Modeling Smoothed-Particle Hydrodynamics Flow

The Smoothed-Particle Hydrodynamics model is a Lagrangian approach that represents the fluid as a collection of particles with inherent material properties that move with the fluid. You use the SPH model to simulate highly dynamic free-surface flows.

For simulations with the Smoothed-Particle Hydrodynamics (SPH) multiphase model, Simcenter STAR-CCM+ requires a sphflow license in addition to the other license features. See also Simcenter STAR-CCM+ 许可.

The SPH model uses an Incompressible Flow (ISPH) physics model for solving the conservation equations for SPH multiphase simulations. You can model particles that are distributed and carried freely in the computational domain by defining a fluid phase. Smoothed-particle hydrodynamics multiphase solver uses a pressure-velocity segregated approach to maintain mass conservation within the velocity field.

For an example workflow with Smoothed-Particle Hydrodynamics (SPH), see the Smoothed-Particle Hydrodynamics (SPH): Gearbox Lubrication tutorial.

To set up a Smoothed-Particle Hydrodynamics (SPH) flow simulation:

Prepare the required geometry and surface regions as appropriate to your simulation.
See Preparing the Geometry for SPH.

Select the physics continuum models:

Right-click the Continua node and click New Physics Continuum.

Right-click the Continua > [physics continuum] > Models node and select the following models, in order:


Group Box	Model
Space	Three Dimensional
Time	Implicit Unsteady
Material	Multiphase Multiphase Interaction (selected automatically)
Multiphase Model	Smoothed-Particle Hydrodynamics (SPH)—this model activates SPH flow modeling. See Smoothed-Particle Hydrodynamics (SPH) Model Reference. Incompressible Flow (ISPH) (selected automatically)—this model facilitates robustness of the numerical solution by smoothing the free surface and the pressure field. See Incompressible Flow (ISPH) Model Reference. Adaptive Time-Step (selected automatically)—this model automatically controls the time-step during the simulation based on SPH flow specific critera. See Adaptive Time-Stepping. Gradients (selected automatically)
Viscous Regime	Select one of: Laminar Inviscid
Optional Models	If gravity forces influence the solution, select Gravity. If you want to improve the robustness and stability of the SPH flow simulation by excluding fluid particles that leave the region of interest of the computational model, select Particle Remediation. See Removing and Redistributing Particles.

If you want to prevent numerical pressure oscillations and enhance the overall accuracy and stability of the simulation, select the Models > Incompressible Flow (ISPH) node and specify the stabilizations properties to smooth the free surface and pressure.
See Incompressible Flow (ISPH) Model Properties.

Define the liquid phase:

Right-click the [physics continuum] > Models > Multiphase > Phases node and select New.

Right-click the Phases > [phase] > Models node and select the following models:


Group Box	Model
Material	Liquid
Equation of State	Constant Density (selected automatically)

To specify the material properties for the phase, select the [phase] > Models > Liquid > [phase material] > Material Properties node and specify values for the following material properties:
- Density
- Dynamic Viscosity

To specify the initial conditions, select the Initial Conditions node and specify the Velocity and Pressure values.
See Initial Conditions.
Specify the wall boundary conditions and values for the surface region.
See Setting Boundary Conditions.
To set up adaptive time-stepping, right-click the Models > Adaptive Time-Step > Time-Step Providers node and select the following:
- Convective CFL—you are advised to always select this time-step provider.
- Gravity CFL—you are advised to always select this time-step provider.
- Viscous CFL—you are advised to add this time-step provider when using explicit time integration for the velocity solver.
  See SPH Adaptive Time-Step Providers Reference.
Discretize the fluid by generating particles within the geometry part that defines the initial shape and position of the fluid.
See 生成 SPH 颗粒.
(Optional) Reverse the orientation of the boundary surfaces. Fluid particles consider a boundary condition only on the positive side of a boundary. For closed surfaces, the positive side is facing outwards by default. Depending on whether you want to simulate internal or external flow, you are required to reverse the orientation of the boundary surface normals.
See Orienting Boundary Normals.
If you want to include rotating parts in your simulation, select the Regions > [surface region] > Physics Values > Direct Rotating Option node and specify the direct rotating motion values.
If there are more parts assigned to the same region, you can subgroup the parts, and then define a rotation for each subgroup. See Defining Direct Motion Rotation.
Set up any reports, monitors, plots, and scenes that you require to prepare for post-processing.

For example, to determine the forces or torque exerted by the fluid on a boundary, you can create a monitor and plot the Force or Moment reports.

See SPH Post-Processing Reference.
Set the solver parameters and stopping criteria, then run the simulation.
In assessing the convergence of SPH flow simulations, the residuals as an initial indicator highlight discrepancies in the monitored field variations. Additionally, it is essential to check that particles satisfy the wall conditions (minimal or no boundary crossing). To ensure result accuracy, a convergence study with multiple discretizations is also recommended.

If necessary, you can enhance the convergence of the simulation by modifying the SPH flow solver numerical properties.
See 平滑颗粒流体动力学求解器参考.