Note
Go to the end to download the full example code
Modeling Cavitation#
This example examines the pressure-driven cavitating flow of water through a sharp-edged orifice. This is a typical configuration in fuel injectors, and brings a challenge to the physics and numerics of cavitation models because of the high pressure differentials involved and the high ratio of liquid to vapor density.
This example uses the multiphase modeling capability of Ansys Fluent, and will be able to predict the strong cavitation near the orifice after flow separation at a sharp edge.
Workflow tasks
This example demonstrates how to do the following:
Set boundary conditions for internal flow
Use the mixture model with cavitation effects
Calculate a solution using the pressure-based coupled solver
Problem description
The problem considers the cavitation caused by the flow separation after a sharp-edged orifice. The flow is pressure driven, with an inlet pressure of 500 kPa and an outlet pressure of 95 kPa. The orifice diameter is 4 mm, and the geometrical parameters of the orifice are D/d = 2.88 and L/d = 4, where D, d, and L are the inlet diameter, orifice diameter, and orifice length respectively.
Example Setup#
Before you can begin, you must set up the example and initialize this workflow.
Launch Fluent#
Perform required imports, which includes downloading and importing the geometry file.
import ansys.fluent.core as pyfluent
from ansys.fluent.core import examples
cav_file = examples.download_file("cav.msh", "pyfluent/cavitation")
Download successful. File path:
/home/ansys/.local/share/ansys_fluent_core/examples/cav.msh
Launch a Fluent session in the 2d solution mode with double precision running on four processors.
solver = pyfluent.launch_fluent(
precision="double",
processor_count=4,
mode="solver",
version="2d",
)
Read the mesh that was downloaded.
solver.file.read_mesh(file_name=cav_file)
solver.mesh.check()
Specify an axisymmetric model.
solver.setup.general.solver.two_dim_space = "axisymmetric"
Enable the multiphase mixture model.
solver.setup.models.multiphase.models = "mixture"
solver.tui.define.models.multiphase.mixture_parameters("no", "implicit")
Enable the k-ω SST turbulence model.
solver.setup.models.viscous = {"model": "k-omega", "k_omega_model": "sst"}
Define materials#
Create a material named water, using 1000 kg/m3 for density and 0.001 kg/m–s for viscosity. Then, copy water vapor properties from the database and modify the copy by changing the density to 0.02558 kg/m3 and the viscosity to 1.26e-06 kg/m–s.
water = {
"density": {"option": "constant", "value": 1000},
"viscosity": {"option": "constant", "value": 0.001},
}
solver.setup.materials.fluid["water"] = water
solver.setup.materials.database.copy_by_name(type="fluid", name="water-vapor")
water_vapor = {"density": {"value": 0.02558}, "viscosity": {"value": 1.26e-06}}
solver.setup.materials.fluid["water-vapor"] = water_vapor
Phases#
Change the name of the primary phase to “liquid” and the secondary phase to “water-vapor”. Then, enable the cavitation model and set the number of mass transfer mechanisms to 1. Finally, specify cavitation as a mass transfer mechanism occurring from the liquid to the vapor.
solver.tui.define.phases.set_domain_properties.change_phases_names("vapor", "liquid")
solver.tui.define.phases.set_domain_properties.phase_domains.liquid.material(
"yes", "water"
)
solver.tui.define.phases.set_domain_properties.phase_domains.vapor.material(
"yes", "water-vapor"
)
solver.tui.define.phases.set_domain_properties.interaction_domain.heat_mass_reactions.mass_transfer(
1, "liquid", "vapor", "cavitation", "1", "no", "no", "no"
)
Boundary Conditions#
For the first inlet momentum boundary conditions set the direction specification method to ‘normal to boundary’, gauge total pressure as 500 kPa and supersonic or initial gauge pressure as 449 kPa.
For the turbulence settings choose ‘Intensity and Viscosity Ratio’ for turbulent specification. Set turbulent intensity and turbulent viscosity ratio to 0.05 and 10 respectively.
inlet_1 = solver.setup.boundary_conditions.pressure_inlet["inlet_1"].phase
in_mixture = {
"direction_spec": "Normal to Boundary",
"gauge_total_pressure": {"value": 500000},
"gauge_pressure": {"value": 449000},
"turb_intensity": 0.05,
"ke_spec": "Intensity and Viscosity Ratio",
"turb_viscosity_ratio": 10,
}
inlet_1["mixture"] = in_mixture
Before copying inlet_1’s boundary conditions to inlet_2, set the vapor fraction to 0.
inlet_1["vapor"] = {"volume_fraction": {"value": 0}}
solver.setup.boundary_conditions.copy(from_="inlet_1", to="inlet_2")
For the outlet boundary conditions, set the gauge pressure as 95 kPa. Use the same turbulence and volume fraction settings as the inlets.
outlet = solver.setup.boundary_conditions.pressure_outlet["outlet"].phase
out_mixture = {
"gauge_pressure": {"value": 95000},
"turb_intensity": 0.05,
"ke_spec": "Intensity and Viscosity Ratio",
"turb_viscosity_ratio": 10,
}
outlet["mixture"] = out_mixture
outlet["vapor"] = {"volume_fraction": {"value": 0}}
Operating Conditions#
Set the operating pressure to 0.
solver.setup.general.operating_conditions.operating_pressure = 0
Solution#
To configure the discretization scheme, set ‘first order upwind’ method for turbulent kinetic energy and turbulent dissipation rate, ‘quick’ for the momentum and volume fraction, and ‘presto!’ for pressure.
methods = solver.solution.methods
discretization_scheme = {
"k": "first-order-upwind",
"mom": "quick",
"mp": "quick",
"omega": "first-order-upwind",
"pressure": "presto!",
}
methods.discretization_scheme = discretization_scheme
For the pressure velocity coupling scheme choose ‘Coupled’. Set the pseudo time step method to ‘global time step’ and enable ‘High Order Term Relaxation’. Then, set the explicit relaxation factor for ‘Volume Fraction’ to 0.3.
methods.p_v_coupling.flow_scheme = "Coupled"
methods.pseudo_time_method.formulation.coupled_solver = "global-time-step"
methods.high_order_term_relaxation.enable = True
solver.solution.controls.pseudo_time_explicit_relaxation_factor.global_dt_pseudo_relax[
"mp"
] = 0.3
To plot the residuals, enable plotting and set the convergence criteria to 1e-05 for x-velocity, y-velocity, k, omega, and vf-vapor. Enable the specified initial pressure then initialize the solution with hybrid initialization.
solver.tui.solve.monitors.residual.plot("yes")
solver.tui.solve.monitors.residual.convergence_criteria(
1e-05, 1e-05, 1e-05, 1e-05, 1e-05, 1e-05
)
solver.solution.initialization.hybrid_init_options.general_settings.initial_pressure = (
True
)
solver.solution.initialization.hybrid_initialize()
Save and Run#
Save the case file ‘cav.cas.h5’. Then, start the calculation by requesting 500 iterations. Save the final case file and the data.
solver.file.write(file_name="cav", file_type="case")
solver.solution.run_calculation.iterate(iter_count=500)
solver.file.write(file_name="cav", file_type="case-data")
Post Processing#
Create a contour plot for static pressure, turbulent kinetic energy and the volume fraction of water vapor. For each plot enable banded coloring and filled option.
solver.results.graphics.contour.create("contour_static_pressure")
contour_static_pressure = {
"coloring": {"option": "banded", "smooth": False},
"field": "pressure",
"filled": True,
}
solver.results.graphics.contour["contour_static_pressure"] = contour_static_pressure
Mirror the display around the symmetry plane to show the full model.
solver.tui.display.set.mirror_zones(["symm_2", "symm_1"])
solver.results.graphics.contour["contour_static_pressure"].display()
solver.results.graphics.picture.save_picture(file_name="contour_static_pressure.png")
solver.results.graphics.contour.create("contour_tke")
contour_tke = {
"coloring": {"option": "banded", "smooth": False},
"field": "turb-kinetic-energy",
"filled": True,
}
solver.results.graphics.contour["contour_tke"] = contour_tke
solver.results.graphics.contour["contour_tke"].display()
solver.results.graphics.picture.save_picture(file_name="contour_tke.png")
solver.results.graphics.contour.create("contour_vf_vapor")
contour_vf_vapor = {
"coloring": {"option": "banded", "smooth": False},
"field": "vapor-vof",
"filled": True,
}
solver.results.graphics.contour["contour_vf_vapor"] = contour_vf_vapor
solver.results.graphics.contour["contour_vf_vapor"].display()
solver.results.graphics.picture.save_picture(file_name="contour_vf_vapor.png")
# Save case to 'cav.cas.h5' and exit
solver.file.write(file_name="cav", file_type="case")
solver.exit()
Total running time of the script: (1 minutes 21.187 seconds)