Setting the Engine Models

Simcenter STAR-CCM+ In-cylinder contains models and methods that allow you to perform different types of in-cylinder simulations.

The following simulation types are supported:
  • Motored-Test

    By default, Simcenter STAR-CCM+ In-cylinder performs a motored-test simulation, which involves modeling the transient flow in the ports and the cylinder.

    The objective of a motored-test simulation is typically to maximize the trapped air mass and to examine the bulk motion (swirl and tumble) and the turbulence that this flow induces.

  • Charge-Motion

    For a charge-motion simulation, you inject a liquid fuel into the engine cylinder. Additionally, you can include models for the primary atomization and secondary breakup. Primary atomization refers to the process of forcing liquid through a small orifice at a high pressure, resulting in a fine spray of liquid droplets. Secondary breakup describes the process of droplets breaking up under the action of non-uniform surface forces that are induced by their motion relative to the air.

    For fuel droplets that impinge on a wall, you can model the formation and transport of a thin film of fuel on the engine walls. In Simcenter STAR-CCM+ In-cylinder, this fluid film is modeled using a shell region that is created from existing Engine Part Surfaces.

    The objective of a charge-motion simulation is typically to examine the fuel evaporation and the air/fuel mixing process in the cylinder until the intended time of ignition (start of combustion).

  • Combustion

    Simcenter STAR-CCM+ In-cylinder allows you to perform combustion simulations of liquid or gaseous fuels. Gaseous fuels enter the engine through burner ports or pre-mixed with air through the intake port.

    The objective of a combustion simulation is to get at a complete prediction of the engine performance including the mechanism of ignition, flame propagation, and diffusion combustion in the engine cylinder.

    If the main interest is in the effects produced by the existence of combustion rather than the combustion process itself (such as wall heat transfer), you can approximate the fuel burning rate through an analytic function instead. This function can be derived from experimental results or a previous simulation.

For motored-test, charge-motion, and combustion simulations, you can include gravity effects in your simulation.

By default, Simcenter STAR-CCM+ In-cylinder calculates the gas density according to the ideal gas equation. Alternatively, you can apply a real gas model. The real gas model is suitable for modeling complex chemistry combustion applications at high pressures and low temperatures in transcritical and supercritical environments. The density of liquid fuels is calculated as a function of temperature in the form of a polynomial by default. You can choose to use constant density instead.

By default, Simcenter STAR-CCM+ In-cylinder solves for the Reynolds-Averaged Navier Stokes (RANS) equations, that govern the transport of the mean flow quantities. To provide closure relations for the RANS equations, Simcenter STAR-CCM+ In-cylinder uses the Realizable K-Epsilon Two-Layer turbulence model with an all- y + wall treatment. Alternatively, you can use the Re-Normalisation Group (RNG) version of the K-Epsilon model with a two-layer all- y + wall treatment. If you want to solve the large scales of the turbulence directly and model only the small-scale motions, you can run a Large Eddy Simulation (LES). One justification for the LES technique is that by modeling “less” of the turbulence, and explicitly solving for more of it, the error in the turbulence modeling assumptions is not as consequential. Furthermore, it is hypothesized that the smaller eddies are self-similar and thus lend themselves to simpler and more universal models. The downside of the approach is the increase in computational expense.

When solving the discretized system of equations for the fluid continuum, Simcenter STAR-CCM+ In-cylinder applies the PISO algorithm by default. Alternatively, you can choose to apply the SIMPLE algorithm. To choose the appropriate algorithm for your simulation, consider the following aspects:

  • Both algorithms provide the same level of temporal accuracy, however, PISO is faster than SIMPLE for small time-steps.
  • For large time-steps, that is, when the combined CFL number increases to a significantly larger value than 10, PISO becomes unstable. SIMPLE, on the other hand, remains stable.
  • As time-step size increases, SIMPLE loses temporal accuracy of transient solutions.
To set the engine models:
  1. Depending on the type of simulation you want to run, set the engine models as follows:
    Simulation Type Procedure
    Motored-Test

    (default)

    		 No additional engine models are required.
    Charge-Motion

    (for liquid fuels)
    1. Right-click the Models node and select Edit.
    2. In the Model Selection dialog, select the following models:
      Group Box Model
      Optional Models
      • Injection

        The Polynomial Fuel Density model is selected automatically. If you want to apply a constant fuel density instead, deselect Polynomial Fuel Density and, in the Fuel Density group box, select Constant Fuel Density.

      • To account for secondary breakup of the liquid fuel droplets, select one of the following models (the most appropriate breakup regime for each model is noted in parantheses):
        • KHRT Breakup (stripping, catastrophic)
        • Reitz-Diwakar Breakup (bag, stripping)
      • To account for the formation and transport of a thin film of liquid fuel on the engine walls, select Liquid Film.
      • To obtain the vapor pressure at the liquid surface for complex multi-component fuels, where the molecular structure of components is very different, select Modified UNIFAC.
      Atomization

      (only if a secondary breakup model is selected)
      • To account for primary atomization, which allows you to simulate the disintegration process of a liquid jet exiting from a nozzle injector, select Huh Atomization.
    3. Click Close.
    4. For the Reith-Diwakar Breakup model, set the model parameters as follows:
      1. Edit the Models > Reitz-Diwakar Breakup node.
      2. In the Bag Breakup group box, set the following properties:
        • Minimum Weber Number (WeCrit)
        • Time-scale coefficient (Cb2)
      3. In the Stripping Breakup group box, set the following properties:
        • Onset coefficient (Cs1)
        • Time-scale coefficient (Cs2)

        See Models Reference—Reitz-Diwakar Breakup Dialog.

      4. Click Apply, then Close.
    5. For the KHRT Breakup model, set the model parameters as follows:
      1. Edit the Models > KHRT Breakup node.
      2. In the KH Breakup group box, set the following properties:
        • Length Coefficient (B0)
        • Time Coefficient (B1)
        • Normal Velocity Coefficient (A1)
      3. In the RT Breakup group box, set the following properties:
        • Length Coefficient (C3)
        • Time Coefficient (Ctau)

        See Models Reference—KHRT Breakup Dialog.

      4. Click Apply, then Close.
    6. For the Huh Atomization model, set the model parameters as follows:
      1. Edit the Models > Huh Atomization node.
      2. In the Model Parameters group box, set the following properties:
        • Atomization Length Scale Coefficient (C1)
        • Wave Length Scale Coefficient (C2)
        • Spontaneous Time Scale Coefficient (C3)
        • Exponential Time Scale Coefficient (C4)
        • Turbulence Time Scale Coefficient (CA1)
        • Turbulence Length Scale Coefficient (CA2)
        • Breakup Rate Coefficient (KA)
        • Normal Velocity Coefficient
        • Critical Weber Number.

        See Models Reference Huh—Atomization Dialog.

      3. Click Apply, then Close.
    Combustion

    (for liquid or gaseous fuels)

    		 See Setting the Engine Models for a Combustion Simulation.
To include gravity effects:
  1. Edit the Models node and, in the Optional Models group box, select Gravity.
    By default, the gravitational acceleration vector has a magnitude of 9.81 m/s² and points in negative Z-direction of the Laboratory coordinate system.
  2. Click Close.
  3. To modify the gravitational acceleration vector, edit the Models > Gravity node and, in the Gravity group box, set the gravity vector as required.
    The Graphics window displays the gravity vector as a black arrow.
  4. Click Apply, then Close.
To apply the real gas model:
  1. Edit the Models node and, in the Optional Models group box, select Real Gas.
  2. Click Close.
To use the RNG version of the K-Epsilon turbulence model:
  1. Edit the Models node and, in the Enabled Models group box, deselect Realizable K-Epsilon Two-Layer.
  2. In the K-Epsilon Turbulence group box, select RNG K-Epsilon.
  3. Click Close.
To apply the Large Eddy Simulation technique:
  1. Edit the Models node and, in the Enabled Models group box, deselect RANS.
  2. In the Turbulence group box, select LES.
  3. Click Close.
To apply the SIMPLE algorithm:
  1. Edit the Models node and, in the Enabled Models group box, deselect PISO Unsteady.
  2. In the In-Cylinder Time group box, select Implicit Unsteady.
  3. Click Close.
For more information, see Models Reference.