The basic components of the manual meshing process are examining and repairing the surface mesh, creating an initial mesh, refining the mesh, and improving the mesh.
The following steps describe the recommended meshing procedure.
The first step in the mesh generation process is to examine the validity and quality of the surface mesh. The recommended approach includes the following steps:
Checking for free and isolated nodes (see Free and Isolated Nodes).
Checking and improving the surface mesh quality (see Improving Boundary Surfaces).
Visually examining the surface mesh for free, multiply-connected, skewed, and/or close-proximity faces (see Displaying the Mesh).
Making local repairs if required (see Modifying the Boundary Mesh).
After obtaining a valid, (ideally) high-quality surface mesh, you can proceed to create the volume mesh.
The first step in generating the volume mesh is creating the initial mesh. This process first creates a pre-meshed box encompassing the entire geometry, and then sequentially introduces each boundary node into the mesh. As the nodes of a boundary face are inserted into the mesh, any necessary mesh modifications needed to insert the face are performed, effectively inserting both boundary nodes and faces into the mesh simultaneously. For more information see Initializing the Tetrahedral Mesh.
Activating Multiple Zones (for Multi-zone Meshes Only)
If the mesh has multiple regions (for example, the problem requires a fluid zone and one or more solid zones), you can refine the mesh using refinement parameters specific to individual zones, if required. The procedure for meshing multiple cell zones includes the following steps:
Initialize the mesh.
Activate the appropriate zones using the Manage Cell Zones dialog box.
Set the zone-specific refinement parameters and refine the active zones.
If you want to mesh all the zones included in the mesh with the same refinement parameters, modify the Non-Fluid Type in the Tet dialog box.
Select the appropriate type from the Non-Fluid Type drop-down list in the Tet Zones group box in the Tet dialog box.
Important: By default, the Non-Fluid Type is set to dead as the mesh is assumed to consist of a single fluid region and one or more dead regions. The active zone is considered to be the fluid zone and only this fluid zone will be considered for refinement during the automatic meshing process.
When the Non-Fluid Type is set to a type other than dead (for example, solid), all the zones will be active after the initialization is complete. Hence, all the zones will be considered for refinement. If required, you can change the zone type using the Manage Cell Zones dialog box.
Note: For zone-based meshing, if any cell zone has at least one boundary zone type as inlet, it will automatically be set to fluid type. For object based meshing, volume region type is used to determine the cell zone type.
You will refine the initial mesh by adding cells at the boundary and in the interior. The refinement methods available are the skewness-based method and the advancing front method. You can also define local refinement regions using the Tet Refinement Region dialog box. You can modify the parameters in the Refinement tab of the Tet dialog box and select additional refinement options for skewness-based refinement in the Tet Refine Controls dialog box, if required.
You can improve the skewness by smoothing, swapping, and refining the mesh further to improve the quality of the volume mesh. At any point in the mesh generation process, you can compute and plot the cell skewness distribution using the Cell Distribution dialog box. The number of cells in the specified range in each of the regularly spaced partitions is displayed in a histogram format. The x axis shows either the size or the quality and the y axis gives the number of cells or the percentage of the total. This will give you an idea of the improvement required. It is typically possible to reduce skewness to 0.8–0.85 (for simple geometries) or 0.9–0.95 (for more complex geometries).
Note: If you have used domains to generate the mesh or group zones for reporting (as described in Using Domains to Group and Mesh Boundary Faces), you can report the cell distribution only for those cell zones that are in the active domain.
Step 4a: Swapping and Smoothing without Refining
Swapping and smoothing improve the mesh by manipulating the nodes and faces without increasing the total number of cells. Refinement, on the other hand, improves the mesh by adding nodes, which typically increases the number of cells. To get the best possible mesh with the minimum number of cells, perform only smoothing and swapping before refining the mesh any further.
Smoothing repositions interior nodes to lower the maximum skewness of the mesh. For swapping, given n+2 nodes in dimension n, there are at most two triangulations of the nodes depending on the configuration of the nodes. In cases where two triangulations exist, the two alternatives are examined, and the one that has the lowest maximum skewness is selected. Smoothing and swapping are automatically performed to improve the mesh when the Improve Mesh option is enabled in the Refinement tab of the Tet dialog box.
Refer to Smoothing Nodes and Swapping for details on improving the mesh by swapping and smoothing.
You can further refine the cells in the active zones by changing parameters such as Max Cell Volume, and Max Cell Skew and Max Boundary Cell Skew (available only for skewness-based refinement).
Important: Changing mesh size controls other than Max Cell Volume will have no effect on a mesh that has already been refined. Alternately, use local refinement regions. Refer to Using Local Refinement Regions for details.
Refining with skewness parameters reduced to values less than 0.5 will rarely improve the mesh and will be very time-consuming.
Important: Do not over-refine the mesh, the volume mesh produced should be of sufficient density to resolve the shape and any intuitive flow features (for example, wall boundary layers). Additional resolution can be more effectively produced using the solution-adaptive mesh capability provided in the solution mode in Fluent.
At this step you will have an acceptable mesh for most geometries.
Step 4c: Boundary Slivers and Other Sources of Lingering High Skewness
When viewing the cell distribution plot, if you find that there are a few cells with very high skewness, check to see where they are located (that is, on the boundary or in the interior). To do so, use the Report Boundary Cell Limits dialog box. When using that dialog box, note that if you have used domains to generate the mesh or group zones for reporting (as described in Using Domains to Group and Mesh Boundary Faces), the report will apply only to the active domain.
Refer to Removing Slivers from a Tetrahedral Mesh and Moving Nodes for details on removing slivers and other mesh improvement options.
You can initialize and refine the tetrahedral mesh in a single step by clicking the button in the Tet dialog box after setting the appropriate parameters in the Initialization and Refinement tabs. Alternatively, you can set the appropriate parameters in the Initialization tab and click the button to create the initial mesh. You can then refine the initial mesh by setting the appropriate parameters in the Refinement tab and clicking the button.
If you need to refine a particular region, you can define the region to be refined using the Tet Refinement Region dialog box.