Mesh: Setting Up the Simulation Domain and Selecting the Meshers

Prepare the regions for the simulation domain and select the meshers.

Begin by creating the regions:

  1. Launch Simcenter STAR-CCM+ and load foundationTutorial_7.sim.

    You can either use the sim file that you saved from the previous tutorial, or load the sim file provided in the tutorials bundle. See Downloading the Tutorial Files from the Support Center Portal.

  2. Save the simulation as foundationTutorial_8.sim.
  3. Create the regions from the geometry parts:
    1. If the geometry scene is not open, double-click the Scenes > Geometry Scene 1 node.
    2. Expand the Geometry > Parts node.
    3. Select the Rotating Region and Static Region nodes.
    4. Right-click on a selection and choose Assign Parts to Regions....
    5. In the Assign Parts to Regions dialog, select:
      1. Create a Region for Each Part
      2. Create a Boundary for Each Part Surface
      3. Create Contact-mode Interfaces From Contacts
      4. Click Apply then Close.
      The geometry in the scene changes to a dark gray color to show that parts displayed in the scene are assigned to regions. Parts that have no region association are displayed in a light gray color.
  4. Create an automated mesh operation and select the mesh models:
    1. Right-click the Geometry > Operations node and select New > Mesh > Automated Mesh.
    2. In the Create Automated Mesh Operation dialog:
      1. Select Rotating Region and Static Regon from the Parts list.
      2. Select the following meshers, in order:
        Group Mesher
        Surface Meshers Surface Remesher
        Core Volume Meshers Polyhedral Mesher
        Optional Boundary Layer Meshers Prism Layer Mesher
      The Surface Remesher retriangulates the surface of the geometry and improves the overall quality of the initial surface. The Polyhedral Mesher generates polyhedral cells that are suitable for turbulent and swirling flow simulations. The Prism Layer Mesher generates a prism layer (orthogonal prismatic cells) next to wall surfaces or boundaries. Prism layer cells are important for resolving the boundary layer and the velocity gradient of the flow near surface.
    3. Click OK.
    An automated mesh operation, Automated Mesh, is added to the Operations node. The mesh models that you select are located inside this operation under the Meshers node.
  5. Set up the mesh parameters:
    1. Expand the Operations > Automated Mesh > Default Controls node.
      The global mesh parameters are located under this node.
    2. Select Base Size and set Value to 2 mm.
      The base size is the reference length for all reference size controls. Using the value that you specify in the base size, you can scale the mesh using relative size controls as a percentage of the base size, or set these controls independently using absolute values. Typically you set the base size to the scale of the object of interest, in this tutorial this is the fan blades in the graphics card.
    3. Select the Target Surface Size node, select Relative to Base and set Percentage of Base to 1000 in the Properties Window.
      The target surface size is set as a percentage of the base size and specifies the cell size that the meshers should aim for when generating the mesh. The target size can be smaller or larger than the base size, and you can use it to grow or shrink the cells in the mesh.
    4. Select the Minimum Surface Size node, select Relative to Base and set Percentage of Base to 50 in the Properties Window.
      The minimum surface size specifies the smallest element size that the mesher can generate. The thickness of the fan blade is 1 mm, while the base size is 2 mm. Setting the minimum surface size to 50% of the base size returns 1 mm and allows the mesh to capture the details of the fan blades.
    5. Select the Prism Layer Controls > Prism Layer Total Thickness node, set Size Type to Absolute, and set Absolute Size to 2 mm in the Properties Window.
      By default, all size controls are set as a percentage of the base size. By setting the size type to absolute, you make this property independent of the base size. Absolute values are useful when you want to have full control over the size of a particular setting.
Boundaries in the simulation regions affect how the mesh is generated. More specifically, prism layers are generated next to wall boundaries and interfaces (the contacting surface between the regions). The far field walls of the simulation domain (the walls that are far away from the object of interest) are not important for this simulation; however, for the purpose of this tutorial, the size of the simulation domain is smaller than what is recommended for industrial cases. Ideally the far field surfaces in the simulation domain should be further away, as having these surfaces close to the geometry of interest will affect the flow inside the simulation domain. One way to reduce the effect of the walls on the overall flow inside the simulation domain is to set the outer surfaces to symmetry boundaries. Prism layers are not generated on symmetry boundaries.
  1. Set the walls of the simulation domain to symmetry boundaries:
    1. Expand the Regions > Static Region > Boundaries node.
    2. Select the Block.Block Surface, Block.Downstream, and Block.Upstream nodes and set Type to Symmetry Plane.
      The selected boundary surfaces change to a blue color in the geometry scene to indicate that they are symmetry boundaries.
  2. Save the simulation.
  3. To generate the volume mesh, right-click the Automated Mesh node and select Execute.
    The surface remesher retriangulates the initial geometry surface tessellation into more evenly sized triangles. The space for the prism layer is calculated and reserved, this is called the prism layer subsurface. The polyhedral mesher creates three-dimensional cells, called tetrahedra, from the retriangulated surface and converts them to polyhedra. The prism layer is then generated and fills the reserved space with prism layer cells.
  4. Create a mesh scene to visualize the mesh:
    1. Right-click Scenes and select New > Mesh.


    2. Rename the Scenes > Mesh Scene 1 node to Simulation Domain.
    3. Create another mesh scene and rename it to Fan and Enclosure.
    4. Click Scene/Plot above the simulation object tree.
    5. Double-click the Mesh 1 > Parts node.
    6. In the Parts dialog, right-click on a blank area of the dialog and select Deselect All to clear the selection.
    7. In the same dialog, expand the Regions node.
    8. Select the Rotating Region > Boundaries > Fan and Static Region > Boundaries > Enclosure.Default.
    9. Click OK.


      The cell size automatically adjusts, within the specified parameters, to capture the shape of geometry.

  5. Save the simulation.