3.3. Quick Start

Complete work procedures, with example dataset and conditions, are available as a separate tutorial guide - Fluent Aero Tutorials.

To Set-up and Run Simulations with Fluent Aero

  • Launch Fluent on your computer. In the Fluent Launcher window that appears, set the Capability Level to Enterprise. Select Aero from the left panel. Set the number of Solver Processes, and click Start.

  • In the Fluent Aero user interface, in the Project ribbon, select Workspaces → Options. A drop down menu will appear. For a typical run on your local machine, ensure that all options are disabled. Specifically, if you would like to calculate your simulations on your local machine, ensure that Use Custom Solver Launch Settings is disabled.

    • These options and more are also available from File → Preferences... within the Preferences window, in Fluent Aero's main menu.

  • In the Project ribbon, select Project → New, and choose an appropriate name and location for the project file, and click OK.

  • Go to Simulations → New Aero Workflow, and select a suitable (.cas, .cas.h5) file.

    Note:  This case file must:

    • Contain a 3D mesh that is oriented such that the geometry is aligned with a cartesian axis.

    • For a Freestream type domain, contain a pressure-farfield or a pressure-farfield with a pressure outlet type boundary to define the main flow inlet/outlet boundary conditions.

    • For a WindTunnel type domain, contain mass-flow-inlet or a velocity-inlet to define the main flow inlet boundary conditions and a pressure-outlet type boundary to define the main flow outlet boundary conditions of the test section in the tunnel, and wall, symmetry, or periodic type boundary conditions to define the side boundaries of this test section. Name these boundaries windtunnel-inlet, windtunnel-outlet, windtunnel-wall*, windtunnel-symm* and windtunnel-periodic* to ensure that the automatic domain type setup works properly.

    • Be set to material type (Air.)

  • A new simulation is created. When prompted, choose an appropriate name for the new simulation. Enable Load in Solver and select OK. A simulation folder with the chosen name is then created inside the project, and the case file is loaded into a remote solver session.

  • Once the solver is loaded, the Project ribbon view will be displayed. Use the aero application to review and apply the conditions and settings.

    • Geometric Properties

      • Ensure the correct domain type for your geometry has been selected (Freestream or WindTunnel).

      • Define the geometric grid orientation with respect to the cartesian axis, and the reference length and area.

    • Airflow Physics

      • Solver: Choose between Pressure-based or Density-based Fluent solver types.

      • Models: Choose the Viscous model. If the Density-based solver is selected, the Two Temperature model becomes available.

      • Materials: Select the fluid materials for your simulation.

    • Simulation Conditions

      • Choose the input Parameter types and set up the atmospheric Flight Conditions to use in your simulation for each Design Point.

      • Choose a Distribution for each parameter

        • Constant: Specify conditions that will be common to all Design Points.

        • Uniform: Specify conditions that will vary uniformly per Design Point.

        • Custom: Specify conditions that will vary non-uniformly per Design Point.

      • Use the Input: Design Points table to set the custom input values for each design point.

    • Component Groups

      • Organize the domain’s boundary zones into aircraft Component Groups, such as Wing, Engine, Fuselage, etc., to help the setup of boundary conditions and the analysis of individual aircraft components.

      • Ensure that the Freestream or WindTunnel group correctly defines the external boundary of your domain.

      • Specify zone specific boundary conditions (such as a mass flow on an engine exhaust).

    • Files

      • Select which types of output files to save per design point. Reduce the amount of disk space the consumed by large simulations by disabling Write Case Files and Write Solution Files. Alternatively, choose to Autosave Intermediate Solution Files or Write Post Files to obtain additional solutions to post process your results.

    • Solve

      • Set the number of Iterations to run for each design point.

      • Keep Convergence Settings to Default or Robust to use Fluent Aero’s default CFD solver parameters. Set Convergence Settings to Custom if you would like to change the default value of various CFD solver parameters.

  • Once the appropriate conditions and settings are applied, click Solve and then click Update to start the calculations.

  • Once the simulation has started, monitor them using the Convergence window. A Results node becomes available in the Outline View tree – use the various Tables, Graphs, Plots and Contours options to investigate the results.