# PyFluent - Python Interface for Ansys Fluent

PyFluent provides comprehensive Pythonic access to Ansys Fluent's computational fluid dynamics (CFD) capabilities. This library enables seamless integration of Fluent within the Python ecosystem, allowing users to automate simulation workflows, perform parametric studies, and extract field data programmatically. PyFluent supports both solver and meshing operations, offering access to Fluent's text user interface (TUI) commands, settings API, workflow automation, and built-in postprocessing capabilities.

The library is designed for engineers and researchers who need to integrate CFD simulations into broader Python-based workflows, automate repetitive tasks, run parametric studies at scale, or build custom applications on top of Fluent's powerful simulation engine. PyFluent supports various deployment modes including local standalone execution, Docker containers, and HPC cluster environments with job schedulers like Slurm.

## Launching Fluent and Creating Sessions

### launch_fluent - Start a Fluent Session

Start a new Fluent session locally or in a containerized environment with full control over simulation parameters.

```python
import ansys.fluent.core as pyfluent
from ansys.fluent.core import examples

# Launch solver session with double precision on 4 processors
solver = pyfluent.launch_fluent(
    product_version="25.1",
    dimension=pyfluent.Dimension.THREE,
    precision="double",
    processor_count=4,
    mode="solver",
    ui_mode=pyfluent.UIMode.NO_GUI
)

# Download and load example mesh
mesh_file = examples.download_file("mixing_elbow.msh.h5", "pyfluent/mixing_elbow")
solver.settings.file.read_case(file_name=mesh_file)

# Verify mesh quality
solver.mesh.check()
print(f"Connected to Fluent {solver.get_fluent_version()}")

# Perform simulation setup and solve
solver.settings.models.energy.enabled = True
solver.settings.solution.initialization.hybrid_initialize()
solver.settings.solution.run_calculation.iterate(iter_count=100)

# Cleanup
solver.exit()
```

### connect_to_fluent - Connect to Existing Session

Connect to a running Fluent instance using IP, port, and password or server-info file.

```python
import ansys.fluent.core as pyfluent

# Connect using explicit connection parameters
solver = pyfluent.connect_to_fluent(
    ip="192.168.1.100",
    port=12345,
    password="fluent_password"
)

# Or connect using server-info file
solver = pyfluent.connect_to_fluent(
    server_info_file_name="/path/to/serverinfo-fluent.txt",
    cleanup_on_exit=False  # Don't shutdown Fluent when done
)

# Use the connected session
print(f"Server healthy: {solver.is_server_healthy()}")
solver.tui.mesh.check()
```

### launch_fluent with Advanced Options

Launch Fluent with GPU acceleration, container configuration, and HPC scheduler integration.

```python
import ansys.fluent.core as pyfluent

# Launch with GPU solver using specific GPUs
solver = pyfluent.launch_fluent(
    mode="solver",
    processor_count=4,
    gpu=[0, 1],  # Use GPU 0 and 1
    precision="double"
)

# Launch in Docker container with custom configuration
solver = pyfluent.launch_fluent(
    container_dict={
        "image": "ghcr.io/ansys/fluent:25.1",
        "mount_source": "/home/user/fluent_data",
        "mount_target": "/fluent_data"
    },
    cwd="/fluent_data",
    processor_count=2
)

# Launch on Slurm cluster (returns SlurmFuture)
slurm_future = pyfluent.launch_fluent(
    scheduler_options={
        "scheduler": "slurm",
        "scheduler_headnode": "cluster-head.domain.com",
        "scheduler_queue": "standard",
        "scheduler_account": "research_project"
    },
    processor_count=16,
    mode="solver"
)
solver = slurm_future.result()  # Wait for job allocation and startup
```

## Settings API for Solver Configuration

### Material and Cell Zone Configuration

Configure fluid properties and assign materials to cell zones using the hierarchical settings API.

```python
import ansys.fluent.core as pyfluent

solver = pyfluent.launch_fluent(mode="solver", processor_count=2)
solver.settings.file.read_case(file_name="mixing_elbow.cas.h5")

# Enable energy equation
solver.settings.models.energy.enabled = True

# Import material from database
solver.settings.materials.database.copy_by_name(
    type="fluid",
    name="water-liquid"
)

# Assign material to cell zone
solver.settings.cell_zone_conditions.fluid["elbow-fluid"].material = "water-liquid"

# Configure turbulence model
solver.settings.models.viscous.model = "k-omega"
solver.settings.models.viscous.k_omega_options.model = "sst"

# Verify configuration
print(f"Energy model enabled: {solver.settings.models.energy.enabled}")
print(f"Fluid material: {solver.settings.cell_zone_conditions.fluid['elbow-fluid'].material}")
```

### Boundary Conditions Setup

Define inlet, outlet, and wall boundary conditions with momentum and thermal specifications.

```python
import ansys.fluent.core as pyfluent

solver = pyfluent.launch_fluent(mode="solver", processor_count=2)
solver.settings.file.read_case(file_name="elbow.cas.h5")
solver.settings.models.energy.enabled = True

# Configure cold inlet
cold_inlet = solver.settings.boundary_conditions.velocity_inlet["cold-inlet"]
cold_inlet.momentum.velocity_magnitude.value = 0.4  # m/s
cold_inlet.thermal.temperature.value = 293.15  # K (20°C)
cold_inlet.turbulence.turbulence_specification = "Intensity and Hydraulic Diameter"
cold_inlet.turbulence.turbulent_intensity = 0.05
cold_inlet.turbulence.hydraulic_diameter.value = 0.1  # meters

# Configure hot inlet
hot_inlet = solver.settings.boundary_conditions.velocity_inlet["hot-inlet"]
hot_inlet.momentum.velocity_magnitude.value = 1.2  # m/s
hot_inlet.thermal.temperature.value = 313.15  # K (40°C)

# Configure pressure outlet
outlet = solver.settings.boundary_conditions.pressure_outlet["outlet"]
outlet.momentum.gauge_pressure.value = 0  # Pa

# Configure wall with heat flux
wall = solver.settings.boundary_conditions.wall["elbow-wall"]
wall.thermal.thermal_condition = "Heat Flux"
wall.thermal.heat_flux.value = 1000  # W/m²

print("Boundary conditions configured successfully")
```

### Solution Initialization and Execution

Initialize flow field and run iterative calculations with residual monitoring.

```python
import ansys.fluent.core as pyfluent
from ansys.fluent.core.streaming_services.events_streaming import SolverEvent

solver = pyfluent.launch_fluent(mode="solver", processor_count=4)
solver.settings.file.read_case(file_name="configured_case.cas.h5")

# Set solution methods
solver.settings.solution.methods.p_v_coupling.scheme = "Coupled"
solver.settings.solution.methods.discretization_scheme.pressure = "Second Order"
solver.settings.solution.methods.discretization_scheme.momentum = "Second Order Upwind"
solver.settings.solution.methods.discretization_scheme.energy = "Second Order Upwind"

# Configure solution controls
solver.settings.solution.controls.advanced.enable_pseudo_time_method = True
solver.settings.solution.controls.pseudo_time_settings.time_step_method = "Automatic"

# Register callback for iteration monitoring
def on_iteration(session, event_info):
    print(f"Iteration {event_info.index} completed")

solver.events.register_callback(SolverEvent.ITERATION_ENDED, on_iteration)

# Initialize solution
print("Initializing solution...")
solver.settings.solution.initialization.hybrid_initialize()

# Run calculation
print("Running calculation...")
solver.settings.solution.run_calculation.iterate(iter_count=500)

# Save results
solver.settings.file.write_case_data(file_name="converged_solution.cas.h5")
```

## Field Data Extraction and Post-Processing

### Scalar Field Data Extraction

Extract scalar field data (pressure, temperature, density) from surfaces with boundary values.

```python
import ansys.fluent.core as pyfluent
from ansys.fluent.core import ScalarFieldDataRequest
import numpy as np

solver = pyfluent.launch_fluent(mode="solver", processor_count=2)
solver.settings.file.read_case_data(file_name="solved_case.cas.h5")

# Request temperature data from wall surfaces
request = ScalarFieldDataRequest(
    field_name="temperature",
    surfaces=["hot-inlet", "cold-inlet", "elbow-wall"],
    node_value=True,
    boundary_value=True
)

# Get field data
data = solver.fields.field_data.get_field_data(request)

# Process results
for surface_name, surface_data in data.items():
    temps = surface_data['temperature']
    print(f"\nSurface: {surface_name}")
    print(f"  Temperature range: {np.min(temps):.2f} - {np.max(temps):.2f} K")
    print(f"  Average temperature: {np.mean(temps):.2f} K")
    print(f"  Data points: {len(temps)}")
```

### Vector Field Data Extraction

Extract vector field data (velocity, momentum) from specified surfaces with magnitude calculations.

```python
import ansys.fluent.core as pyfluent
from ansys.fluent.core import VectorFieldDataRequest
import numpy as np

solver = pyfluent.launch_fluent(mode="solver", processor_count=2)
solver.settings.file.read_case_data(file_name="flow_solution.cas.h5")

# Request velocity vectors from inlet
request = VectorFieldDataRequest(
    field_name="velocity",
    surfaces=["inlet", "outlet"]
)

velocity_data = solver.fields.field_data.get_field_data(request)

# Calculate velocity magnitudes
for surface_name, surface_data in velocity_data.items():
    vel_x = surface_data['velocity'][0]  # X-component
    vel_y = surface_data['velocity'][1]  # Y-component
    vel_z = surface_data['velocity'][2]  # Z-component

    magnitude = np.sqrt(vel_x**2 + vel_y**2 + vel_z**2)

    print(f"\n{surface_name}:")
    print(f"  Max velocity: {np.max(magnitude):.3f} m/s")
    print(f"  Min velocity: {np.min(magnitude):.3f} m/s")
    print(f"  Mean velocity: {np.mean(magnitude):.3f} m/s")
```

### Surface Data Extraction with Connectivity

Extract surface mesh data including vertices, face connectivity, normals, and centroids.

```python
import ansys.fluent.core as pyfluent
from ansys.fluent.core import SurfaceFieldDataRequest, SurfaceDataType

solver = pyfluent.launch_fluent(mode="solver", processor_count=2)
solver.settings.file.read_case_data(file_name="case.cas.h5")

# Request comprehensive surface data
request = SurfaceFieldDataRequest(
    data_types=[
        SurfaceDataType.Vertices,
        SurfaceDataType.FacesConnectivity,
        SurfaceDataType.FacesNormal,
        SurfaceDataType.FacesCentroid
    ],
    surfaces=["wall-1", "inlet"],
    overset_mesh=False,
    flatten_connectivity=True
)

surface_data = solver.fields.field_data.get_field_data(request)

# Process mesh topology
for surface_name, data in surface_data.items():
    vertices = data['vertices']  # Nx3 array of vertex coordinates
    connectivity = data['faces']  # Face-to-vertex connectivity
    normals = data['face-normal']  # Face normal vectors
    centroids = data['face-centroid']  # Face centroids

    print(f"\n{surface_name}:")
    print(f"  Vertices: {vertices.shape}")
    print(f"  Faces: {len(connectivity)}")
    print(f"  Normals: {normals.shape}")
```

### Batch Field Data Requests

Create batched requests for multiple fields to optimize data transfer performance.

```python
import ansys.fluent.core as pyfluent
from ansys.fluent.core import (
    ScalarFieldDataRequest,
    VectorFieldDataRequest,
    SurfaceFieldDataRequest,
    SurfaceDataType
)

solver = pyfluent.launch_fluent(mode="solver", processor_count=2)
solver.settings.file.read_case_data(file_name="results.cas.h5")

# Create batch with multiple requests
batch = solver.fields.field_data.new_batch()

# Add multiple field requests
batch.add_requests(
    ScalarFieldDataRequest(field_name="pressure", surfaces=["inlet", "outlet"]),
    ScalarFieldDataRequest(field_name="temperature", surfaces=["wall"]),
    VectorFieldDataRequest(field_name="velocity", surfaces=["inlet"]),
    SurfaceFieldDataRequest(
        data_types=[SurfaceDataType.Vertices, SurfaceDataType.FacesConnectivity],
        surfaces=["wall"]
    )
)

# Execute all requests in single transaction
results = batch.get_response()

# Access results by request type
pressure_data = results['ScalarFieldDataRequest']['pressure']
temperature_data = results['ScalarFieldDataRequest']['temperature']
velocity_data = results['VectorFieldDataRequest']['velocity']
surface_mesh = results['SurfaceFieldDataRequest']['wall']

print(f"Retrieved {len(results)} field data types in batch")
```

### Pathlines Generation and Extraction

Generate and extract pathline data for flow visualization with particle tracking.

```python
import ansys.fluent.core as pyfluent
from ansys.fluent.core import PathlinesFieldDataRequest

solver = pyfluent.launch_fluent(mode="solver", processor_count=2)
solver.settings.file.read_case_data(file_name="flow_field.cas.h5")

# Configure pathlines request
request = PathlinesFieldDataRequest(
    field_name="velocity-magnitude",
    surfaces=["inlet"],
    steps=1000,
    step_size=0.001,  # seconds
    skip=0,
    reverse=False,
    zones=None,
    accuracy_control_on=True,
    tolerance=0.001
)

# Generate and extract pathlines
pathlines_data = solver.fields.field_data.get_field_data(request)

# Process pathline results
vertices = pathlines_data['vertices']  # All pathline points
lines = pathlines_data['lines']  # Connectivity for each pathline
velocities = pathlines_data['velocity-magnitude']  # Field values along paths
particle_time = pathlines_data['particle-time']  # Time at each point

print(f"Generated {len(lines)} pathlines")
print(f"Total pathline points: {len(vertices)}")
print(f"Velocity range: {velocities.min():.3f} - {velocities.max():.3f} m/s")
```

## Parametric Studies and Design Exploration

### Local Parametric Study Definition

Define parametric studies locally with multiple design points before submitting to Fluent.

```python
from ansys.fluent.core.parametric import LocalParametricStudy
import ansys.fluent.core as pyfluent

# Create local parametric study from case file
study = LocalParametricStudy(case_filepath="/path/to/elbow_parametric.cas.h5")

# Configure base design point
base_dp = study.design_point("Base DP")
base_dp.input_parameters['inlet_velocity'] = 1.0
base_dp.input_parameters['inlet_temperature'] = 300.0

# Add design points with varying parameters
for i in range(1, 21):
    dp = study.add_design_point(f"design_point_{i}")
    dp.input_parameters['inlet_velocity'] = 0.5 + (i * 0.1)  # 0.6 to 2.5 m/s
    dp.input_parameters['inlet_temperature'] = 290 + (i * 2)  # 292 to 330 K

# Display study configuration
print(f"Total design points: {len(study.design_point_table)}")
for dp in study.design_point_table[:3]:
    print(f"{dp.name}: velocity={dp.input_parameters['inlet_velocity']:.2f}, "
          f"temp={dp.input_parameters['inlet_temperature']:.1f}")
```

### Running Parametric Studies in Parallel

Execute parametric studies across multiple Fluent instances for parallel evaluation.

```python
from ansys.fluent.core.parametric import LocalParametricStudy

# Create and configure study (as shown above)
study = LocalParametricStudy(case_filepath="parametric_case.cas.h5")
base_dp = study.design_point("Base DP")
base_dp.input_parameters['inlet_velocity'] = 1.0

for i in range(1, 51):
    dp = study.add_design_point(f"dp_{i}")
    dp.input_parameters['inlet_velocity'] = i * 0.05

# Run study on 8 parallel Fluent servers
print("Starting parametric study execution...")
study.run_in_fluent(
    num_servers=8,
    start_transcript=False,
    capture_report_data=True
)

# Process results
print("\nParametric Study Results:")
print("-" * 80)
for dp in study.design_point_table:
    vel = dp.input_parameters['inlet_velocity']

    # Output parameters populated after execution
    if dp.output_parameters:
        pressure_drop = dp.output_parameters.get('pressure_drop', 'N/A')
        avg_temp = dp.output_parameters.get('average_temperature', 'N/A')
        print(f"{dp.name}: vel={vel:.2f} m/s, ΔP={pressure_drop}, T_avg={avg_temp}")
    else:
        print(f"{dp.name}: vel={vel:.2f} m/s, Status=Not completed")
```

## Meshing Workflows and Mesh Generation

### Watertight Meshing Workflow

Create high-quality volume mesh from CAD geometry using watertight workflow.

```python
import ansys.fluent.core as pyfluent
from ansys.fluent.core import examples

# Launch meshing mode
meshing = pyfluent.launch_fluent(mode="meshing", processor_count=4)

# Download example geometry
cad_file = examples.download_file("exhaust_system.pmdb", "pyfluent/exhaust_system")

# Initialize watertight geometry workflow
meshing.workflow.InitializeWorkflow(WorkflowType="Watertight Geometry")

# Import CAD geometry
import_geom = meshing.workflow.TaskObject["Import Geometry"]
import_geom.Arguments = {"FileName": cad_file, "LengthUnit": "mm"}
import_geom.Execute()

# Add local sizing controls
add_local_sizing = meshing.workflow.TaskObject["Add Local Sizing"]
add_local_sizing.AddChildToTask()
local_sizing = meshing.workflow.TaskObject["Add Local Sizing"].TaskObject["inlet_sizing"]
local_sizing.Arguments = {
    "BOIControlName": "inlet",
    "BOIExecution": "Body Of Influence",
    "BOISize": 2.5
}
add_local_sizing.Execute()

# Generate surface mesh
generate_surface = meshing.workflow.TaskObject["Generate the Surface Mesh"]
generate_surface.Arguments = {
    "CFDSurfaceMeshControls": {
        "MinSize": 0.5,
        "MaxSize": 10.0,
        "GrowthRate": 1.2
    }
}
generate_surface.Execute()

# Improve surface mesh quality
improve_surface = meshing.workflow.TaskObject["Improve Surface Mesh"]
improve_surface.Execute()

# Generate volume mesh
generate_volume = meshing.workflow.TaskObject["Generate the Volume Mesh"]
generate_volume.Arguments = {
    "VolumeFill": "poly-hexcore",
    "VolumeFillControls": {
        "HexMaxCellLength": 15.0
    }
}
generate_volume.Execute()

# Check mesh quality
print("Mesh quality check:")
meshing.tui.mesh.check_quality()

# Switch to solver
solver = meshing.switch_to_solver()
print("Successfully switched to solver mode")
```

### Fault-Tolerant Meshing Workflow

Generate mesh from imperfect CAD geometry using fault-tolerant workflow.

```python
import ansys.fluent.core as pyfluent

# Launch meshing
meshing = pyfluent.launch_fluent(mode="meshing", processor_count=4)

# Initialize fault-tolerant workflow
meshing.workflow.InitializeWorkflow(WorkflowType="Fault-tolerant Meshing")

# Import geometry
import_cad = meshing.workflow.TaskObject["Import CAD and Part Management"]
import_cad.Arguments = {
    "FileName": "/path/to/geometry.scdoc",
    "LengthUnit": "in"
}
import_cad.Execute()

# Update regions
update_regions = meshing.workflow.TaskObject["Update Regions"]
update_regions.Execute()

# Update boundaries
update_boundaries = meshing.workflow.TaskObject["Update Boundaries"]
update_boundaries.Arguments = {
    "BoundaryLabelList": ["inlet", "outlet", "wall"],
    "BoundaryLabelTypeList": ["velocity-inlet", "pressure-outlet", "wall"]
}
update_boundaries.Execute()

# Define size functions
describe_geom = meshing.workflow.TaskObject["Describe Geometry"]
describe_geom.Arguments = {"SetupType": "The geometry consists of only fluid regions with no voids"}
describe_geom.Execute()

# Generate surface mesh
generate_surface = meshing.workflow.TaskObject["Generate the Surface Mesh"]
generate_surface.Arguments = {"SurfaceMeshControls": {"MaxSize": 5.0}}
generate_surface.Execute()

# Generate volume mesh
generate_volume = meshing.workflow.TaskObject["Generate the Volume Mesh"]
generate_volume.Execute()

# Write mesh and switch to solver
meshing.tui.file.write_mesh("fault_tolerant_mesh.msh.h5")
solver = meshing.switch_to_solver()
```

## TUI (Text User Interface) Commands

### Solver TUI Command Execution

Execute Fluent solver commands through hierarchical TUI interface for advanced operations.

```python
import ansys.fluent.core as pyfluent

solver = pyfluent.launch_fluent(mode="solver", processor_count=2)

# File operations
solver.tui.file.read_case("simulation.cas.h5")

# Mesh operations
solver.tui.mesh.check()
solver.tui.mesh.repair_improve.allow_repair_at_boundaries("yes")
solver.tui.mesh.scale(0.001, 0.001, 0.001)  # mm to m conversion

# Models configuration
solver.tui.define.models.energy("yes")
solver.tui.define.models.viscous.ke_realizable("yes")

# Material creation
solver.tui.define.materials.copy("fluid", "air")

# Boundary condition setup
solver.tui.define.boundary_conditions.velocity_inlet(
    "inlet",        # Zone name
    "yes",          # Apply to mixture
    "no",           # Turbulent intensity and length scale
    "no",           # Reference frame
    1.5,            # Velocity magnitude (m/s)
    "no",           # Temperature specified
    300             # Temperature (K)
)

# Solution settings
solver.tui.solve.set.p_v_coupling(24)  # Coupled scheme
solver.tui.solve.set.discretization_scheme.pressure(12)  # Second order
solver.tui.solve.set.discretization_scheme.mom(1)  # Second order upwind

# Initialize and solve
solver.tui.solve.initialize.hybrid_initialize()
solver.tui.solve.iterate(200)

# Report results
solver.tui.report.surface_integrals.area("inlet", "outlet")
solver.tui.report.surface_integrals.mass_flow_rate("inlet", "outlet")

# Save case and data
solver.tui.file.write_case_data("converged.cas.h5")
```

### Meshing TUI Command Execution

Execute meshing operations and quality checks using TUI commands.

```python
import ansys.fluent.core as pyfluent

meshing = pyfluent.launch_fluent(mode="meshing", processor_count=4)

# Import mesh or geometry
meshing.tui.file.import_.cad_geometry("model.scdoc", "yes")

# Mesh quality checks
meshing.tui.mesh.check_quality()
meshing.tui.mesh.smooth.smooth("surf-mesh", 20, 0.75)

# Boundary layer settings
meshing.tui.boundary.prism_settings.n_layers(5)
meshing.tui.boundary.prism_settings.first_aspect_ratio(5)
meshing.tui.boundary.prism_settings.growth_rate(1.2)

# Generate mesh
meshing.tui.mesh.poly_hexcore(
    "yes",      # Enable poly-hexcore
    "yes",      # Auto size
    2.0,        # Max cell length
    0.1         # Min cell length
)

# Write mesh file
meshing.tui.file.write_mesh("generated_mesh.msh.h5")

# Switch to solution mode
meshing.tui.switch_to_solution_mode("yes")
```

## File Session for Read-Only Access

### Read Case Files Without Launching Fluent

Access field data from case/data files without starting a full Fluent session.

```python
from ansys.fluent.core.file_session import FileSession
from ansys.fluent.core import ScalarFieldDataRequest, VectorFieldDataRequest
import numpy as np

# Open file session (lightweight, read-only)
file_session = FileSession(
    case_file_name="/path/to/solved_case.cas.h5",
    data_file_name="/path/to/solved_case.dat.h5"
)

# Access field data using same API as regular sessions
batch = file_session.field_data.new_batch()

batch.add_requests(
    ScalarFieldDataRequest(field_name="pressure", surfaces=["inlet", "outlet"]),
    ScalarFieldDataRequest(field_name="temperature", surfaces=["wall"]),
    VectorFieldDataRequest(field_name="velocity", surfaces=["inlet"])
)

# Retrieve data
data = batch.get_response()

# Process extracted data
pressure_inlet = data['ScalarFieldDataRequest']['pressure']['inlet']
pressure_outlet = data['ScalarFieldDataRequest']['pressure']['outlet']
temperature = data['ScalarFieldDataRequest']['temperature']['wall']
velocity = data['VectorFieldDataRequest']['velocity']['inlet']

print(f"Inlet pressure: {np.mean(pressure_inlet):.2f} Pa")
print(f"Outlet pressure: {np.mean(pressure_outlet):.2f} Pa")
print(f"Pressure drop: {np.mean(pressure_inlet - pressure_outlet):.2f} Pa")
print(f"Wall temperature: {np.mean(temperature):.2f} K")

# File session automatically releases resources when done
file_session.exit()
```

## Event Streaming and Monitoring

### Register Event Callbacks for Real-Time Monitoring

Monitor simulation progress with event callbacks for iterations, data reads, and case modifications.

```python
import ansys.fluent.core as pyfluent
from ansys.fluent.core.streaming_services.events_streaming import SolverEvent

solver = pyfluent.launch_fluent(mode="solver", processor_count=4)
solver.settings.file.read_case(file_name="setup.cas.h5")

# Iteration monitoring callback
def on_iteration_ended(session, event_info):
    iteration = event_info.index
    if iteration % 10 == 0:
        print(f"Completed iteration {iteration}")

# Case modification callback
def on_case_modified(session, event_info):
    print(f"Case modified at {event_info.timestamp}")

# Data read callback
def on_data_read(session, event_info):
    print(f"Data file loaded: {event_info.file_name}")

# Register callbacks
solver.events.register_callback(SolverEvent.ITERATION_ENDED, on_iteration_ended)
solver.events.register_callback(SolverEvent.CASE_MODIFIED, on_case_modified)
solver.events.register_callback(SolverEvent.DATA_READ, on_data_read)

# Run simulation with active monitoring
solver.settings.solution.initialization.hybrid_initialize()
solver.settings.solution.run_calculation.iterate(iter_count=500)

# Unregister callbacks when done
solver.events.unregister_callback(SolverEvent.ITERATION_ENDED, on_iteration_ended)
```

## Journal Recording and Playback

### Record and Execute Fluent Journals

Capture command sequences as journal files for reproducibility and automation.

```python
import ansys.fluent.core as pyfluent

solver = pyfluent.launch_fluent(mode="solver", processor_count=2)

# Start journal recording
solver.journal.start("setup_commands.jou")

# Execute commands (automatically recorded)
solver.settings.file.read_case(file_name="base_case.cas.h5")
solver.settings.models.energy.enabled = True
solver.settings.models.viscous.model = "k-epsilon"

inlet = solver.settings.boundary_conditions.velocity_inlet["inlet"]
inlet.momentum.velocity_magnitude.value = 2.0
inlet.thermal.temperature.value = 300

solver.settings.solution.initialization.hybrid_initialize()
solver.settings.solution.run_calculation.iterate(iter_count=100)

# Stop recording
solver.journal.stop()
print("Journal saved to setup_commands.jou")

# Later: Execute recorded journal on new session
new_solver = pyfluent.launch_fluent(
    mode="solver",
    journal_file_names="setup_commands.jou"
)

# Or execute journal in running session
solver.tui.file.read_journal("setup_commands.jou")
```

## Advanced Configuration and Utilities

### Search API for Finding Settings

Search through Fluent object hierarchy to find settings, commands, and parameters.

```python
from ansys.fluent.core import search
import ansys.fluent.core as pyfluent

# Search for settings related to boundary conditions
results = search("boundary condition")
print("Boundary condition related objects:")
for result in results[:5]:
    print(f"  {result}")

# Search for turbulence models
turbulence_results = search("turbulence model")
print("\nTurbulence model objects:")
for result in turbulence_results[:5]:
    print(f"  {result}")

# Search in specific session context
solver = pyfluent.launch_fluent(mode="solver")
inlet_results = search("inlet", session=solver)
print("\nInlet related objects:")
for result in inlet_results[:10]:
    print(f"  {result}")
```

### Module Configuration Options

Configure PyFluent global settings for launch behavior and performance tuning.

```python
import ansys.fluent.core as pyfluent

# Configure Fluent version
pyfluent.config.fluent_release_version = "25.1"

# Set launch timeout
pyfluent.config.launch_fluent_timeout = 120  # seconds

# Enable container launch by default
pyfluent.config.launch_fluent_container = True

# Configure container mount paths
pyfluent.config.container_mount_source = "/home/user/fluent_data"
pyfluent.config.container_mount_target = "/fluent_data"

# Enable watchdog for cleanup
pyfluent.config.start_watchdog = True

# Configure data model caching
pyfluent.config.datamodel_use_state_cache = True
pyfluent.config.datamodel_use_attr_cache = True

# Launch with configured settings
solver = pyfluent.launch_fluent(mode="solver", processor_count=2)
print(f"Launched Fluent {solver.get_fluent_version()}")
```

## Summary

PyFluent serves as a comprehensive Python interface for Ansys Fluent, enabling automation of complex CFD workflows from geometry import through mesh generation to solution and post-processing. The library supports multiple session types including full solver sessions with equation solving capabilities, meshing sessions with automated workflow support, and lightweight file sessions for data extraction without launching Fluent. Key use cases include running parametric design studies with parallel execution across multiple Fluent instances, extracting field data for custom visualization and analysis in Python scientific computing environments, and integrating CFD simulations into larger multiphysics or optimization workflows.

The API provides three primary interaction paradigms: the Settings API for object-oriented access to solver and mesh configurations, the TUI interface for executing traditional Fluent text commands, and the Workflow API for automating meshing operations. Field data extraction capabilities support various request types including scalar fields (pressure, temperature, density), vector fields (velocity, momentum), surface mesh topology with connectivity information, and particle pathlines for flow visualization. The library handles deployment complexity through support for local standalone execution, Docker containerization with volume mounting, and HPC cluster integration via job schedulers like Slurm, making it suitable for both interactive development and production automation scenarios.