Specifying Physics Models and Global Parameters

Two physics continua are required for this tutorial, one for the solid manifold region and another for the fluid that flows through it. Unsteady time models are chosen for both physics continua, along with compatible energy models.

To select the physics models for the exhaust gas within the manifold:
  1. Rename the Continua > Physics 1 node to Physics Fluid.
  2. For the physics continuum, Continua > Physics Fluid, select the following models in order:
    Group Box Model
    Space Three Dimensional (selected automatically)
    Material Gas
    Time Implicit Unsteady
    Flow Segregated Flow
    Equation of State Ideal Gas
    Energy Segregated Fluid Temperature
    Viscous Regime Turbulent

    Reynolds-Averaged Navier-Stokes (selected automatically)

    Reynolds-Averaged Turbulence K-Epsilon Turbulence

    Two-Layer All y+ Wall Treatment (selected automatically)

    Wall Distance (selected automatically)

    Realizable K-Epsilon Two-Layer (selected automatically)

To define a physics continuum for the solid manifold:
  1. Create a physics continuum named Physics Solid.
  2. For the physics continuum, Continua > Physics Solid, select the following models in order:

    Group Box

    Model

    Space Three Dimensional
    Material Solid
    Time Implicit Unsteady
    Optional Models Segregated Solid Energy

    Gradients (selected automatically)

    Equation of State Constant Density
  3. Right-click the Models > Solid > Al node and select Replace With....
  4. In the Replace Material dialog, expand the Material Databases node and select Standard > Solids > Ductile Iron.
  5. Select the Regions > Manifold Solid node and set Physics Continuum to Physics Solid.
As this tutorial is defined in the context of a reciprocating engine, it is natural to define time durations using degrees crank angle rather than seconds. Here, you use global parameters to define the time corresponding to 1 deg CA of engine motion and the engine cycle length. For the engine from which the fluid boundary conditions are taken, the cycle length is 720 deg CA and the rotation rate is 1400 rpm.
  1. To create a parameter for the crank angle time:
    1. Right-click the Automation > Parameters node and select New > Scalar.
    2. Rename the Scalar node to CrankAngleTime(s) and set its properties as follows:
      Property Setting
      Value 1/(6*1400)
      Dimensions Time
  2. To create a parameter for the time step size of the fluid solution:
    1. Right-click the Automation > Parameters node and select New > Scalar.
    2. Rename the Scalar node to FluidTimeStep(s) and set its properties as follows:
      Property Setting
      Value 2*${CrankAngleTime(s)}
      Dimensions Time
  3. To create a parameter for a cycle length:
    1. Right-click the Automation > Parameters node and select New > Scalar.
    2. Rename the Scalar node to FluidCycleLength(s) and set its properties as follows:
      Property Setting
      Value 720*${CrankAngleTime(s)}
      Dimensions Time
  4. To create a parameter for the time step size of the solid solution:
    1. Right-click the Automation > Parameters node and select New > Scalar.
    2. Rename the Scalar node to SolidTimeStep(s) and set its properties as follows:
      Property Setting
      Value 2*${FluidCycleLength(s)}
      Dimensions Time
  5. Save the simulation.