.. DO NOT EDIT.
.. THIS FILE WAS AUTOMATICALLY GENERATED BY SPHINX-GALLERY.
.. TO MAKE CHANGES, EDIT THE SOURCE PYTHON FILE:
.. "examples/workflows/05-pymechanical-to-cdb-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_05-pymechanical-to-cdb-workflow.py>`
to download the full example code.
.. rst-class:: sphx-glr-example-title
.. _sphx_glr_examples_workflows_05-pymechanical-to-cdb-workflow.py:
.. _pymechanical_to_cdb_example:
PyMechanical to CDB shell workflow
==================================
This example shows how to set up a workflow that uses PyMechanical to mesh the
geometry and define the load case, PyACP to define a layup, PyMAPDL to solve the
model, and PyDPF - Composites to post-process the results.
This workflow does *not* suffer from the limitations of the PyACP to
PyMechanical integration.
.. GENERATED FROM PYTHON SOURCE LINES 42-44
Import modules and start the Ansys products
-------------------------------------------
.. GENERATED FROM PYTHON SOURCE LINES 47-48
Import the standard library and third-party dependencies.
.. GENERATED FROM PYTHON SOURCE LINES 48-54
.. code-block:: Python
from concurrent.futures import ThreadPoolExecutor
import pathlib
import tempfile
import textwrap
.. GENERATED FROM PYTHON SOURCE LINES 55-56
Import PyACP, PyMechanical, and PyDPF - Composites.
.. GENERATED FROM PYTHON SOURCE LINES 56-65
.. code-block:: Python
# isort: off
import ansys.acp.core as pyacp
import ansys.dpf.core as pydpf_core
import ansys.dpf.composites as pydpf_composites
import ansys.mapdl.core as pymapdl
import ansys.mechanical.core as pymechanical
.. GENERATED FROM PYTHON SOURCE LINES 67-69
Start the ACP, Mechanical, and DPF servers. We use a ``ThreadPoolExecutor``
to start them in parallel.
.. GENERATED FROM PYTHON SOURCE LINES 69-79
.. code-block:: Python
with ThreadPoolExecutor() as executor:
futures = [
executor.submit(pymechanical.launch_mechanical, batch=True),
executor.submit(pyacp.launch_acp),
executor.submit(pymapdl.launch_mapdl),
executor.submit(pydpf_composites.server_helpers.connect_to_or_start_server),
]
mechanical, acp, mapdl, dpf = (fut.result() for fut in futures)
mapdl.clear()
.. GENERATED FROM PYTHON SOURCE LINES 80-85
Get example input files
-----------------------
Create a temporary working directory, and download the example input files
to this directory.
.. GENERATED FROM PYTHON SOURCE LINES 85-92
.. 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 93-98
Generate the mesh in PyMechanical
---------------------------------
Load the geometry into Mechanical, generate the mesh, and define the
load case.
.. GENERATED FROM PYTHON SOURCE LINES 98-169
.. code-block:: Python
cdb_path_initial = working_dir_path / "model_from_mechanical.cdb"
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()
# Define named selections at the front and back edges
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()
# Create a static structural analysis, and define the boundary
# conditions (fixed support at the back edge, force at the front edge).
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
# Export the model to a CDB file
analysis.WriteInputFile({str(cdb_path_initial)!r})
"""
)
)
.. GENERATED FROM PYTHON SOURCE LINES 170-174
Set up the ACP model
--------------------
Setup basic ACP lay-up based on the CDB file.
.. GENERATED FROM PYTHON SOURCE LINES 174-233
.. code-block:: Python
model = acp.import_model(path=cdb_path_initial, format="ansys:cdb")
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
)
.. GENERATED FROM PYTHON SOURCE LINES 234-236
Update and Save the ACP model
-----------------------------
.. GENERATED FROM PYTHON SOURCE LINES 236-247
.. code-block:: Python
model.update()
cdb_filename_out = "model_from_acp.cdb"
composite_definitions_h5_filename = "ACPCompositeDefinitions.h5"
matml_filename = "materials.xml"
model.export_analysis_model(working_dir_path / cdb_filename_out)
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 248-250
Solve with PyMAPDL
------------------
.. GENERATED FROM PYTHON SOURCE LINES 250-252
.. code-block:: Python
mapdl.clear()
.. GENERATED FROM PYTHON SOURCE LINES 253-254
Load the CDB file into PyMAPDL.
.. GENERATED FROM PYTHON SOURCE LINES 254-256
.. code-block:: Python
mapdl.input(str(working_dir_path / cdb_filename_out))
.. GENERATED FROM PYTHON SOURCE LINES 257-258
Solve the model.
.. GENERATED FROM PYTHON SOURCE LINES 258-262
.. code-block:: Python
mapdl.allsel()
mapdl.slashsolu()
mapdl.solve()
.. GENERATED FROM PYTHON SOURCE LINES 263-264
Show the displacements in postprocessing.
.. GENERATED FROM PYTHON SOURCE LINES 264-268
.. code-block:: Python
mapdl.post1()
mapdl.set("last")
mapdl.post_processing.plot_nodal_displacement(component="NORM")
.. GENERATED FROM PYTHON SOURCE LINES 269-270
Download the RST file for further postprocessing.
.. GENERATED FROM PYTHON SOURCE LINES 270-274
.. code-block:: Python
rstfile_name = f"{mapdl.jobname}.rst"
rst_file_local_path = working_dir_path / rstfile_name
mapdl.download(rstfile_name, working_dir_path)
.. GENERATED FROM PYTHON SOURCE LINES 275-279
Postprocessing with PyDPF - Composites
--------------------------------------
Specify the combined failure criterion.
.. GENERATED FROM PYTHON SOURCE LINES 279-286
.. code-block:: Python
max_strain = pydpf_composites.failure_criteria.MaxStrainCriterion()
cfc = pydpf_composites.failure_criteria.CombinedFailureCriterion(
name="Combined Failure Criterion",
failure_criteria=[max_strain],
)
.. GENERATED FROM PYTHON SOURCE LINES 287-288
Create the composite model and configure its input.
.. GENERATED FROM PYTHON SOURCE LINES 288-302
.. code-block:: Python
composite_model = pydpf_composites.composite_model.CompositeModel(
composite_files=pydpf_composites.data_sources.ContinuousFiberCompositesFiles(
rst=rst_file_local_path,
composite={
"shell": pydpf_composites.data_sources.CompositeDefinitionFiles(
definition=working_dir_path / composite_definitions_h5_filename
),
},
engineering_data=working_dir_path / matml_filename,
),
default_unit_system=pydpf_core.unit_system.unit_systems.solver_nmm,
server=dpf,
)
.. GENERATED FROM PYTHON SOURCE LINES 303-304
Evaluate the failure criteria.
.. GENERATED FROM PYTHON SOURCE LINES 304-306
.. code-block:: Python
output_all_elements = composite_model.evaluate_failure_criteria(cfc)
.. GENERATED FROM PYTHON SOURCE LINES 307-312
Query and plot the results.
Note that the maximum IRF is different when compared to :ref:`pymechanical_shell_example`
because ACP sets the ``ERESX,NO`` option in the CDB file. This option disables interpolation
of the results from the integration point to the nodes.
.. GENERATED FROM PYTHON SOURCE LINES 312-320
.. code-block:: Python
irf_field = output_all_elements.get_field(
{"failure_label": pydpf_composites.constants.FailureOutput.FAILURE_VALUE}
)
irf_field.plot()
# Close MAPDL instance
mapdl.exit()
.. _sphx_glr_download_examples_workflows_05-pymechanical-to-cdb-workflow.py:
.. only:: html
.. container:: sphx-glr-footer sphx-glr-footer-example
.. container:: sphx-glr-download sphx-glr-download-jupyter
:download:`Download Jupyter notebook: 05-pymechanical-to-cdb-workflow.ipynb <05-pymechanical-to-cdb-workflow.ipynb>`
.. container:: sphx-glr-download sphx-glr-download-python
:download:`Download Python source code: 05-pymechanical-to-cdb-workflow.py <05-pymechanical-to-cdb-workflow.py>`
.. container:: sphx-glr-download sphx-glr-download-zip
:download:`Download zipped: 05-pymechanical-to-cdb-workflow.zip <05-pymechanical-to-cdb-workflow.zip>`
.. only:: html
.. rst-class:: sphx-glr-signature
`Gallery generated by Sphinx-Gallery <https://sphinx-gallery.github.io>`_