This is a quick-reference guide for PyFluent. You can jump to a section of your choosing by using these links:
Launching Fluent | Import Mesh in Launched Session | Enable Heat Transfer Physics | Accessing the Object State Using pprint | Define materials | Define Boundary Conditions | Modify Cell Zone Conditions | Apply Solution Settings
Launching Fluent Locally
The following method is used to start Fluent from Python in gRPC mode. This code starts Fluent in the background so that commands can be sent to Fluent from the Python interpreter.
import ansys.fluent.core as pyfluent
solver=pyfluent.launch_fluent(mode="solver", show_gui=True) The solver object contains attributes such as file, setup, solution, and results, which are also instances of settings objects.
Import Mesh in Launched Session
The following examples show how to read the available mesh file in Fluent Session.
import_filename='example_file.msh.h5'
solver.file.read(file_type="case", file_name= import_filename) There are other specific Client Libraries available for reading case files and reading case-datafiles.
# e.g., read_case(), read_case_data()
import_filename = 'example_file.cas.h5'
solver.file.read_case(file_type="case", file_name=import_filename)
Enable heat transfer physics
The following examples show how to enable heat transfer by activating the energy equation.
solver.setup.models.energy.enabled = True
Accessing the Object State Using pprint
>>> from pprint import pprint
>>> pprint(solver.setup.models.energy())
{'enabled':True,
'inlet_diffusion': True,
'kinetic_energy': False,
'pressure_work': False,
'viscous_dissipation': False}
Define materials
This example shows how to use solver settings objects to define materials.
solver.setup.materials.copy_database_material_by_name(type="fluid", name="water-liquid")
solver.setup.cell_zone_conditions.fluid["elbow-fluid" ].material = "water-liquid"
Define Boundary Conditions
The examples in this section show how you use solver settings objects to define boundary conditions.
solver.setup.boundary_conditions.velocity_inlet["coldinlet"].vmag = {
"option": "constantorexpression",
"constant": 0.4,
}
solver.setup.boundary_conditions.velocity_inlet["cold-inlet"].ke_spec = "IntensityandHydraulicDiameter"
solver.setup.boundary_conditions.velocity_inlet["coldinlet"].turb_intensity = 5
solver.setup.boundary_conditions.velocity_inlet[ "cold-inlet" ].turb_hydraulic_diam = "4[in]"
solver.setup.boundary_conditions.velocity_inlet["coldinlet"].t = { "option": "constantorexpression", "constant": 293.15}
Modify Cell Zone Conditions
The examples in this section show how you use solver settings objects to modify cell zone conditions.
# Enabling Laminar Zone
solver.setup.cell_zone_conditions.fluid["elbow-fluid"] = {"laminar": True}
Apply Solution Settings
PyFluent allows you to use solver settings objects to apply solution settings, initialize, and solve.
solver.solution.initialization.hybrid_initialize()
solver.solution.run_calculation.iterate(number_of_iterations=150)
Post-Processing
PyFluent allows you to post-process data with the results object. The following example shows you how to create and display contours on a plane.
solver.results.graphics.contour["contour"] = {}
solver.results.graphics.contour["contour"].print_state()
solver.results.graphics.contour["contour"].field = " temperature"
solver.results.graphics.contour["contour"]. surfaces_list = [ "symmetry-xyplane"]
Temperature Contour
