### 6.3.3. Grid Generation

In a CFD analysis, the flow domain is subdivided in a large number of computational cells. All these computational cells together form the so-called mesh or grid. The number of cells in the mesh should be taken sufficiently large, such that an adequate resolution is obtained for the representation of the geometry of the flow domain and the expected flow phenomena in this domain.

A good mesh quality is essential for performing a good CFD analysis. Therefore, assessment of the mesh quality before performing a large and complex CFD analysis is very important. Most of the mesh generators and CFD solvers offer the possibility of checking the mesh on several cells or mesh parameters, such as aspect ratio, internal angle, face warpage, right handiness, negative volumes, cracks, and tetrahedral quality. The reader is referred to the user's guides of the various mesh generators and CFD solvers for more information on these cells and mesh parameters.

Recommendations for grid generation are:

- Avoid high grid stretching ratios.

  - Aspect ratios should not be larger than 20 to 50 in regions away from the boundary.

  - Aspect ratios may be larger than that in unimportant regions.

  - Aspect ratios may, and should, be larger than that in the boundary layers. For well resolved boundary layers at high Re numbers, the near-wall aspect ratios can be of the order of 105-106.

- Avoid jumps in grid density.

  - Growth factors should be smaller than 1.3.

- Avoid poor grid angles.

- Avoid non-scalable grid topologies. Non-scalable topologies can occur in block-structured grids and are characterized by a deterioration of grid quality under grid refinement.

- Avoid non-orthogonal, for example, unstructured tetrahedral meshes, in (thin) boundary layers.

- Use a finer and more regular grid in critical regions, for example, regions with high gradients or large changes such as shocks.

- Avoid the presence of arbitrary grid interfaces, mesh refinements, or changes in element types in critical regions. An arbitrary grid interface occurs when there is no one-to-one correspondence between the cell faces on both sides of a common interface, between adjacent mesh parts.

If possible, determine the size of the cells adjacent to wall boundaries where turbulence models are used, before grid generation has started.

Numerical diffusion is high when computational cells are created that are not orthogonal to the fluid flow. If possible, avoid computational cells that are not orthogonal to the fluid flow.

Judge the mesh quality by using the possibilities offered by the mesh generator. Most mesh generators offer checks on mesh parameters, such as aspect ratio, internal angle, face warpage, right handiness, negative volumes, cracks, and tetrahedral quality.

It should be demonstrated that the final result of the calculations is independent of the grid that is used. This is usually done by comparison of the results of calculations on grids with different grid sizes.

Some CFD methods enable the application of grid adaptation procedures. In these methods, the grid is refined in critical regions (high truncation errors, large solution gradients, and so on). In these methods, the selection of appropriate indicator functions for the adaptation is essential for the success of the simulations. They should be based on the most important flow features to be computed.

As a general rule, any important shear layer in the flow (boundary layer, mixing layer, free jets, wakes, and so on) should be resolved with at least 10 nodes normal to the layer. This is a very challenging requirement that often requires the use of grids that are aligned with the shear layers.

Release 18.2 - © ANSYS, Inc. All rights reserved.