted. Reference was made to [24; 37] as a guide. For what concerns the computational domain, the outer rectangle in Figure 11 delimits the fluid region, the left and right sides representing the velocity inlet and the pressure outlet, respectively. The dimensions of the computational domain were set following the indication in [24]: around 12\(B\) (360 m) in the along-wind direction and 5.5\(B\) (180 m) in the transverse one. The cross-section centroid is located at a horizontal distance of 120 m from the velocity inlet. The domain is subdivided into different regions as shown in Figure 11. The circle and the inner rectangle were created as auxiliary geometric entities so to allow for a differentiated meshing of the region closer to the obstacle and of the wind wake. The circle and the inner rectangle have radius and height equal to 35 m for the single deck model and 40 m for the double-deck. Being the dimensions of the two models rather similar, the same mesh size was set for both the single- and the double-deck versions. As for the mesh, in the inner regions, the mesh dimension ranges from an edge size of 1 cm (order \(B\times 10^{-3}\)) to a maximum size of 25 cm (order \(B\times 10^{-2}\)), with a growth ratio equal to 1.1 [24]. In the fluid region between the outer boundary and the inner parts, a maximum size of 3 m (order \(B\times 10^{-1}\)) and a growth ratio of 1.2 were set. A quadrilateral mesh was chosen for each model to favor convergence and, thus, reduce the computational time. Figure 11 shows an example of meshed model of the double-deck George Washington Bridge, with different zoom levels. Regarding the boundary conditions, the inlet was given a velocity of 30 m/s, a turbulent intensity of 0.5%, according to standard wind tunnel conditions for laminar flow, and a turbulent viscosity ratio equal to 2. The outlet was given a null pressure and the same turbulent intensity and viscosity as the inlet. The bridge deck edges were selected for the integration of the pressure distribution. The model parameters as the wind velocity, the chord length, and the air density were set so that dimensionless pressure coefficients were directly given by the program. Moment coefficients are referred to the upper deck centroid.