Selecting the Mesh Models

For this type of simulation, the quality of the result depends to a large extent on how successful the mesh is at capturing features of the flow around the propeller.

In this simulation, you use the trimmer mesh model for the rotating region and its surroundings. The static region surrounding the shaft is meshed using the extruder mesher as this minimizes the computational costs.

An important criteria to consider when choosing mesh sizes is the wall y+ value. In general, you are advised to keep the wall y+ values outside the buffer layer, that is values from 5 to 30. In this tutorial, you aim for wall y+ values greater than 30.

The meshing strategy adopted in this tutorial adheres to the Parts-Based Meshing (PBM) approach. This meshing strategy executes a pipeline of mesh operations on geometry parts; hence, you can modify an input part and the changes are propagated through the pipeline to the volume mesh. The extruder mesh also forms part of the pipeline operations.

To create the automated mesh operation:
  1. Right-click the Geometry > Operations node and select New > Mesh > Automated Mesh.
  2. In the Create Automated Mesh Operation dialog, select Parts > Rotating Region and Static Region.
  3. Activate the following meshing models:
    Group box Model
    Surface Meshers Surface Remesher
    Core Volume Meshers Trimmed Cell Mesher
    Optional Boundary Layer Meshers Prism Layer Mesher
  4. Click OK.
To set the controls for the operation:
  1. Select the Operations > Automated Mesh node and activate Per-Part Meshing.
  2. Select the Automated Mesh > Meshers > Trimmed Cell Mesher node and activate Perform Mesh Alignment.