Step 1: Mesh

1.   Read the mesh file airfoil.msh.

File $\rightarrow$ Read $\rightarrow$ Mesh...

2.   Check the mesh.

General Check

   ANSYS FLUENT will perform various checks on the mesh and will report the progress in the console. Make sure that the reported minimum volume is a positive number.

3.   Examine the mesh (Figures  3.2 and 3.3).

Figure 3.2: The Entire Mesh

  Quadrilateral cells were used for this simple geometry because they can be stretched easily to account for different flow gradients in different directions. In the present case, the gradients normal to the airfoil wall are much greater than those tangent to the airfoil. Consequently, the cells near the surface have high aspect ratios. For geometries that are more difficult to mesh, it may be easier to create a hybrid mesh comprised of quadrilateral and triangular cells.

Figure 3.3: Magnified View of the Mesh Around the Airfoil

  A parabola was chosen to represent the far-field boundary because it has no discontinuities in slope, enabling the construction of a smooth mesh in the interior of the domain.

Extra:   You can use the right mouse button to probe for mesh information in the graphics window. If you click the right mouse button on any node in the mesh, information will be displayed in the ANSYS FLUENT console about the associated zone, including the name of the zone. This feature is especially useful when you have several zones of the same type and you want to distinguish between them quickly.

4.   Reorder the mesh.

Mesh $\rightarrow$ Reorder $\rightarrow$ Domain

  This is done to reduce the bandwidth of the cell neighbor number and to speed up the computations. This is especially important for large cases involving 1 million or more cells. The method used to reorder the domain is the Reverse Cuthill-McKee method.