Failure analysis of an MAPDL (RST) model

This example shows the postprocessing of an MAPDL (RST) model with layered elements that was not preprocessed by ACP. The difference between the RST-only and ACP-based workflow is that the section data are loaded from the RST file instead of the ACP layup file. This happens automatically if the parameter composite of the ContinuousFiberCompositesFiles class is not set.

The engineering data file (XML or ENGD) with the material properties is needed anyway. Otherwise, the material properties cannot be mapped. At the end of this example, two workflows are shown on how to create the engineering data file based on a MAPDL model and how to set the material UUIDs in MAPDL.

Important

The material UUIDs in the engineering data file must be identical to the UUIDs in Mechanical APDL (RST file).

The postprocessing of MAPDL models is supported in 2024 R2 (DPF Server version 8.0) and later. A few advanced features are not supported with the RST only workflow. For more information, see Limitations.

Set up analysis

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

Load Ansys libraries.

from ansys.dpf.composites.composite_model import CompositeModel
from ansys.dpf.composites.constants import FailureOutput
from ansys.dpf.composites.example_helper import get_continuous_fiber_example_files
from ansys.dpf.composites.failure_criteria import (
    CombinedFailureCriterion,
    CoreFailureCriterion,
    FaceSheetWrinklingCriterion,
    MaxStrainCriterion,
    MaxStressCriterion,
    VonMisesCriterion,
)
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()

Get input files (RST and material.engd but skip the ACP layup file).

composite_files_on_server = get_continuous_fiber_example_files(server, "shell", True)
print(composite_files_on_server)

ContinuousFiberCompositesFiles(rst=['/tmp/dataProcessingTemp139962901063424/5eada5af-edb2-46f0-8aed-a1deba5fb65f/shell.rst'], composite={}, engineering_data='/tmp/dataProcessingTemp139962901063424/b8969876-69f2-4caa-aefe-490c3c4dbd47/material.engd', files_are_local=False)

Configure combined failure criterion

Configure the combined failure criterion.

combined_fc = CombinedFailureCriterion(
    name="failure of all materials",
    failure_criteria=[
        MaxStrainCriterion(),
        MaxStressCriterion(),
        CoreFailureCriterion(),
        VonMisesCriterion(vme=True, vms=False),
        FaceSheetWrinklingCriterion(),
    ],
)

Set up model and evaluate failures

Set up the composite model.

composite_model = CompositeModel(composite_files_on_server, server)

Evaluate failures for the entire model

output_all_elements = composite_model.evaluate_failure_criteria(
    combined_criterion=combined_fc,
)
irf_field = output_all_elements.get_field({"failure_label": FailureOutput.FAILURE_VALUE})
irf_field.plot()

Static Scene

Interactive Scene

Create and plot a sampling point

sampling_point = composite_model.get_sampling_point(combined_criterion=combined_fc, element_id=2)
sampling_plot = sampling_point.get_result_plots(core_scale_factor=0.1)
sampling_plot.figure.show()

Create Engineering Data file and set material UUIDs in MAPDL

Here are two workflows for setting up the engineering data file and the material UUIDs in MAPDL. The material UUIDs must be set in MAPDL before the model is solved.

With WB and Engineering Data:

• Create an External Model system in WB and load the solver input file

• Link the External Model with an Engineering Data system and update it

• Save the project and copy the generated engineering data file (EngineeringData.xml)

• For each material, look for the DataTransferID, go to MAPDL and set the material UUIDs with the MP,UVID,<material index>,<value> command

With ACP Standalone (for constant material properties only):

• Start ACP, go to File - Import Model and load the solver input file (CDB)

• Go to the Materials folder and export the engineering data file (Ansys Workbench XML)

• For each material, look for the DataTransferID, go to MAPDL and set the material UUID with the MP,UVID,<material index>,<value> command.