*3.2.2 Numerical simulation details*

The computational domain and boundary conditions are illustrated in **Figure 3**. The building model is scaled to 1/400 with dimensions of 180 mm (breadth) 60 mm (depth) 600 mm (height) and set as wall condition. The calculation domain covers the ranges of 20H in the streamwise direction, 16H in the crosswind direction and 8H in the vertical direction. In this study, the wind incident angle of 90 degree exactly corresponds to the side ratio case of 3:1, where the flow phenomenon is more complex.

The structured hexahedral grids were utilized to mesh the outer calculation domain, while for the inner region, an O-shaped grid with good orthogonality was employed. Additionally, local mesh refinement was performed near the building surface and wake region to better capture the significant features of the shear layer and recirculation zone. For example, 10 layers were imposed on the building wall to simulate the near-wall velocity gradient. The normal growth rate of the mesh within the boundary layer was 1.02, while for the grids was relatively far away from the external surface boundary, the growth rate was 1.1. To ensure y+ in the most region was around 1, the distance from the building wall to the center of the first layer was set as <sup>Δ</sup>y/B = 2.0 <sup>10</sup>–<sup>4</sup> . The mesh scheme and distributions around the building are illustrated in **Figure 4**.

**Figure 3.** *The boundary conditions of the computational domain for CWP and TWP.*

**Figure 4.**

*Mesh scheme and distributions around building: (a) perspective view of 3D mesh distribution; (b) side view of the local 2D mesh (y = 0); (c) top view of the local 2D mesh (z/H = 0.5).*

LES with the NSRFG-generated inflow boundary condition was adopted in this study to evaluate the effect of different wind profiles on a tall building. The numerical solver used herein is the commercial CFD code FLUENT. The finite volume method (FVM) was employed to solve the governing equations. SIMPLEC algorithm, initially proposed by [24], was adopted to solve the pressure–velocity coupling scheme. The convection and diffusion terms are discretized using the second-order upwind scheme. The temporal discretization scheme is the implicit time-stepping method. The time step in this paper was set as <sup>Δ</sup>*<sup>t</sup>* = 5 <sup>10</sup>–<sup>5</sup> to ensure the courant number in most calculation region is less than one.
