[ANSYS, Inc. Logo] return to home search
next up previous contents index

6.2.2 Mesh Quality

The quality of the mesh plays a significant role in the accuracy and stability of the numerical computation. The attributes associated with mesh quality are node point distribution, smoothness, and skewness.

Regardless of the type of mesh used in your domain, checking the quality of your mesh is essential. Depending on the cell types in the mesh (tetrahedral, hexahedral, polyhedral, etc.), different quality criteria are evaluated:

The aspect ratio is a measure of the stretching of a cell. It is computed as the ratio of the maximum value to the minimum value of any of the following distances: the distances between the cell centroid and face centroids, and the distances between the cell centroid and nodes. For a unit cube (see Figure  6.2.2), the maximum distance is 0.866, and the minimum distance is 0.5, so the aspect ratio is 1.732. This type of definition can be applied on any type of mesh, including polyhedral.

Figure 6.2.2: Calculating the Aspect Ratio for a Unit Cube

To check the quality of your mesh, you can use the Report Quality button in the General task page:

figure General figure Report Quality

A message will be printed to the console. The example below provides an example of the output.

Applying quality criteria for tetrahedra/mixed cells.
Maximum cell squish =  4.61001e-001
Maximum cell skewness =  4.48776e-001
Maximum aspect ratio =  5.23830e+000

Node Density and Clustering

Since you are discretely defining a continuous domain, the degree to which the salient features of the flow (such as shear layers, separated regions, shock waves, boundary layers, and mixing zones) are resolved , depends on the density and distribution of nodes in the mesh. In many cases, poor resolution in critical regions can dramatically alter the flow characteristics. For example, the prediction of separation due to an adverse pressure gradient depends heavily on the resolution of the boundary layer upstream of the point of separation.

Resolution of the boundary layer (i.e., mesh spacing near walls) also plays a significant role in the accuracy of the computed wall shear stress and heat transfer coefficient . This is particularly true in laminar flows where the mesh adjacent to the wall should obey

 y_p \sqrt{\frac{u_{\infty}}{\nu x}} \;\;\; \leq \;\;\; 1 (6.2-1)

where $y_p$ = distance to the wall from the adjacent cell centroid
  $u_{\infty}$ = free-stream velocity
  $\nu$ = kinematic viscosity of the fluid
  $x$ = distance along the wall from the starting point of the boundary layer

Equation  6.2-1 is based upon the Blasius solution for laminar flow over a flat plate at zero incidence [ 69].

Proper resolution of the mesh for turbulent flows is also very important. Due to the strong interaction of the mean flow and turbulence, the numerical results for turbulent flows tend to be more susceptible to mesh dependency than those for laminar flows. In the near-wall region, different mesh resolutions are required depending on the near-wall model being used. See Section  12.3 for guidelines.

In general, no flow passage should be represented by fewer than 5 cells. Most cases will require many more cells to adequately resolve the passage. In regions of large gradients, as in shear layers or mixing zones, the mesh should be fine enough to minimize the change in the flow variables from cell to cell. Unfortunately, it is very difficult to determine the locations of important flow features in advance. Moreover, the mesh resolution in most complicated 3D flow fields will be constrained by CPU time and computer resource limitations (i.e., memory and disk space). Although accuracy increases with larger meshes, the CPU and memory requirements to compute the solution and postprocess the results also increase. Solution-adaptive mesh refinement can be used to increase and/or decrease mesh density based on the evolving flow field, and thus provides the potential for more economical use of grid points (and hence reduced time and resource requirements). See Chapter  27 for information on solution adaption.


Truncation error is the difference between the partial derivatives in the governing equations and their discrete approximations. Rapid changes in cell volume between adjacent cells translate into larger truncation errors. ANSYS FLUENT provides the capability to improve the smoothness by refining the mesh based on the change in cell volume or the gradient of cell volume. For information on refining the mesh based on change in cell volume. (See Sections  27.3 and  27.7).

Cell Shape

The shape of the cell (including its skewness, aspect ratio, and squish) also has a significant impact on the accuracy of the numerical solution.

Flow-Field Dependency

The effect of resolution, smoothness, and cell shape on the accuracy and stability of the solution process is dependent on the flow field being simulated. For example, very skewed cells can be tolerated in benign flow regions, but can be very damaging in regions with strong flow gradients.

Since the locations of strong flow gradients generally cannot be determined a priori, you should strive to achieve a high-quality mesh over the entire flow domain.

next up previous contents index Previous: 6.2.1 Geometry/Mesh Requirements
Up: 6.2 Mesh Requirements and
Next: 6.3 Mesh Import
Release 12.0 © ANSYS, Inc. 2009-01-29