## 2 Numerical Setup  
CFD simulations were carried out in the present study to investigate and understand the development of the primary vortex generated by VGs. The vortex generated by a single vortex generator (VG) was simulated by the OpenFOAM open-source code. OpenFOAM is a library written in C++ that allows the manipulation and development of numerical solvers for problems of continuum mechanics. One of the main advantages of this noncommercial CFD code is that it can be improved and tailored to reproduce different physical phenomena depending on user interests. A semi-implicit method for pressure-linked equations (SIMPLE) algorithm wasn applied for turbulent, steady-state, and incompressible flow solving the Reynolds average Navier-Stokes (RANS) equations. With the purpose of speeding up the convergence process, a potentialFoam solver was used to initialize the fields. This solver is appropriate to set initial conditions for the next step when a more advanced solver is applied. After that, a simpleFoam solver was used for solving RANS equations, and the turbulence model used in the present study was the \(k\)-\(\omega\) shear-stress transport (SST) turbulence model presented by [PERSON] [30]. Two transport equations were solved by this turbulence model, the one for the turbulent kinematic energy \(k\) and the specific dissipation \(\omega\). The used computational technique was justified on the steady Reynolds average Navier-Stokes (RANS) simulations made by [PERSON] et al. [31] for a single VG in a flat plate for two incident angles computed with OVERFLOW, a code developed by the National Aeronautics and Space Administration (NASA). These simulations were compared to experimentally obtained data, resulting on a good agreement for CFD results except for short distances downstream of the VG. In that study, the streamwise peak vorticity and vortex trajectory were better predicted by the shear-stress transport (SST) compared to the Spalart-Allmaras (SA) turbulence model. Second order discretization schemes were employed regarding the numerical schemes, following similar studies developed by [PERSON] et al. [17]. The computational setup consists of a flat plate with a single VG whose leading edge (LE) is placed at 10.25 m from the inlet boundary, see Figure 1. This passive device consists of a rectangular vane with a length twice its height (H), which varies to make possible the parametric study. The normalization of the domain is done with respect to the conventional VG height (H); this height is equal to the boundary layer thickness \(\delta=0.25\) m at the leading edge (LE) of the VG. Different boundary conditions have been set for the domain limits. According to [PERSON] et al. [23], the ceiling and the two lateral sides were set as slip conditions. Additionally, nonslip conditions were set for the vane and flat plate surfaces, while the upstream part of the domain was specified as inflow conditions with prescribed velocity according to the undisturbed velocity. The downstream part was set as an outlet assuming a fully developed flow. The strategy carried out to save computational cost was to divide the mesh in blocks because the cell density in the mesh is different in order to capture more accurate results in those places where the vortex is generated, around and downstream of the VG. Each block has a particular stretching factor in the three spatial coordinates, as shown in Figure 2.  
Two types of structured meshes in the computational domain were designed according to the different VG heights used for the parametric study. A first mesh with around 12 million hexaedral cells and 64 blocks for the 0.2H and 0.4H VG height cases, and a second mesh sized 11 million hexaedral cells and 44 blocks for the other three VG height cases were used with a normalized height of the closest cell to the wall of \(\frac{\Delta y}{\delta}\ =\ 1.5\times 10^{-6}\). Both meshes have a block-based structure and are divided in regions which allow a different grid resolution.