import flow360 as fl
from flow360 import u
from flow360.examples import TutorialCHTSolver

TutorialCHTSolver.get_files()

project = fl.Project.from_volume_mesh(
    TutorialCHTSolver.mesh_filename, name="Conjugate Heat Transfer"
)

volume_mesh = project.volume_mesh

with fl.SI_unit_system:
    params = fl.SimulationParams(
        reference_geometry=fl.ReferenceGeometry(
            moment_center=[0, 0, 0] * fl.u.m,
            moment_length=[1, 1, 1] * fl.u.m,
            area=1 * fl.u.m**2,
        ),
        operating_condition=fl.AerospaceCondition.from_mach(mach=0.1),
        time_stepping=fl.Steady(
            max_steps=10000, CFL=fl.RampCFL(initial=1, final=100, ramp_steps=1000)
        ),
        models=[
            fl.Fluid(
                navier_stokes_solver=fl.NavierStokesSolver(
                    absolute_tolerance=1e-9,
                    linear_solver=fl.LinearSolver(max_iterations=35),
                    order_of_accuracy=2,
                    kappa_MUSCL=-1,
                ),
                turbulence_model_solver=fl.SpalartAllmaras(
                    absolute_tolerance=1e-8,
                    linear_solver=fl.LinearSolver(max_iterations=25),
                    equation_evaluation_frequency=4,
                    order_of_accuracy=2,
                ),
            ),
            fl.Wall(
                surfaces=volume_mesh["fluid/centerbody"],
            ),
            fl.Freestream(
                surfaces=volume_mesh["fluid/farfield"],
            ),
        ],
        outputs=[
            fl.VolumeOutput(
                output_format=["paraview", "tecplot"],
                output_fields=[
                    "primitiveVars",
                    "T",
                    "Cp",
                    "Mach",
                ],
            ),
            fl.SurfaceOutput(
                surfaces=volume_mesh["*"],
                output_format=["paraview", "tecplot"],
                output_fields=["primitiveVars", "T", "Cp", "Cf", "CfVec"],
            ),
            fl.SliceOutput(
                entities=[
                    fl.Slice(
                        name="slice_x",
                        normal=(1, 0, 0),
                        origin=(0.35, 0, 0),
                    ),
                    fl.Slice(
                        name="slice_y",
                        normal=(0, 1, 0),
                        origin=(0, 0, 0),
                    ),
                ],
                output_fields=["T", "Mach"],
            ),
        ],
    )

with fl.SI_unit_system:
    models = [
        fl.Solid(
            entities=volume_mesh["solid"],
            heat_equation_solver=fl.HeatEquationSolver(
                absolute_tolerance=1e-11,
                linear_solver=fl.LinearSolver(
                    max_iterations=25,
                    absolute_tolerance=1e-12,
                ),
                equation_evaluation_frequency=10,
            ),
            material=fl.SolidMaterial(
                name="copper",
                thermal_conductivity=398 * fl.u.W / (fl.u.m * fl.u.K),
            ),
            volumetric_heat_source=5e3 * fl.u.W / (0.01257 * fl.u.m**3),
        ),
        fl.Wall(
            surfaces=volume_mesh["solid/adiabatic"],
            heat_spec=fl.HeatFlux(0 * fl.u.W / fl.u.m**2),
        ),
    ]

params.models.extend(models)

case = project.run_case(params=params, name="Steady CHT")

case.wait()

results = case.results

surface_heat_transfer = results.surface_heat_transfer.as_dataframe()
print(surface_heat_transfer)