Directed Meshing Workflow

In Simcenter STAR-CCM+, a directed mesh has its own operation node that identifies the parts in which the mesh belongs, and the sources and target surfaces within those parts.

You can use geometry that has CAD, partial CAD, and no CAD with the directed mesher. For parts with CAD, see Preparing CAD Parts for Directed Meshing. For parts with without CAD, see Preparing Non-CAD Parts for Directed Meshing.

To create a mesh using the directed mesh approach:

Right-click the Geometry > Operations node and select New > Mesh > Directed Mesh.
In the Create Directed Mesh Operation dialog, select the parts that you want to use for the directed meshing operation and click OK.

Simcenter STAR-CCM+ creates an Operations > Directed Mesh node.

Parts that are selected for directed meshing are listed under the Directed Mesh > Connected Parts node. Multiple parts that form a contiguous set of bodies are represented by a single connected parts object.

Note The yellow warning triangles indicate that further action is needed before the operation is fully defined. The triangles disappear when you generate the volume mesh.

For subsequent steps, you are generally advised to work with the Directed Mesh panel activated, as this mode allows interactive editing within the graphics window. However, you can also choose particular child nodes in the simulation tree, and edit their properties directly.

To activate the Directed Mesh panel:

Right-click the Operations > Directed Mesh node and choose Edit...
Choose the source surface(s) and target surface for each connected part.
See Choosing Source and Target Surfaces.
Create the starting mesh on the source surfaces. Choose from one of the following methods:
- Draw patches on the source surface and have Simcenter STAR-CCM+ mesh these with quad faces (applies to 1-1, single-source to single-target directed meshing only). See Creating a Source Mesh Using Patches.
- Take the source meshes from the side of an existing volume mesh. See Creating a Source Mesh Using An Existing Mesh.
- Create a 2D source mesh using an 2D Auto Mesh operation. See Creating a 2D Source Mesh.

Two methods are available to define the cell layers for a volume distribution. You can either set the number of layers directly, or you can provide size parameters and let the mesher compute the number of layers and their thickness variation.

Select the Default Distribution node and set Size Specification to one of the following options:
- Number of Layers (Default)
  Allows you to specify the number of layers across the volume mesh. Complete the steps in Volume Distribution Using Number of Layers.
- Size
  Allows you to control the properties of the cell layers in the volume mesh. Complete the steps in Volume Distribution Using Size Based Specification.
The default distribution is only available for new directed mesh operations. You can also create volume distributions directly under the Mesh Distribution node. For more information, see Creating Additional Distributions. If you load a simulation file containing a previously defined directed mesh, the default distribution node is not available.
Generate the volume mesh.
See Generating the Directed Volume Mesh.