Material properties and custom failure criterion#

This example shows how to access constant material properties and how to implement a custom failure criterion. The failure criterion is computed for all layers and integration points. Finally, the elemental maximum is computed and shown.

Note: Only constant material properties are currently supported.


Import dependencies

import ansys.dpf.core as dpf
import numpy as np

from ansys.dpf.composites.composite_model import CompositeModel
from ansys.dpf.composites.constants import Sym3x3TensorComponent
from ansys.dpf.composites.example_helper import get_continuous_fiber_example_files
from ansys.dpf.composites.layup_info.material_properties import MaterialProperty
from ansys.dpf.composites.select_indices import get_selected_indices
from ansys.dpf.composites.server_helpers import connect_to_or_start_server

Start a server and get the examples files. This will copy the example files into the current working directory.

server = connect_to_or_start_server()
composite_files_on_server = get_continuous_fiber_example_files(server, "shell")

Set up the composite model

composite_model = CompositeModel(composite_files_on_server, server)

Get dictionary that maps dpf_material_id to properties The creation of the dictionary is currently quite slow and should be done before using the properties in a loop. Currently only constant properties are supported. For variable material properties, the default value is returned.

material_property = MaterialProperty.Strain_Limits_eXt
property_dict = composite_model.get_constant_property_dict([material_property])

Get strain field

strain_operator = composite_model.core_model.results.elastic_strain()
strain_field = strain_operator.get_output(pin=0, output_type=dpf.types.fields_container)[0]

Implement a custom failure criterion: basic max strain

result_field = dpf.field.Field(location=dpf.locations.elemental, nature=dpf.natures.scalar)

with result_field.as_local_field() as local_result_field:
    component = Sym3x3TensorComponent.TENSOR11

    for element_id in strain_field.scoping.ids:
        strain_data = strain_field.get_entity_data_by_id(element_id)
        element_info = composite_model.get_element_info(element_id)
        element_max = 0
        for layer_index, dpf_material_id in enumerate(element_info.dpf_material_ids):
            tensile_strain_limit_1 = property_dict[dpf_material_id][material_property]
            selected_indices = get_selected_indices(element_info, layers=[layer_index])
            # Tensile max strain criteria in 1 direction
            layer_strain_values = strain_data[selected_indices][:, component]
            if tensile_strain_limit_1 > 0:
                layer_max = np.max(layer_strain_values)
                element_max = max(element_max, layer_max / tensile_strain_limit_1)

        # add to output field
        local_result_field.append([element_max], element_id)

004 get material properties example

Total running time of the script: ( 0 minutes 8.675 seconds)

Gallery generated by Sphinx-Gallery