Post-Processing: Creating Streamlines

In Simcenter STAR-CCM+, streamlines are created as derived parts and then added to a scene using a streamline displayer. A streamline part represents the path of a massless particle through the flow—although you can compute the path from any vector field, not just velocity.

Here, you define a streamline derived part so that it shows the recirculating flow behind a blunt body. Modify the part to show streamlines over the blunt body.

To prepare for this tutorial, either work through the Introductory tutorial first, and use that simulation file, or else download the file supplied in the tutorials bundle. To use the file from the tutorials bundle:
  1. From the tutorials bundle, from the introduction folder, copy Introduction_final.sim to your working directory.

    See Downloading the Tutorial Files from the Support Center Portal.

  2. Open Introduction_final.sim and save it as velocityMagnitudeStreamlines.sim.
To set up the streamlines in a new scene:
  1. Right-click the Scenes node and select New > Geometry.
  2. Right-click the Derived Parts node and select New > Streamline.

    A new interactive in-place dialog (Create Streamline) appears.

    The entire fluid region is used as the input part for the streamline part. The seed point is located just after the back of the blunt body (in the direction of flow).

  3. Set the following values:
    Property Value
    Input Parts [subdomain-1]
    Seed Mode Line Seed
    Point 1 [0.045, 0.02, 0.01] m
    Point 2 [0.045, 0.001, 0.01] m
    Resolution 20
    Vector Field Velocity
    Direction Both
    To visualize the seed point interactively, activate Display Tool.

    The properties of the Edit dialog are similar to those in the following screenshot:



  4. Click Create and then Close.

    In the Simulation tab, a node, Streamline, has been added within the Derived Parts. In addition, a new streamline displayer Streamline Stream 1 has been added to the scene.

  5. Fine-tune the streamline derived part:
    1. Select the Streamline > 2nd Order Integrator node and set Initial Integration Step to 0.1 to provide more resolution to the streamlines.
    2. Set Maximum Propagation to 5.0.
    3. Set Max Steps to 1000.
      This option, together with the maximum propagation, provide a stopping criterion to make sure that the streamlines are not calculated endlessly.
  6. In the Scene/Plot tab, select the Surface 1 > Parts node and set Parts to Parts > subdomain-1 > Surfaces > Inner_wall.
  7. select the Streamline Stream 1 node to customize how the streamlines appear:
    1. Set the Mode to Tubes so that the streamlines are displayed as tubes instead of lines.
    2. Specify Width at 2.0E-4, the width of the tube in meters.
  8. To highlight large differences in velocity magnitude effectively, within the Streamline Stream 1 node, select Color Bar and set Color Map to purple-red basic (large difference).
  9. Also within the Streamline Stream 1 node, select the Scalar Field node and set Function to Velocity: Magnitude.

    The modified streamlines appear as below.



  10. Save the simulation.