.. DO NOT EDIT.
.. THIS FILE WAS AUTOMATICALLY GENERATED BY SPHINX-GALLERY.
.. TO MAKE CHANGES, EDIT THE SOURCE PYTHON FILE:
.. "examples/workflows/06-cdb-to-pymechanical-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_06-cdb-to-pymechanical-workflow.py>`
to download the full example code.
.. rst-class:: sphx-glr-example-title
.. _sphx_glr_examples_workflows_06-cdb-to-pymechanical-workflow.py:
.. _cdb_to_pymechanical_example:
CDB to PyMechanical shell workflow
==================================
This example shows how to define a composite lay-up in PyACP based on a mesh
from a CDB file, import the model into PyMechanical for defining the load and
boundary conditions, and run a failure analysis with 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 44-46
Import modules and start the Ansys products
-------------------------------------------
.. GENERATED FROM PYTHON SOURCE LINES 49-50
Import the standard library and third-party dependencies.
.. GENERATED FROM PYTHON SOURCE LINES 50-56
.. code-block:: Python
from concurrent.futures import ThreadPoolExecutor
import pathlib
import tempfile
import textwrap
.. GENERATED FROM PYTHON SOURCE LINES 57-58
Import PyACP, PyMechanical, and PyDPF - Composites.
.. GENERATED FROM PYTHON SOURCE LINES 58-66
.. code-block:: Python
# isort: off
import ansys.acp.core as pyacp
from ansys.acp.core.extras import example_helpers
import ansys.dpf.composites as pydpf_composites
import ansys.mechanical.core as pymechanical
.. GENERATED FROM PYTHON SOURCE LINES 68-70
Start the ACP, Mechanical, and DPF servers. We use a ``ThreadPoolExecutor``
to start them in parallel.
.. GENERATED FROM PYTHON SOURCE LINES 70-78
.. code-block:: Python
with ThreadPoolExecutor() as executor:
futures = [
executor.submit(pyacp.launch_acp),
executor.submit(pymechanical.launch_mechanical, batch=True),
executor.submit(pydpf_composites.server_helpers.connect_to_or_start_server),
]
acp, mechanical, dpf = (fut.result() for fut in futures)
.. GENERATED FROM PYTHON SOURCE LINES 79-84
Get example input files
-----------------------
Create a temporary working directory, and download the example input files
to this directory.
.. GENERATED FROM PYTHON SOURCE LINES 84-91
.. code-block:: Python
working_dir = tempfile.TemporaryDirectory()
working_dir_path = pathlib.Path(working_dir.name)
input_file = example_helpers.get_example_file(
example_helpers.ExampleKeys.BASIC_FLAT_PLATE_DAT, working_dir_path
)
.. GENERATED FROM PYTHON SOURCE LINES 92-96
Set up the ACP model
--------------------
Setup basic ACP lay-up based on the CDB file.
.. GENERATED FROM PYTHON SOURCE LINES 96-101
.. code-block:: Python
model = acp.import_model(path=input_file, format="ansys:cdb")
model.unit_system
.. GENERATED FROM PYTHON SOURCE LINES 102-103
Visualize the loaded mesh.
.. GENERATED FROM PYTHON SOURCE LINES 103-107
.. code-block:: Python
mesh = model.mesh.to_pyvista()
mesh.plot(show_edges=True)
.. GENERATED FROM PYTHON SOURCE LINES 108-113
Define the composite lay-up
---------------------------
Create an orthotropic material and fabric including strain limits, which are later
used to postprocess the simulation.
.. GENERATED FROM PYTHON SOURCE LINES 113-142
.. code-block:: Python
engineering_constants = (
pyacp.material_property_sets.ConstantEngineeringConstants.from_orthotropic_constants(
E1=5e10, E2=1e10, E3=1e10, nu12=0.28, nu13=0.28, nu23=0.3, G12=5e9, G23=4e9, G31=4e9
)
)
strain_limit = 0.01
strain_limits = pyacp.material_property_sets.ConstantStrainLimits.from_orthotropic_constants(
eXc=-strain_limit,
eYc=-strain_limit,
eZc=-strain_limit,
eXt=strain_limit,
eYt=strain_limit,
eZt=strain_limit,
eSxy=strain_limit,
eSyz=strain_limit,
eSxz=strain_limit,
)
ud_material = model.create_material(
name="UD",
ply_type=pyacp.PlyType.REGULAR,
engineering_constants=engineering_constants,
strain_limits=strain_limits,
)
fabric = model.create_fabric(name="UD", material=ud_material, thickness=1e-4)
.. GENERATED FROM PYTHON SOURCE LINES 143-144
Define a rosette and oriented selection set. Plot the orientation.
.. GENERATED FROM PYTHON SOURCE LINES 144-160
.. code-block:: Python
rosette = model.create_rosette(origin=(0.0, 0.0, 0.0), dir1=(1.0, 0.0, 0.0), dir2=(0.0, 0.0, 1.0))
oss = model.create_oriented_selection_set(
name="oss",
orientation_point=(0.0, 0.0, 0.0),
orientation_direction=(0.0, 1.0, 0),
element_sets=[model.element_sets["All_Elements"]],
rosettes=[rosette],
)
model.update()
plotter = pyacp.get_directions_plotter(model=model, components=[oss.elemental_data.orientation])
plotter.show()
.. GENERATED FROM PYTHON SOURCE LINES 161-162
Create various plies with different angles and add them to a modeling group.
.. GENERATED FROM PYTHON SOURCE LINES 162-175
.. code-block:: Python
modeling_group = model.create_modeling_group(name="modeling_group")
angles = [0, 45, -45, 45, -45, 0]
for idx, angle in enumerate(angles):
modeling_group.create_modeling_ply(
name=f"ply_{idx}_{angle}_{fabric.name}",
ply_angle=angle,
ply_material=fabric,
oriented_selection_sets=[oss],
)
model.update()
.. GENERATED FROM PYTHON SOURCE LINES 176-177
Show the fiber directions of a specific ply.
.. GENERATED FROM PYTHON SOURCE LINES 177-190
.. code-block:: Python
modeling_ply = model.modeling_groups["modeling_group"].modeling_plies["ply_4_-45_UD"]
fiber_direction = modeling_ply.elemental_data.fiber_direction
assert fiber_direction is not None
plotter = pyacp.get_directions_plotter(
model=model,
components=[fiber_direction],
)
plotter.show()
.. GENERATED FROM PYTHON SOURCE LINES 191-194
For a quick overview, print the model tree. Note that
the model can also be opened in the ACP GUI. For more
information, see :ref:`view_the_model_in_the_acp_gui`.
.. GENERATED FROM PYTHON SOURCE LINES 194-196
.. code-block:: Python
pyacp.print_model(model)
.. GENERATED FROM PYTHON SOURCE LINES 197-199
Save the ACP model
------------------
.. GENERATED FROM PYTHON SOURCE LINES 199-209
.. code-block:: Python
cdb_filename = "model.cdb"
composite_definitions_h5_filename = "ACPCompositeDefinitions.h5"
matml_filename = "materials.xml"
model.export_analysis_model(working_dir_path / cdb_filename)
model.export_shell_composite_definitions(working_dir_path / composite_definitions_h5_filename)
model.export_materials(working_dir_path / matml_filename)
.. GENERATED FROM PYTHON SOURCE LINES 210-214
Import mesh, materials and plies into Mechanical
------------------------------------------------
Import geometry, mesh, and named selections into Mechanical
.. GENERATED FROM PYTHON SOURCE LINES 214-221
.. code-block:: Python
pyacp.mechanical_integration_helpers.import_acp_mesh_from_cdb(
mechanical=mechanical, cdb_path=working_dir_path / cdb_filename
)
.. GENERATED FROM PYTHON SOURCE LINES 222-223
Import materials into Mechanical
.. GENERATED FROM PYTHON SOURCE LINES 223-226
.. code-block:: Python
mechanical.run_python_script(f"Model.Materials.Import({str(working_dir_path / matml_filename)!r})")
.. GENERATED FROM PYTHON SOURCE LINES 227-228
Import plies into Mechanical
.. GENERATED FROM PYTHON SOURCE LINES 228-233
.. code-block:: Python
pyacp.mechanical_integration_helpers.import_acp_composite_definitions(
mechanical=mechanical, path=working_dir_path / composite_definitions_h5_filename
)
.. GENERATED FROM PYTHON SOURCE LINES 234-237
Set boundary condition and solve
---------------------------------
.. GENERATED FROM PYTHON SOURCE LINES 237-280
.. code-block:: Python
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.Largest
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.Smallest
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(100, "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]
.. GENERATED FROM PYTHON SOURCE LINES 281-285
Postprocess results
-------------------
Evaluate the failure criteria using the PyDPF - Composites.
.. GENERATED FROM PYTHON SOURCE LINES 285-315
.. 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={
"shell": pydpf_composites.data_sources.CompositeDefinitionFiles(
definition=working_dir_path / composite_definitions_h5_filename
),
},
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_06-cdb-to-pymechanical-workflow.py:
.. only:: html
.. container:: sphx-glr-footer sphx-glr-footer-example
.. container:: sphx-glr-download sphx-glr-download-jupyter
:download:`Download Jupyter notebook: 06-cdb-to-pymechanical-workflow.ipynb <06-cdb-to-pymechanical-workflow.ipynb>`
.. container:: sphx-glr-download sphx-glr-download-python
:download:`Download Python source code: 06-cdb-to-pymechanical-workflow.py <06-cdb-to-pymechanical-workflow.py>`
.. container:: sphx-glr-download sphx-glr-download-zip
:download:`Download zipped: 06-cdb-to-pymechanical-workflow.zip <06-cdb-to-pymechanical-workflow.zip>`
.. only:: html
.. rst-class:: sphx-glr-signature
`Gallery generated by Sphinx-Gallery <https://sphinx-gallery.github.io>`_