PyMechanical shell workflow#

This example shows how to set up a simple shell model with PyACP and PyMechanical:

The geometry is imported into Mechanical and meshed.
The mesh is exported to ACP.
A simple lay-up is defined in ACP.
Plies and materials are exported from ACP, and imported into Mechanical.
Boundary conditions are set in Mechanical.
The model is solved.
The results are post-processed in PyDPF - Composites.

Warning

The PyACP / PyMechanical integration is still experimental. Refer to the limitations section for more information.

Note

Outputs and plots for this example are not shown in the rendered online documentation. To see the outputs and plots, run the example script or Jupyter notebook locally.

Import modules and start the Ansys products#

Import the standard library and third-party dependencies.

from concurrent.futures import ThreadPoolExecutor
import pathlib
import tempfile
import textwrap

Import PyACP, PyMechanical, and PyDPF - Composites.

# isort: off
import ansys.acp.core as pyacp
from ansys.acp.core.extras import set_plot_theme
import ansys.dpf.composites as pydpf_composites
import ansys.mechanical.core as pymechanical

Set the plot theme for the example. This is optional, and ensures that you get the same plot style (theme, color map, etc.) as in the online documentation.

set_plot_theme()

Start the ACP, Mechanical, and DPF servers. We use a ThreadPoolExecutor to start them in parallel.

with ThreadPoolExecutor() as executor:
    futures = [
        executor.submit(pymechanical.launch_mechanical, batch=True),
        executor.submit(pyacp.launch_acp),
        executor.submit(pydpf_composites.server_helpers.connect_to_or_start_server),
    ]
    mechanical, acp, dpf = (fut.result() for fut in futures)

Get example input files#

Create a temporary working directory, and download the example input files to this directory.

working_dir = tempfile.TemporaryDirectory()
working_dir_path = pathlib.Path(working_dir.name)
input_geometry = pyacp.extras.example_helpers.get_example_file(
    pyacp.extras.example_helpers.ExampleKeys.CLASS40_AGDB, working_dir_path
)

Generate the mesh in PyMechanical#

Load the geometry into Mechanical, generate the mesh, and export it to the appropriate transfer format for ACP.

mesh_path = working_dir_path / "mesh.h5"
mechanical.run_python_script(
    # This script runs in the Mechanical Python environment, which uses IronPython 2.7.
    textwrap.dedent(
        f"""\
        # Import the geometry
        geometry_import = Model.GeometryImportGroup.AddGeometryImport()

        import_format = Ansys.Mechanical.DataModel.Enums.GeometryImportPreference.Format.Automatic
        import_preferences = Ansys.ACT.Mechanical.Utilities.GeometryImportPreferences()
        import_preferences.ProcessNamedSelections = True
        import_preferences.ProcessCoordinateSystems = True

        geometry_file = {str(input_geometry)!r}
        geometry_import.Import(
            geometry_file,
            import_format,
            import_preferences
        )

        # The thickness will be overridden by the ACP model, but is required
        # for the model to be valid.
        for body in Model.Geometry.GetChildren(
            Ansys.Mechanical.DataModel.Enums.DataModelObjectCategory.Body, True
        ):
            body.Thickness = Quantity(1e-6, "m")

        Model.Mesh.GenerateMesh()
        """
    )
)
pyacp.mechanical_integration_helpers.export_mesh_for_acp(mechanical=mechanical, path=mesh_path)

Set up the ACP model#

Setup basic ACP lay-up based on the mesh in mesh_path, and export material and composite definition file to output_path.

composite_definitions_h5 = "ACPCompositeDefinitions.h5"
matml_file = "materials.xml"


model = acp.import_model(mesh_path, format="ansys:h5")

mat = model.create_material(name="mat")

mat.ply_type = "regular"
mat.engineering_constants.E1 = 1e12
mat.engineering_constants.E2 = 1e11
mat.engineering_constants.E3 = 1e11
mat.engineering_constants.G12 = 1e10
mat.engineering_constants.G23 = 1e10
mat.engineering_constants.G31 = 1e10
mat.engineering_constants.nu12 = 0.3
mat.engineering_constants.nu13 = 0.3
mat.engineering_constants.nu23 = 0.3

mat.strain_limits = pyacp.material_property_sets.ConstantStrainLimits.from_orthotropic_constants(
    eXc=-0.01,
    eYc=-0.01,
    eZc=-0.01,
    eXt=0.01,
    eYt=0.01,
    eZt=0.01,
    eSxy=0.01,
    eSyz=0.01,
    eSxz=0.01,
)

corecell_81kg_5mm = model.create_fabric(name="Corecell 81kg", thickness=0.005, material=mat)

ros = model.create_rosette(name="ros", origin=(0, 0, 0))

oss = model.create_oriented_selection_set(
    name="oss",
    orientation_point=(-0, 0, 0),
    orientation_direction=(0.0, 1, 0.0),
    element_sets=[model.element_sets["All_Elements"]],
    rosettes=[ros],
)

mg = model.create_modeling_group(name="group")
mg.create_modeling_ply(
    name="ply",
    ply_material=corecell_81kg_5mm,
    oriented_selection_sets=[oss],
    ply_angle=45,
    number_of_layers=1,
    global_ply_nr=0,  # add at the end
)
mg.create_modeling_ply(
    name="ply2",
    ply_material=corecell_81kg_5mm,
    oriented_selection_sets=[oss],
    ply_angle=0,
    number_of_layers=2,
    global_ply_nr=0,  # add at the end
)

Update and Save the ACP model#

model.update()

model.export_shell_composite_definitions(working_dir_path / composite_definitions_h5)
model.export_materials(working_dir_path / matml_file)

Import materials and plies into Mechanical#

Import materials into Mechanical

mechanical.run_python_script(f"Model.Materials.Import({str(working_dir_path / matml_file)!r})")

Import plies into Mechanical

pyacp.mechanical_integration_helpers.import_acp_composite_definitions(
    mechanical=mechanical,
    path=working_dir_path / composite_definitions_h5,
)

Set boundary condition and solve#

mechanical.run_python_script(
    textwrap.dedent(
        """\
        front_edge = Model.AddNamedSelection()
        front_edge.Name = "Front Edge"
        front_edge.ScopingMethod = GeometryDefineByType.Worksheet

        front_edge.GenerationCriteria.Add(None)
        front_edge.GenerationCriteria[0].EntityType = SelectionType.GeoEdge
        front_edge.GenerationCriteria[0].Criterion = SelectionCriterionType.LocationX
        front_edge.GenerationCriteria[0].Operator = SelectionOperatorType.GreaterThan
        front_edge.GenerationCriteria[0].Value = Quantity('-4.6 [m]')
        front_edge.Generate()

        back_edge = Model.AddNamedSelection()
        back_edge.Name = "Back Edge"
        back_edge.ScopingMethod = GeometryDefineByType.Worksheet

        back_edge.GenerationCriteria.Add(None)
        back_edge.GenerationCriteria[0].EntityType = SelectionType.GeoEdge
        back_edge.GenerationCriteria[0].Criterion = SelectionCriterionType.LocationX
        back_edge.GenerationCriteria[0].Operator = SelectionOperatorType.LessThan
        back_edge.GenerationCriteria[0].Value = Quantity('-7.8 [m]')
        back_edge.Generate()

        analysis = Model.AddStaticStructuralAnalysis()

        fixed_support = analysis.AddFixedSupport()
        fixed_support.Location = back_edge

        force = analysis.AddForce()
        force.DefineBy = LoadDefineBy.Components
        force.XComponent.Output.SetDiscreteValue(0, Quantity(1e6, "N"))
        force.Location = front_edge

        analysis.Solution.Solve(True)
        """
    )
)

rst_file = [filename for filename in mechanical.list_files() if filename.endswith(".rst")][0]
matml_out = [filename for filename in mechanical.list_files() if filename.endswith("MatML.xml")][0]

Postprocess results#

Evaluate the failure criteria using the PyDPF - Composites.

max_strain = pydpf_composites.failure_criteria.MaxStrainCriterion()
cfc = pydpf_composites.failure_criteria.CombinedFailureCriterion(
    name="Combined Failure Criterion",
    failure_criteria=[max_strain],
)

composite_model = pydpf_composites.composite_model.CompositeModel(
    composite_files=pydpf_composites.data_sources.ContinuousFiberCompositesFiles(
        rst=rst_file,
        composite={
            "shell": pydpf_composites.data_sources.CompositeDefinitionFiles(
                definition=working_dir_path / composite_definitions_h5
            ),
        },
        engineering_data=working_dir_path / matml_out,
    ),
    server=dpf,
)

# Evaluate the failure criteria
output_all_elements = composite_model.evaluate_failure_criteria(cfc)

# Query and plot the results
irf_field = output_all_elements.get_field(
    {"failure_label": pydpf_composites.constants.FailureOutput.FAILURE_VALUE}
)

irf_field.plot()

Gallery generated by Sphinx-Gallery