.. DO NOT EDIT.
.. THIS FILE WAS AUTOMATICALLY GENERATED BY SPHINX-GALLERY.
.. TO MAKE CHANGES, EDIT THE SOURCE PYTHON FILE:
.. "examples/workflows/04-pymechanical-solid-workflow.py"
.. LINE NUMBERS ARE GIVEN BELOW.

.. only:: html

    .. note::
        :class: sphx-glr-download-link-note

        :ref:`Go to the end <sphx_glr_download_examples_workflows_04-pymechanical-solid-workflow.py>`
        to download the full example code.

.. rst-class:: sphx-glr-example-title

.. _sphx_glr_examples_workflows_04-pymechanical-solid-workflow.py:


.. _pymechanical_solid_example:

PyMechanical solid workflow
===========================

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

- The geometry is imported into Mechanical and meshed.
- The mesh is exported to ACP.
- A simple lay-up and solid model is defined in ACP.
- The solid model is exported, to a CDB file and a composite definition file.
- In a separate Mechanical instance, the solid model is imported.
- Materials and plies are imported.
- Boundary conditions are set.
- The model is solved.
- The results are post-processed in PyDPF Composites.

.. warning::

    The PyACP / PyMechanical integration is still experimental. Refer to the
    :ref:`limitations section <limitations>` for more information.

.. GENERATED FROM PYTHON SOURCE LINES 52-54

Import modules and start the Ansys products
-------------------------------------------

.. GENERATED FROM PYTHON SOURCE LINES 57-58

Import the standard library and third-party dependencies.

.. GENERATED FROM PYTHON SOURCE LINES 58-64

.. code-block:: Python


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


.. GENERATED FROM PYTHON SOURCE LINES 65-66

Import PyACP, PyMechanical, and PyDPF Composites.

.. GENERATED FROM PYTHON SOURCE LINES 66-74

.. code-block:: Python


    # isort: off

    import ansys.acp.core as pyacp
    import ansys.dpf.composites as pydpf_composites
    import ansys.mechanical.core as pymechanical



.. GENERATED FROM PYTHON SOURCE LINES 76-78

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

.. GENERATED FROM PYTHON SOURCE LINES 78-87

.. code-block:: Python

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


.. GENERATED FROM PYTHON SOURCE LINES 88-93

Get example input files
-----------------------

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

.. GENERATED FROM PYTHON SOURCE LINES 93-101

.. code-block:: Python


    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
    )



.. GENERATED FROM PYTHON SOURCE LINES 102-107

Generate the mesh in PyMechanical
---------------------------------

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

.. GENERATED FROM PYTHON SOURCE LINES 107-171

.. code-block:: Python


    mesh_path = working_dir_path / "mesh.h5"
    mechanical_shell_geometry.run_python_script(
        # This script runs in the Mechanical Python environment, which uses IronPython 2.7.
        textwrap.dedent(
            f"""\
            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
            )

            for body in Model.Geometry.GetChildren(
                Ansys.Mechanical.DataModel.Enums.DataModelObjectCategory.Body, True
            ):
                body.Thickness = Quantity(1e-6, "m")

            hull = Model.AddNamedSelection()
            hull.Name = "hull"
            hull.ScopingMethod = GeometryDefineByType.Worksheet
            # Add all faces with Z location < 0.9 m
            hull.GenerationCriteria.Add(None)
            hull.GenerationCriteria[0].EntityType = SelectionType.GeoFace
            hull.GenerationCriteria[0].Operator = SelectionOperatorType.LessThan
            hull.GenerationCriteria[0].Criterion = SelectionCriterionType.LocationZ
            hull.GenerationCriteria[0].Value = Quantity('0.9 [m]')
            # Remove keeltower
            hull.GenerationCriteria.Add(None)
            hull.GenerationCriteria[1].Action = SelectionActionType.Remove
            hull.GenerationCriteria[1].Criterion = SelectionCriterionType.LocationX
            hull.GenerationCriteria[1].Operator = SelectionOperatorType.RangeInclude
            hull.GenerationCriteria[1].LowerBound = Quantity('-6.7 [m]')
            hull.GenerationCriteria[1].UpperBound = Quantity('-5.9 [m]')
            # Add back keeltower bottom
            hull.GenerationCriteria.Add(None)
            hull.GenerationCriteria[2].Criterion = SelectionCriterionType.LocationZ
            hull.GenerationCriteria[2].Operator = SelectionOperatorType.LessThan
            hull.GenerationCriteria[2].Value = Quantity('-0.25 [m]')
            # Remove bulkhead
            hull.GenerationCriteria.Add(None)
            hull.GenerationCriteria[3].Action = SelectionActionType.Remove
            hull.GenerationCriteria[3].Criterion = SelectionCriterionType.LocationX
            hull.GenerationCriteria[3].Operator = SelectionOperatorType.RangeInclude
            hull.GenerationCriteria[3].LowerBound = Quantity('-5.7 [m]')
            hull.GenerationCriteria[3].UpperBound = Quantity('-5.6 [m]')
            hull.Generate()

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



.. GENERATED FROM PYTHON SOURCE LINES 172-182

Set up the ACP model
--------------------

Setup basic ACP lay-up based on the mesh in ``mesh_path``, and export the following
files to ``output_path``:

- Materials XML file
- Composite definitions HDF5 file
- Solid model composite definitions HDF5 file
- Solid model CDB file

.. GENERATED FROM PYTHON SOURCE LINES 182-251

.. code-block:: Python


    matml_file = "materials.xml"  # TODO: load an example materials XML file instead of defining the materials in ACP
    solid_model_cdb_file = "SolidModel.cdb"
    solid_model_composite_definitions_h5 = "SolidModel.h5"


    mesh_path = acp.upload_file(mesh_path)

    model = acp.import_model(path=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
    )

    solid_model = model.create_solid_model(
        element_sets=[model.element_sets["hull"]],
    )


.. GENERATED FROM PYTHON SOURCE LINES 252-254

Update and Save the ACP model
-----------------------------

.. GENERATED FROM PYTHON SOURCE LINES 254-275

.. code-block:: Python


    model.update()

    if acp.is_remote:
        export_path = pathlib.PurePosixPath(".")

    else:
        export_path = working_dir_path  # type: ignore

    model.export_materials(export_path / matml_file)
    solid_model.export(export_path / solid_model_cdb_file, format="ansys:cdb")
    solid_model.export(export_path / solid_model_composite_definitions_h5, format="ansys:h5")

    for filename in [
        matml_file,
        solid_model_cdb_file,
        solid_model_composite_definitions_h5,
    ]:
        acp.download_file(export_path / filename, working_dir_path / filename)



.. GENERATED FROM PYTHON SOURCE LINES 276-280

Import mesh, materials and plies into Mechanical
------------------------------------------------

Import geometry, mesh, and named selections into Mechanical

.. GENERATED FROM PYTHON SOURCE LINES 280-286

.. code-block:: Python


    pyacp.mechanical_integration_helpers.import_acp_solid_mesh(
        mechanical=mechanical_solid_model, cdb_path=working_dir_path / solid_model_cdb_file
    )



.. GENERATED FROM PYTHON SOURCE LINES 287-288

Import materials into Mechanical

.. GENERATED FROM PYTHON SOURCE LINES 288-293

.. code-block:: Python


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


.. GENERATED FROM PYTHON SOURCE LINES 294-295

Import plies into Mechanical

.. GENERATED FROM PYTHON SOURCE LINES 295-301

.. code-block:: Python


    pyacp.mechanical_integration_helpers.import_acp_composite_definitions(
        mechanical=mechanical_solid_model, path=working_dir_path / solid_model_composite_definitions_h5
    )



.. GENERATED FROM PYTHON SOURCE LINES 302-306

Set boundary condition and solve
---------------------------------

Set boundary condition and solve

.. GENERATED FROM PYTHON SOURCE LINES 306-350

.. code-block:: Python


    mechanical_solid_model.run_python_script(
        textwrap.dedent(
            """\
            analysis = Model.AddStaticStructuralAnalysis()

            front_face = Model.AddNamedSelection()
            front_face.Name = "front_face"
            front_face.ScopingMethod = GeometryDefineByType.Worksheet
            front_face.GenerationCriteria.Add(None)
            front_face.GenerationCriteria[0].EntityType = SelectionType.GeoFace
            front_face.GenerationCriteria[0].Criterion = SelectionCriterionType.LocationX
            front_face.GenerationCriteria[0].Operator = SelectionOperatorType.Largest
            front_face.Generate()

            back_face = Model.AddNamedSelection()
            back_face.Name = "back_face"
            back_face.ScopingMethod = GeometryDefineByType.Worksheet
            back_face.GenerationCriteria.Add(None)
            back_face.GenerationCriteria[0].EntityType = SelectionType.GeoFace
            back_face.GenerationCriteria[0].Criterion = SelectionCriterionType.LocationX
            back_face.GenerationCriteria[0].Operator = SelectionOperatorType.Smallest
            back_face.Generate()

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

            force = analysis.AddForce()
            force.DefineBy = LoadDefineBy.Components
            force.XComponent.Output.SetDiscreteValue(0, Quantity(1e5, "N"))
            force.Location = front_face

            analysis.Solve(True)
            """
        )
    )

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


.. GENERATED FROM PYTHON SOURCE LINES 351-355

Postprocess results
-------------------

Evaluate the failure criteria using the PyDPF Composites.

.. GENERATED FROM PYTHON SOURCE LINES 355-384

.. code-block:: Python


    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={
                "solid": pydpf_composites.data_sources.CompositeDefinitionFiles(
                    definition=working_dir_path / solid_model_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()


.. _sphx_glr_download_examples_workflows_04-pymechanical-solid-workflow.py:

.. only:: html

  .. container:: sphx-glr-footer sphx-glr-footer-example

    .. container:: sphx-glr-download sphx-glr-download-jupyter

      :download:`Download Jupyter notebook: 04-pymechanical-solid-workflow.ipynb <04-pymechanical-solid-workflow.ipynb>`

    .. container:: sphx-glr-download sphx-glr-download-python

      :download:`Download Python source code: 04-pymechanical-solid-workflow.py <04-pymechanical-solid-workflow.py>`

    .. container:: sphx-glr-download sphx-glr-download-zip

      :download:`Download zipped: 04-pymechanical-solid-workflow.zip <04-pymechanical-solid-workflow.zip>`


.. only:: html

 .. rst-class:: sphx-glr-signature

    `Gallery generated by Sphinx-Gallery <https://sphinx-gallery.github.io>`_