Preparing and Generating the Mesh

After assigning parts to regions and creating the interfaces, you can define the mesh settings for the volume mesh.

  1. For this simulation, the trimmed cell mesher is used in conjunction with the prism layer mesher to build a suitable mesh for the fluid volume. To set up and generate the volume mesh:
    1. Right-click the Geometry > Operations node and select New > Mesh > Automated Mesh.
    2. In the Create Automated Mesh Operation dialog:
      1. From the Parts list, select Surface Wrapper (All Parts).
      2. Within Select Meshers, select the following meshers in order:
        Group Mesher
        Surface Meshers Surface Remesher
        Core Volume Meshers Trimmed Cell Mesher
        Optional Boundary Layer Meshers Prism Layer Mesher
      3. Click OK.
    3. Rename the Automated Mesh node to Automated Mesh (Fluid).
    4. Select the Automated Mesh > Meshers > Trimmed Cell Mesher node and activate Perform Mesh Alignment.
    5. Edit the Automated Mesh (Fluid) > Default Controls node and set the following properties:
      Node Property Setting
      Base Size Value 0.025 m
      Prism Layer Controls Number of Prism Layers 4
      Prism Layer Stretching 1.3
      Prism Layer Total Thickness Size Type Relative to Base
      Percentage of Base 25
    6. Create a surface control for the fluid volume:
      1. Right-click the Geometry > Operations > Automated Mesh (Fluid) > Custom Controls node and select New > Surface Control.
      2. Select the Surface Control node and click the custom editor for Part Surfaces.
      3. In the Surface Control - Part Surfaces dialog, select Surface Wrapper (All Parts) > Fluid Volume and click OK.
      4. Edit the Surface Control node and set the custom control settings as shown below:
        Node Property Setting
        Controls
        Target Surface Size Target Surface Size Custom
        Minimum Surface Size Minimum Surface Size Custom
        Values
        Target Surface Size Size Type Relative to Base
        Percentage of Base 500
        Minimum Surface Size Size Type Relative to Base
        Percentage of Base 300
For the mesh inside the exhaust pipe, the polyhedral mesher is used in conjunction with the prism layer mesher.
  1. To define the volume mesh for the exhaust pipe:
    1. Right-click the Geometry > Operations node and select New > Mesh > Automated Mesh.
    2. In the Create Automated Mesh Operation dialog:
      1. From the Parts list, select Surface Wrapper (Exhaust).
      2. Within Select Meshers, select the following meshers in order:
        Group Mesher
        Surface Meshers Surface Remesher
        Core Volume Meshers Polyhedral Mesher
        Optional Boundary Layer Meshers Prism Layer Mesher
      3. Click OK.
    3. Rename the Automated Mesh node to Automated Mesh (Exhaust).
    4. Edit the Automated Mesh (Exhaust) > Default Controls node and set the following properties:
      Node Property Setting
      Base Size Value 0.02 m
      Number of Prism Layers Number of Prism Layers 4
      Prism Layer Stretching Prism Layer Stretching 1.3
      Prism Layer Total Thickness Size Type Relative to Base
      Percentage of Base 25
  2. Multi-select the Automated Mesh (Fluid) and Automated Mesh (Exhaust) nodes and set Mesher Execution Mode to Parallel.
For the attached shell parts, you define a shell mesh operation that generates a quadrilateral mesh.
  1. To define the mesh for the attached shell parts:
    1. Right-click the Geometry > Operations node and select New > Mesh > Automated Mesh (Shell).
    2. From the Parts list, select all the attached shells creator parts.
    3. Within Select Meshers, select the Quadrilateral Mesher.
    4. Click OK.
    5. Select the Geometry > Operations > Automated Mesh (Shell) > Default Controls > Base Size node and set Value to 0.02 m.
Now that all mesh settings are defined, you can generate the volume mesh.
  1. Click (Generate Volume Mesh) in the toolbar or select Generate Volume Mesh in the Mesh menu.

    The run and progress of the meshers are displayed in the Output window.

  2. To display the volume mesh, from the Vis toolbar, click (Create/Open Scenes) and select Mesh.
  3. Save the simulation.