Running the Simulation

Before running the simulation, you create one report for the volume-averaged fluid temperature. Another two reports are defined to monitor the boundary heat flux across the contact interface. One pre-defined report outputs the current coupling cycle.

  1. Create a report of volume averaged fluid temperature:
    1. Right-click the Reports node and select New > Metrics > Volume Average.
    2. Rename the report to VA_T_Fluid.
    3. Select the VA_T_Fluid node and set the properties as follows:
      Property Setting
      Unit C
      Field Function Temperature
      Parts Exhaust Gas
    4. Right-click the report and select Create Monitor from Report.
  2. Since the VA_T_Solid Monitor was created in a previous step for the solid stopping criterion, you create a single plot for both volume averaged temperature monitors:
    1. Multi-select the Monitors > VA_T_Fluid Monitor and VA_T_Solid Monitor nodes, right-click one of them and select Create Plot from Monitor .
    2. Select Single Plot in the Create Plot From Monitors dialog.
    3. Rename the plot to Volume Averaged Temperature (C).
    4. Select the Volume Averaged Temperature (C) node and set Title to be the same, that is, Volume Averaged Temperature (C).
The boundary heat flux is the key physical quantity you use to monitor the heat transfer through the contact interface. When it approaches a constant value, the Boundary Heat Flux and Specified Y+ Heat Transfer Coefficient can be exchanged across the interface. From fluid to solid, the time-averaged values are mapped. From solid to fluid, the instantaneous values are mapped.
  1. Create a report of Surface Averaged Instantaneous Boundary Heat Flux of the solid side of the contact interface:
    1. Right-click the Reports node and select New > Metrics > Surface Average.
    2. Rename the report Surface Average 1 to SA_INS_BoundaryHeatFlux.
    3. Select the SA_INS_BoundaryHeatFlux node and set the properties as follows:
      Property Setting
      Field Function Boundary Heat Flux
      Parts Regions > Manifold Solid > Faces[Manifold Solid/Exhaust Gas]
  2. To create a single plot from the boundary heat flux reports:
    1. Right-click the Reports > SA_INS_BoundaryHeatFlux node and select Create Monitor from Report.
    2. Within the Monitors node, multi-select the SA_TA_BoundaryHeatFlux Monitor and SA_INS_BoundaryHeatFlux Monitor nodes, right-click and select Create Plot from Monitor.
    3. Select Single Plot in the Create Plot From Monitors dialog.
    4. Rename the created plot Reports Plot to Boundary Heat Flux; select the plot node and set Title to the same.
  3. To update the pre-defined scalar scene Temperature:
    1. Select the Scenes > Temperature > Scalar 1 > Scalar Field node and set the properties as follows:
      Property Setting
      Function Temperature
      Clip Off
      Units C
      Min 500.0 C
      Max 700.0 C
  4. To run the simulation operations, first activate the Multiple Timescale CHT with one of the following options:
    • Select the icon on the toolbar and select Multiple Timescale CHT from the drop-down menu.
    • Right-click the Automation > Simulation Operations > Multiple Timescale CHT node and select Activate.
To start the managed simulation:
  1. Right-click the Automation > Simulation Operations > Multiple Timescale CHT and select Play/Resume Simulation Operations.
    The simulation starts with the fluid time scale until the associated stopping criterion is fulfilled. The solid time scale is then activated subsequently.
    Note To stop the workflow, click on Stop on the tool bar. To restart solver iterating, right-click again the Multiple Timescale CHT node and select Play/Resume.
  2. Save the simulation.