Preparing the Geometry

One of the first steps in preparing a fluid flow simulation is to define the geometry of the flow domain. In Simcenter STAR-CCM+, you can create the geometry of the flow domain in 3D-CAD or import the geomety from a third-party tool.

Before you prepare the geometry of the flow domain, decide which parts of the physical system being modeled are occupied by a fluid and must therefore to be included in the solution domain. Simcenter STAR-CCM+ allows you to model internal flow, external flow, or both. Whatever its geometry, the fundamental requirement is that the solution domain is bounded. This means that you have to examine the system geometry carefully and decide exactly where the enclosing boundaries lie.

The boundaries of a flow domain can be categorized as follows:

Wall Boundaries
Wall boundaries represent walls or solid obstacles of some description that serve to physically confine a fluid flow.
Symmetry/Periodic Boundaries
Symmetry boundaries and periodic boundaries represent imaginary axes or planes of symmetry or periodicity. The purpose of these boundaries is to reduce the extent of the computational domain in locations where the geometry and the flow are symmetric or periodic. Excluding regions where the solution is essentially known allows you to save computational expense and to model the remaining flow domain in greater detail.
Flow Boundaries
Flow boundaries are boundaries where the fluid enters or leaves the simulation domain, such as inflow boundaries, outflow boundaries, or free-stream boundaries. These boundaries are non-physical surfaces that serve to close off the solution domain in regions not covered by the other two types of boundary.

Difficulties in specifying boundary location normally arise where the flow conditions are not completely known, for example at outlets. The recommended solutions are to place boundaries as follows:

  • In regions where the conditions are known or can be guessed reasonably well
  • In regions where the approximations in the boundary condition specification are unlikely to propagate upstream into the regions of interest

Thus, locating boundaries may require some trial and error. Whenever possible, it is particularly important to avoid the following situations:

  • A boundary that passes through a major recirculation zone
  • In transient transonic or supersonic compressible flows, an outlet boundary located where the flow is not supersonic

To prepare or import the geometry in Simcenter STAR-CCM+:

  1. Launch Simcenter STAR-CCM+ and start a simulation.
  2. Define bodies and surfaces of the geometry using 3D-CAD or a third-party software of your choice:
    • For internal fluid flow, extract the wetted volume contained within the bodies that define the solid enclosure. 3D-CAD can automatically extract the volume of space inside a model, see Internal Volume Extraction.
    • For external fluid flow, create a shape that contains the fluid as it moves around the body. For external aerodynamics, you typically use a hexahedron or a sphere whose outer surface represents the far-field conditions of the flow, with domain extents around 8–10 body lengths or wing spans, whichever is larger, from the body. You can extract the required external volume in 3D-CAD, see External Volume Extraction.
    • Make sure that the surfaces where you want to apply different boundary conditions have their own patch and name.
    • For a fully-developed flow, you can model a short section of the pipe and use periodic contacts upstream and downstream, rather than using a length of pipe with inlet and outlet boundaries. Make sure that the upstream and downstream flow boundaries are defined as separate part surfaces.
    • To limit the computational cost, remove any non-essential CAD features.
  3. Create geometry parts:
    • If you prepared the geometry using 3D-CAD, right-click the Geometry > 3D-CAD Models > [3D-CAD Model] node and select New Geometry Part. In the Parts Creation Options dialog, click OK. Simcenter STAR-CCM+ creates a geometry part for each body defined in the 3D-CAD model. For each named surface, Simcenter STAR-CCM+ creates corresponding part surfaces. Simcenter STAR-CCM+ also creates part contacts from coincident surfaces in the 3D-CAD model, such as contact surfaces between a solid and a fluid body.
    • If you prepared the geometry using a third-party tool, import the surface mesh as a part in the simulation. During the import process, Simcenter STAR-CCM+ automatically creates geometry parts and surfaces based on the surface mesh specifications, and generates part contacts from coincident surfaces. See Importing Surface Data into STAR-CCM+.
  4. If you wish to split a surface for use in defining specific boundary conditions or customizing the mesh, you can manipulate part surfaces in several different ways, see Manipulating Part Surfaces.
  5. For a fully developed flow simulation where you only model a section of the geometry, create a periodic contact between the upstream and downstream surfaces:
    1. Within Geometry > Parts, multi-select the part surfaces that represent the upstream and downstream surfaces, right-click one of the selected surfaces, and select Create Periodic.
      When you select the part surfaces, select the upstream side first, then the downstream side. If you select the sides in the wrong order, the flow direction is reversed.
    2. Select the Contacts > [part/part] > [periodic contact] > Periodic Transformation node and set Periodicity to Translational.
  6. Assign the geometry parts that represent your flow domain to regions.
    For a fully developed flow simulation, to create the periodic interface as a boundary-mode interface, set the following options in the Assigns Parts to Regions dialog:
    • Create a Region for Each Part
    • Create a Boundary for Each Part Surface
    • Create Boundary-mode Interfaces From Contacts

    These settings create an Interfaces > [periodic interface] node.

    In general, it is good practice to assign the surfaces that belong to an interface to separate boundaries. This practice is useful when troubleshooting interface issues, as you can check whether the boundary faces are correctly mapped to the interface boundary.

    For more information on creating regions, boundaries, and interfaces, see Regions Layout Workflow.