Coupling Simcenter STAR-CCM+ to GT-SUITE

Instruct Simcenter STAR-CCM+ to launch GT-SUITE in server mode and connect to it. Use the average zone flag field function to visualize the areas where the flow is approximately one dimensional.

To set up the communication, specify the version of GT-SUITE (in this tutorial, v2022), the location of the GT-SUITE input file, and the method for launching and connecting to GT-SUITE:
  1. Expand the External Links > Link 1 > Conditions node and set the following properties:
    Node Property Setting
    GT-SUITE Version Version v2022
    Launch Partner Option Option Launch Application (default)
  2. Expand the Link 1 > Values node.
  3. Select the GT-SUITE Model File node and set GT-SUITE Input File to GT-SUITE_caseFiles/CFDCoupling_Setup.gtm. If you saved the input file to a different location, adjust the file path as required.
    You can type the file path and name manually, or you can click (Custom Editor) and use the dialog to navigate to the file.
In order to launch GT-SUITE in server mode, Simcenter STAR-CCM+ requires you to specify the location of the GT-SUITE installation and license file using two environment variables, $GTIHOME and $GTISOFT_LICENSE_FILE, respectively.
  • If you did not define the required global variables on your system, specify them locally by setting the following properties:
    Node Property Setting
    GTIHOME Environment Variable GTIHOME [Path to GT-SUITE Installation]
    GTISOFT_LICENSE_FILE Environment Variable GTISOFT_LICENSE_FILE [Path to GT-SUITE License]
  1. Right-click the Link 1 node and select Launch and Connect.
    The GT-SUITE solver is started in the background, waiting for Simcenter STAR-CCM+ to begin running its solver. Clearing the solution stops the GT-SUITE solver and breaks the connection to Simcenter STAR-CCM+. If you clear the solution, restart the GT-SUITE solver as outlined above.
Visualize the volume where physics values and mass fractions are averaged and sent to GT-SUITE. Inspect the zone and determine whether the flow is relatively one dimensional.
  1. Create a scalar scene.
  2. Edit the Scalar Scene 1 node and set the following properties:
    Node Property Setting
    Outline 1 Surface Activated
    Mesh Activated
    Scalar 1
    Parts Parts Cyl1
    Cyl2
    Cyl3
    Cyl4
    EGR
    Intake
    Wall
    Scalar Field Function Average Zone Flag
    Min 1
    Max 6
    Color Bar Levels 6
  3. Click (Save-Restore-Select views) and restore View 1.
  4. Initialize the Solution.
    A scene similar to the one shown below appears.

    The scalar values, which relate to which boundary was created first in Simcenter STAR-CCM+, are of no significance and simply highlight the individual zones.

  5. Save the simulation.