## 2 Parametric Study Based on CFD Calculations  
### Numerical Setup  
In order to obtain some of the main features of the MT, Computational Fluid Dynamic (CFD) techniques have been employed. Currently, non-commercial and proprietary CFD codes are used to reproduce relatively well any physical problem. In this work, the open source code OpenFOAM has been used for simulating the effects of a MT on a DU91W(2)250. This open source CFD code is an object-oriented library written in C++ to solve computational continuum mechanics problems. One of its advantages is that the user can modify the code to create new solvers and applications as well as freely share the code developed. The SIMPLE algorithm was employed for the pressure-velocity coupling. The convective terms were discretized with a second order linear-upwind scheme. The discretization of the viscous terms was achieved by means of a second order central-differences linear scheme. The simulations were run fully turbulent. Steady state simulations were carried out and performed with a structured finite-volume flow solver using Reynolds averaged Navier-Stokes (RANS) equations. For these computations the \(k\)-\(\omega\) SST shear stress turbulence model developed by [PERSON] [23] was used due to its superior separated flow performance, as reported by [PERSON] [24] and [PERSON] [25]. The model is a combination of two models: [PERSON]'s \(k\)-\(\omega\) model for near wall regions and the \(k\)-\(\varepsilon\) model for the outer region and in free shear flows. The SST model departs from existing \(k\)-\(\omega\) and \(k\)-\(\varepsilon\) models by way of a modified eddy viscosity definition that results in improved prediction of separated flows. Reynolds-averaged Navier-Stokes calculations with SST turbulence model for various tab configurations applied to an airfoil are presented in [PERSON] et al. [26]. Figure 2 illustrates the computational setup with the current setting consisting of a DU airfoil. An O-mesh type was designed for the computations with a computational domain radius of 32 times the airfoil chord length \(R=32c\), which is in the order of the computational size recommended by [PERSON] et al. [27] for this type of simulations. The Reynolds number based on the airfoil chord length of \(c=1\) m is Re = 7 \(\times\) 10\({}^{6}\). The computational setup of the simulations consists of a structured mesh with the first cell height \(\Delta z/c\) of 1.45 \(\times\) 10\({}^{-6}\) normalized by the airfoil chord length. The stretching in the chord-wise and normal directions is accomplished by double sided tanh stretching functions based on [PERSON] [28] and [PERSON] et al. [29]. The mesh domain was designed to have a dimensionless distance less than 1  
Figure 2: Computational domain. (\(y+<1\)) on the airfoil wall. An optimized mesh plays a major role in the CFD simulations as the tool that will help the user to discretize the domain. It is important to identify the mesh regions where the results have to be quite accurate as well as to establish a balance between the accuracy of the simulations and the computational cost. Figure 3 shows the cell distribution around the MT and in the near wake of the trailing edge. The wake and the regions where high gradients were expected were accordingly refined. There are certain regions close to the MT in which the velocity gradient changes drastically, which is the reason why those areas are so important. In OpenFoam, both the velocity and the pressure conditions have to be defined at all boundaries, since the velocity-pressure coupling is based on a collocated grid approach. Non-slip boundary condition was set for the airfoil and MT walls. Computational simulations of the DU91(2)250 airfoil without any MT have been carried out and validated against the data obtained by Xfoil from DOWEC project of [PERSON] et al. [30] and [PERSON] [31]. The Lift-to-drag ratio was calculated for ten angles of attack (AoA) from \(\alpha=0\) to \(\alpha=9\) degrees.