Preparing for Post-Processing

Simcenter STAR-CCM+ In-cylinder provides several plots and scenes by default. You can analyze the scenes and plots while the simulation is running, as well as when it completes.

If you open and prepare the scenes and plots before you run the simulation, they are updated continuously as the solution progresses: For combustion simulations that use the Complex Chemistry model or an ECFM model, Simcenter STAR-CCM+ In-cylinder provides various reports and plots for heat release post-processing, such as the chemical or apparent heat release, by default. As the computation of these quantities can be computationally expensive, you can deactivate the quantities that are not relevant for you: Set up chemical heat release post-processing.
To prepare for post-processing:
  1. To open a plot, right-click the Results > Plots > [plot] node and select Open, where [plot] is the plot of interest, such as In-Cylinder - Cylinder > Cylinder : Mass.
    The plot opens in the Graphics window.
  2. To open a scene:
    1. Right-click the Results > Scenes > [scene] node and select Open, where [scene] is the scene you want to display, such as Velocity Magnitude.
      The scene opens in the Graphics window and displays the respective scalar field on a section that cuts through the engine domain.
    2. If you want to show the mesh on that plane section, select the [scene] > [scene] Derived Parts Scalar 1 node and activate Display Mesh.
  3. To display the solution on additional plane sections in a scene:
    1. Right-click the [scene] > [scene] Derived Parts Scalar 1 > Parts > [plane section] node and select Show, where [plane section] is the plane section of interest, such as Cylinder Center X Plane.
    2. To hide a plane section from a displayer, right-click the [plane section] node of interest and select Hide.
  4. To display a scalar field on Engine Part Surfaces in a scene:
    1. Depending on the Engine Part Surfaces on which you want to display a scalar field, select one of the following nodes:
      • For valve surfaces, select the respective [scene] > Intake/Exhaust Valve [n] Displayer 1 > Scalar Field node.
      • For the piston surface, select the [scene] > Cylinder Piston Surface Displayer 1 > Scalar Field node.
      • For cylinder surfaces, apart from the piston surface, select the [scene] > Cylinder Displayer 1 > Scalar Field node.
    2. Set Function to the scalar field that you want to display, such as Temperature.
      The scene displays the selected scalar field on the surfaces of interest. For cylinder surfaces, including the piston surface, the scalar field is displayed with reduced opacity to reveal internal structures.
    3. To obtain a view of internal structures, you can render a displayer visible or invisible by right-clicking the respective [scene] > [displayer] node and select Toggle Visibility.
  5. For charge-motion simulations, to display a scalar field other than the default particle diameter on injected fuel parcels, or to toggle the visibility of the parcels, follow Step 4 using the displayer Spray 1.
  6. For charge-motion simulations, the Fuel Distribution scene allows you to visualize different definitions of air-fuel mixture ratio. For each definition, the scene provides an individual displayer. The displayer that is visible by default is the Air/Fuel Ratio Derived Parts Scalar 1 displayer, which displays the air/fuel ratio. To visualize another definition of air-fuel mixture ratio, such as the fuel/air equivalence ratio, toggle the respective displayer, such as the Fuel/Air Equivalence Ratio Derived Parts Scalar 1 displayer, visible as described in Step 4c.
  7. If you require additional scenes to analyze your simulation results, create a new scene:
    1. Be clear on what quantities you want to analyze and from which objects you want to extract the quantities.
    2. Right-click one of the pre-defined scenes and select Copy.
    3. Right-click the Scenes manager node and select Paste.
    4. Modify the scene displayers to suit your analysis requirements, see Using Displayers.
  8. To write a scene to image files at regular intervals, follow the steps described in Saving Scene Images to File.
    By default, Simcenter STAR-CCM+ In-cylinder writes scenes to image files using the following file format:

    [scene_title]_image_[time]_degCA.png

    where the number format of [time] is %011.5f.

    Example: Absolute_Pressure_image_00070.00216_degCA.png
  9. For combustion simulations, to set up the heat release post-processing:
    1. Right-click the Results > Settings > Combustion node and select Edit.
    2. In the Combustion Settings dialog, deactivate the options that are not relevant for you:
      • Generate Heat Release Output
      • Calculate Apparent Heat Release
      • Calculate Chemical Heat Release
      • Generate Mass Fraction Burned Output
    3. For the generation of mass fraction burned output values, define the combustion interval by activating at least one start and end event, respectively:
      • For Start: Custom Start Angle, Ignitor [n] : Spark Start Time, or Injector [n] : Start of Injection
      • For End: Custom End Angle or Exhaust Valve [n] : Opening
      The combustion interval is the time between the latest start event and the latest end event.
      For more information, see Results Reference—Combustion Settings Dialog.
For more information, see Visualizing the Solution.

The setup of your ICE simulation is now complete.

  1. Save the simulation .