Generating the Mesh

The construction of the volume mesh has a direct influence on how well Simcenter STAR-CCM+ simulates the fluid flow. It influences the rate of convergence and the accuracy of the final solution.

You define and generate the volume mesh using a parts-based mesh operation. Within the automated mesh operation, you select different meshers for the generation of the surface mesh, the volume mesh, and the prism layers.

The type of a boundary determines the default behavior for the prism layer mesher next to a boundary surface. For inflow, outflow, and symmetry boundaries, no prism layers are created by the prism layer mesher. Therefore, setting the boundary types before you generate a mesh saves time during setup.

To set the boundary types:
  1. Expand the Regions > [region] > Boundaries node.
  2. Select the [boundary] node and set Type to the appropriate boundary type. See the specific topics under Setting Boundary and Interface Conditions.
To set up the mesh:
  1. Create an automated mesh operation and select the mesh models:
    1. Right-click Geometry > Operations and select New > Mesh > Automated Mesh.
    2. In the Create Automated Mesh Operation dialog, select the respective geometry parts from the Parts list and, typically, select the following meshers:
      Group Box Model
      Surface Meshers
      • Surface Remesher—use the Surface Remesher to remesh the initial surface of the geometry.
      Core Volume Meshers One of:
      • Polyhedral Mesher—select this model for swirling flow and complex flow.
      • Trimmed Cell Mesher—select this model for uni-directional ducts or external flows with a prevalent flow direction. Whenever possible, align the mesh with the flow to improve accuracy and increase the rate of convergence.
      Optional Boundary Layer Meshers One of:
      • Prism Layer Mesher—select this mesher to add prismatic cell layers next to wall boundaries. Prismatic layers are important for resolving the boundary layer and the velocity gradient of the flow near the wall.
      • Advancing Layer Mesher (only if the Polyhedral Mesher is selected)—as the Prism Layer Mesher, this mesher adds prismatic cell layers next to wall boundaries. However, the Advancing Layer Mesher allows you to generate thicker, more uniform layers than the Prism Layer Mesher.
      For more information, see What Are the Differences Between the Advancing Layer and Prism Layer Meshers?
    3. Click OK.
  2. Set up mesh controls based on your geometry and flow characteristics:
    • Make sure that you use an adequate mesh resolution in areas where spatial gradients are high. Such areas occur when:
      • The mean flow changes rapidly. Examples: irrigation canals, vortex shedding, forced mixing, and atmospheric flows.
      • There are strong shear layers. Examples are: atmospheric flows, fluid jets, flows past solids, and flows with strong vorticity.
    • Refine the mesh downstream of a body as boundary layer separation causes unsteady and turbulent fluid phenomena. In external aerodynamic simulations, this separated region is known as the wake. For detailed instructions, see Mesh Refinement in a Wake.
    • Avoid creating a mesh that has excessive stretching in the direction normal to a wall. Keep cell aspect ratios as small as possible (for example, below 1000) to avoid convergence problems in the solver.
  3. (Optional) To extend the volume mesh beyond the original dimensions of the starting surface, create Surface Extruder and Volume Extruder operations. These operations are typically used to extend the solution domain at inlet or outlet boundaries with orthogonal extruded cells so that flow boundary conditions are set in positions of stable flow. For detailed instructions, see Extruding Surfaces from a Parts-Based Volume Mesh.
  4. Execute the mesh operations by clicking (Generate Volume Mesh) in the Mesh Generation toolbar.
  5. After the mesh operations complete, create a mesh scene to visualize the generated volume mesh.
For successively more accurate solutions, you can dynamically refine the mesh with respect to representative solution variables, such as Total Pressure. In Simcenter STAR-CCM+, you achieve successive refinement using Adaptive Mesh Refinement. For detailed instructions, see Adaptive Mesh General Workflow.

In order to make sure that simulation results are independent of the mesh, plan a mesh sensitivity study with two or more meshes after the first run.

For more information on mesh generation, see Meshing.