## 6 Adaptive Wing CFD Model  
In this section, a simulation model must be designed and meshed for CFD calculations. The first step consists of the design of the geometry of the adaptive wing prototype in Figure 20 and that of the wind tunnel, as shown in Figure 3 in CATIA V5. The second consists of the geometries meshing using structured and unstructured mesh sizes on the model's surface, and the last step is the use of CFD solver to find the lift and drag forces [34]. A robust mesh model of the adaptive wing prototype was designed using an ANSYS ICEM mesh generator. The mesh volume of these two objects consists of a finite number of polygons composed of triangle and quad elements. Quad polygons have a better topology (how the polygons are connected to the flow around them) and a better resolution of the flow boundary conditions. For a wind tunnel CFD model, there are five boundary conditions that must be specified during the mesh design, and as well as in the CFD Solver: (i) the \"inlet boundary condition\", which is the surface where the flow is initiated, mainly when the flow speed in one of the axes (\(x\), \(y\), \(z\)) is specified; (ii) the \"outlet boundary condition\", which is the region where the flow attains a fully developed state and where no change in velocity or direction occurs far from the model disturbances; (iii) the \"wall boundary condition\", which defines the appropriate flow condition near the walls (inside the wind tunnel test chamber and at the surface of the model); (iv) the \"Constant pressure boundary conditions\", which are used when the inlet pressure is known and when the outlet pressure can be determined; in an open circuit wind tunnel, the outlet pressure is the atmospheric pressure; and (v) the \"symmetric boundary condition\", which is calculated when the same physical conditions exist on two sides of a model. The designed CADs (step files) of the adaptive wing prototype and of the wind tunnel were imported to the ANSYS ICEM meshing software. The meshing process includes the (i) design of an initial mesh, followed by an evaluation of its quality and the boundary conditions specifications; (ii) the improvement and repairing of the mesh holes, discontinuities, and space between its cells; (iii) the generation of the volume mesh using triangle and quad elements and the refining of the mesh density close to its boundary layer; and (iv) the exportation of the final mesh to the CFD solver. A mesh with an optimum grid resolution had to be refined along the model's surface. The fluid at the wing model surface, named \"Inner_fluid\", and the flow inside the wind tunnel have to be simulated together. The generated grids have coarse regions, and it was achieved using the octree method with \"Tetra Cell\". It was re-meshed using the Delaunay refinement mesh technique. The octree method allows the design of regular internal mesh geometry and does not require an initial mesh to be implemented. The Delaunay technique allows for a smoother mesh and a better accuracy in representing complex shapes. Figure 20: CFD model of the adaptive wing prototype. A \"grid sensitivity\" study was conducted to determine the mesh density required to produce final results of acceptable fidelity. Grids of varying resolution were tested using the flight test number 22 (leading edge at \(-5^{\circ}\) and trailing edge at \(-10^{\circ}\)), the angle of attack of \(3^{\circ}\), and the Reynolds number of 5.89 \(\times\)\(10^{5}\), corresponding to a flow velocity of U = 30.10 m/s. The wall parameter y\({}^{+}\) < 1 was maintained regardless of the tested grid [35]. The variations of \(C_{l}\), \(C_{d}\) and \(C_{l}/C_{d}\) are shown in Table 7. It can be observed that the results change significantly for the first three grid resolutions (Grid 1, 2, and 3); after the fourth and fifth grid resolutions (Grid 4 and 5), the mesh density does not significantly affect the results of the aerodynamics coefficients.