Cyclic symmetry

This example shows how to postprocess a cyclic symmetry analysis. The initial (original) sector can be postprocessed with the same tools as a standard analysis. The postprocessing workflow is demonstrated by running a failure analysis, extracting ply-wise stresses, and implementing a custom failure criterion.

The postprocessing of expanded sectors is not yet supported.

Note

When using a Workbench project, use the composite_files_from_workbench_harmonic_analysis() method to obtain the input files.

Set up analysis

Setting up the analysis consists of loading the required modules, connecting to the DPF server, and retrieving the example files.

Load Ansys libraries and helper functions.

import ansys.dpf.core as dpf

from ansys.dpf.composites.composite_model import CompositeModel
from ansys.dpf.composites.constants import FailureOutput, Sym3x3TensorComponent
from ansys.dpf.composites.example_helper import get_continuous_fiber_example_files
from ansys.dpf.composites.failure_criteria import CombinedFailureCriterion, MaxStressCriterion
from ansys.dpf.composites.layup_info import get_all_analysis_ply_names
from ansys.dpf.composites.layup_info.material_properties import MaterialProperty
from ansys.dpf.composites.ply_wise_data import SpotReductionStrategy, get_ply_wise_data
from ansys.dpf.composites.select_indices import get_selected_indices
from ansys.dpf.composites.server_helpers import connect_to_or_start_server

Start a DPF server and copy the example files into the current working directory.

server = connect_to_or_start_server()
composite_files = get_continuous_fiber_example_files(server, "cyclic_symmetry")

Create a composite model.

composite_model = CompositeModel(composite_files, server)

Evaluate a combined failure criterion.

combined_failure_criterion = CombinedFailureCriterion(failure_criteria=[MaxStressCriterion()])
failure_result = composite_model.evaluate_failure_criteria(combined_failure_criterion)

Plot the failure results.

irf_field = failure_result.get_field({"failure_label": FailureOutput.FAILURE_VALUE})
irf_field.plot()

Static Scene

Interactive Scene

Plot ply-wise stresses

All functions in PyDPF Composites can be used to postprocess the initial (original) sector.

rst_stream = composite_model.core_model.metadata.streams_provider
stress_operator = dpf.operators.result.stress()
stress_operator.inputs.streams_container.connect(rst_stream)
stress_operator.inputs.bool_rotate_to_global(False)
stress_container = stress_operator.outputs.fields_container()

all_ply_names = get_all_analysis_ply_names(composite_model.get_mesh())
all_ply_names

component_s11 = Sym3x3TensorComponent.TENSOR11
stress_field = stress_container[0]
elemental_values = get_ply_wise_data(
    field=stress_field,
    ply_name="P3L1__ModelingPly.1",
    mesh=composite_model.get_mesh(),
    component=component_s11,
    spot_reduction_strategy=SpotReductionStrategy.MAX,
    requested_location=dpf.locations.elemental,
)
composite_model.get_mesh().plot(elemental_values)

Static Scene

Interactive Scene

Custom failure criterion

The following code block shows how to implement a custom failure criterion. It computes the inverse reserve factor for each element with respect to fiber failure. The criterion distinguishes between tension and compression.

# Prepare dict with the material properties.
property_xt = MaterialProperty.Stress_Limits_Xt
property_xc = MaterialProperty.Stress_Limits_Xc
property_dict = composite_model.get_constant_property_dict([property_xt, property_xc])

result_field = dpf.field.Field(location=dpf.locations.elemental, nature=dpf.natures.scalar)
with result_field.as_local_field() as local_result_field:
    # Process only the layered elements
    for element_id in composite_model.get_all_layered_element_ids():
        element_info = composite_model.get_element_info(element_id)
        element_irf_max = 0.0
        stress_data = stress_field.get_entity_data_by_id(element_id)
        for layer_index, dpf_material_id in enumerate(element_info.dpf_material_ids):
            xt = property_dict[dpf_material_id][property_xt]
            xc = property_dict[dpf_material_id][property_xc]
            selected_indices = get_selected_indices(element_info, layers=[layer_index])
            # Maximum of fiber failure in tension and compression
            layer_stress_values = stress_data[selected_indices][:, component_s11]
            max_s11 = max(layer_stress_values)
            min_s11 = min(layer_stress_values)
            if xt > 0 and max_s11 > 0:
                element_irf_max = max(max_s11 / xt, element_irf_max)
            if xc < 0 and min_s11 < 0:
                element_irf_max = max(min_s11 / xc, element_irf_max)

        local_result_field.append([element_irf_max], element_id)

composite_model.get_mesh().plot(result_field)

Static Scene

Interactive Scene

Plot deformations on the expanded model

You can expand the deformations of the cyclic symmetry model as shown below. The same expansion is possible for strains and stresses. For more information, see Ansys DPF.

# Get the displacements and expand them
symmetry_option = 2  # fully expand the model
u_cyc = composite_model.core_model.results.displacement()
u_cyc.inputs.read_cyclic(symmetry_option)
# expand the displacements
deformations = u_cyc.outputs.fields_container()[0]

# Get and expand the mesh
mesh_provider = composite_model.core_model.metadata.mesh_provider
mesh_provider.inputs.read_cyclic(symmetry_option)
mesh = mesh_provider.outputs.mesh()
# Plot the expanded deformations
mesh.plot(deformations)

Static Scene

Interactive Scene