Quick Start

This guide provides a fundamental illustration of the Flow360 Python API workflow, commencing with geometry definition and proceeding through simulation setup, execution, and basic results visualization. The example script demonstrates a streamlined process suitable for initiating straightforward CFD analyses.

The script executes the following sequential steps:

1. Project Initialization: Creates a new Flow360 project from a predefined geometry file.

2. Geometry Inspection: Displays available geometric groupings to aid in boundary condition assignment.

3. Face Grouping: Organizes geometry faces based on tags, facilitating the definition of Surface objects.

4. Simulation Parameter Definition: Configures the simulation settings within the SI unit system context, including meshing parameters, operating conditions, numerical schemes, physical models, and output specifications. It utilizes an AutomatedFarfield component for simplified boundary setup.

5. Simulation Execution: Submits the defined simulation case for execution.

6. Results Retrieval and Visualization: Waits for simulation completion, retrieves key aerodynamic coefficients (CL, CD), and generates a basic plot of their convergence history.

The complete script is presented below:

# Import necessary modules from the Flow360 library
from matplotlib.pyplot import show

import flow360 as fl
from flow360.examples import Airplane

# Step 1: Create a new project from a predefined geometry file in the Airplane example
# This initializes a project with the specified geometry and assigns it a name.
project = fl.Project.from_geometry(
    Airplane.geometry,
    name="Python Project (Geometry, from file)",
)
geo = project.geometry  # Access the geometry of the project

# Step 2: Display available groupings in the geometry (helpful for identifying group names)
geo.show_available_groupings(verbose_mode=True)

# Step 3: Group faces by a specific tag for easier reference in defining `Surface` objects
geo.group_faces_by_tag("groupName")

# Step 4: Define simulation parameters within a specific unit system
with fl.SI_unit_system:
    # Define an automated far-field boundary condition for the simulation
    far_field_zone = fl.AutomatedFarfield()

    # Set up the main simulation parameters
    params = fl.SimulationParams(
        # Meshing parameters, including boundary layer and maximum edge length
        meshing=fl.MeshingParams(
            defaults=fl.MeshingDefaults(
                boundary_layer_first_layer_thickness=0.001,  # Boundary layer thickness
                surface_max_edge_length=1,  # Maximum edge length on surfaces
            ),
            volume_zones=[far_field_zone],  # Apply the automated far-field boundary condition
        ),
        # Reference geometry parameters for the simulation (e.g., center of pressure)
        reference_geometry=fl.ReferenceGeometry(),
        # Operating conditions: setting speed and angle of attack for the simulation
        operating_condition=fl.AerospaceCondition(
            velocity_magnitude=100,  # Velocity of 100 m/s
            alpha=5 * fl.u.deg,  # Angle of attack of 5 degrees
        ),
        # Time-stepping configuration: specifying steady-state with a maximum step limit
        time_stepping=fl.Steady(max_steps=1000),
        # Define models for the simulation, such as walls and freestream conditions
        models=[
            fl.Wall(
                surfaces=[geo["*"]],  # Apply wall boundary conditions to all surfaces in geometry
            ),
            fl.Freestream(
                surfaces=[
                    far_field_zone.farfield
                ],  # Apply freestream boundary to the far-field zone
            ),
        ],
        # Define output parameters for the simulation
        outputs=[
            fl.SurfaceOutput(
                surfaces=geo["*"],  # Select all surfaces for output
                output_fields=["Cp", "Cf", "yPlus", "CfVec"],  # Output fields for post-processing
            )
        ],
    )

# Step 5: Run the simulation case with the specified parameters
project.run_case(params=params, name="Case of Simple Airplane from Python")

# Step 6: wait for results and plot CL, CD when available
case = project.case
case.wait()

total_forces = case.results.total_forces.as_dataframe()
total_forces.plot("pseudo_step", ["CL", "CD"], ylim=[-5, 15])
show()

Notes

• Utilize the AutomatedFarfield component for streamlined setup of farfield boundary conditions.

• Ensure physical quantities are defined within the with fl.SI_unit_system: or other context manager for correct unit handling. Specify units explicitly where needed using fl.u (e.g., alpha=5 * fl.u.deg).

• Access simulation outputs and results data through the case.results attribute (e.g., case.results.total_forces) for post-processing and analysis.