Preparing the Geometry for SPH

The first step in SPH flow simulations consists of preparing the geometry and subsequently associating the geometry parts with their respective surface regions.

You prepare the following three types of geometry for an SPH simulation:
  • The geometry parts and their surfaces that describe the boundaries in the simulation. For an SPH simulation, you are not required to import or create closed and error-free surfaces as a starting point for discretization.
  • You define the initial shape and position of the liquid by using geometry parts. For these geometry parts, you are required to import or create closed and error-free surfaces.
  • In cases where you use position-based particle removal, you create a Bounded Shape geometry part that encloses the geometry parts that describe the boundaries. Particles that cross the surfaces of this geometry part are removed automatically from the simulation. For more information, see Removing and Redistributing Particles.

A surface region represents the domain for a Smoothed-Particle Hydrodynamics (SPH) multiphase simulation. Although each geometry in SPH flow has an initial triangulation, specific (complex) surfaces may need remeshing before running an analysis to ensure an optimal solution on the surface.

To prepare the geometry for SPH flow simulations:
  1. Define the bodies and surfaces of the geometry that represent the actual boundaries in the domain:
    1. Import the geometry from a third-party software of your choice or create the geometry in 3D-CAD.
    2. Right-click a Geometry > Parts > [part] node and select Assign Parts to Regions.
      The Assign Parts to Regions dialog appears.

    3. Select Surface Topology for the topology definition.
    4. Set the remaining properties in the Assign Parts to Regions dialog. See Assign Parts to Regions Reference.
    5. Click Apply and then Close to exit the dialog.

To define the initial shape and position of the liquid, you create a geometry part. You define this geometry part such that it conforms to the wall boundaries.

You can use boolean operations to adapt the geometry.

  1. For example, one way to create the geometry part that defines the initial shape and position of the liquid:
    1. Right-click the Geometry > Parts node and select New Shape Part > Block and choose the coordinates that correspond to your wall boundaries and the initial height of the fluid.
    2. Multi-select the Parts > Block node and outer boundary parts, right-click one of the selected nodes, and select Create Mesh Operation > Boolean > Intersect.
    3. In the Create Intersect Operation dialog, activate Execute Operation Upon Creation, then click OK.
    4. Select the Parts > Intersect node and any internal parts of your domain, right-click one of the selected nodes, and select Create Mesh Operation > Boolean > Subtract.
      The Parts > [subtract] node is created. Depending on your geometry, you may require more operations to extract the fluid volume, refer to Performing Boolean Operations for more details.
    Refer to Generating the Particles for SPH for how to initialize the liquid within the created geometry part.
  2. Create a Bounded Shape geometry part to use with position-based particle removal:
    1. Right-click the Geometry > Operations node and select New > Boolean > Bounded Shape.
    2. In the Create Bounded Shape Operations dialog, select the geometry parts that the bounded shape is meant to enclose, then click OK.
    3. Right-click the Operations > Bounded Shape node and select Execute.
    You do not assign the bounding box to the surface region for analysis, as this specific part is only used for the Particle Remediation model.

The surface mesh is used when computing boundary values. When you analyze forces and moments the surface mesh must not be 5 times smaller than the particle size to ensure that there are ghost particles within each surface cell.

  1. If you want to remesh the initial surface for any complex surfaces, you use a Surface Remesher automated mesh operation and select the parts that you want to remesh. For guidelines on setting up the surface mesh, see Surface Remesher Reference.