Note
Go to the end to download the full example code.
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 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(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)
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_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
)
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
matml_file = "materials.xml"
solid_model_cdb_file = "SolidModel.cdb"
solid_model_composite_definitions_h5 = "SolidModel.h5"
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"]],
)
Update and Save the ACP model#
model.update()
model.export_materials(working_dir_path / matml_file)
solid_model.export(working_dir_path / solid_model_cdb_file, format="ansys:cdb")
solid_model.export(working_dir_path / solid_model_composite_definitions_h5, format="ansys:h5")
Import mesh, materials and plies into Mechanical#
Import geometry, mesh, and named selections into Mechanical
pyacp.mechanical_integration_helpers.import_acp_mesh_from_cdb(
mechanical=mechanical_solid_model, cdb_path=working_dir_path / solid_model_cdb_file
)
Import materials into Mechanical
mechanical_solid_model.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_solid_model, path=working_dir_path / solid_model_composite_definitions_h5
)
Set boundary condition and solve#
Set boundary condition and solve
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]
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={
"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()