Note

Go to the end to download the full example code.

LS-Dyna Bird Strike#

This example shows how to set up the composite model for a LSDyna analysis, how to post-process it and how to filter the results. The simulation uses SPH (Smooth Particle Hydrodynamics) to mimic a bird strike on a leading edge of a composite wing.

Additional steps are required to process LS-Dyna results if compared with a Mechanical APDL analysis.

On the pre-processing side, these are:

  • The input file must be generated with WB LS Dyna

  • In WB Mechanical, enable the beta options and Output Integration Points Results for All ACP Plies or manually set MAXINT of the keyword DATABASE_EXTENT_BINARY to the maximum number of plies.

And these items must be considered on setting up the post-processing:

  • On initializing the composite model, these properties of ContinuousFiberCompositesFiles must be set: solver_type to LSDYNA and solver_input_file must point to the keyword file (for instance input.k).

  • The number of maximum integration points (MAXINT) has to be extracted from the keyword file. See composite::ls_dyna_keyword_parser operator.

  • The results (stress, strain, history variable etc.) must be pre-processed to support ply-wise filtering and to make them consistent with the layup model. See composite::ls_dyna_preparing_results operator.

Note:

  • Use the get_composite_files_from_workbench_result_folder() to get the composite files from a WB LS-Dyna result folder. Set solver_type to LSDYNA.

  • Only the first d3plot file must be passed to the composite model. The LSDyna reader will automatically pick up the other files.

Set up analysis#

Setup of the analysis and initialize the composite model.

import json

import ansys.dpf.core as dpf
from ansys.dpf.core import Operator, unit_systems

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.ply_wise_data import SpotReductionStrategy, get_ply_wise_data
from ansys.dpf.composites.server_helpers import connect_to_or_start_server

# sphinx_gallery_thumbnail_number = 4

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

composite_model = CompositeModel(
    composite_files=composite_files_on_server,
    server=server,
    default_unit_system=unit_systems.solver_nmm,
)

Get all the time ids to read all time steps and to select the correct results.

time_freq_support = composite_model.core_model.metadata.time_freq_support
time_ids = [v for v in time_freq_support.time_frequencies.scoping.ids]

Get displacements at the final time step

disp_result = composite_model.core_model.results.displacement()
displacement = disp_result.eval().get_field({"time": time_ids[-1]})

Read stresses in the material coordinate system

stress_operator = composite_model.core_model.results.stress()
stress_operator.inputs.bool_rotate_to_global(False)

Prepare data#

The LS Dyna results have to be pre-processed to support ply-wise filtering because the data must be consistent with the layup model. This pre-processing is based on the maximum integration points (MAXINT) from the DATABASE_EXTENT_BINARY keyword. This parameter can be extracted from the input file (input.k) with the help of the composite::ls_dyna_keyword_parser operator.

def prepare_lsdyna_results(
    my_results_container: dpf.fields_container.FieldsContainer,
) -> dpf.fields_container.FieldsContainer:
    keyword_parser = Operator("composite::ls_dyna_keyword_parser")
    keyword_parser.inputs.data_sources(composite_model.data_sources.solver_input_file)
    keyword_parser.inputs.keyword("DATABASE_EXTENT_BINARY")
    keyword_options_as_json = json.loads(keyword_parser.outputs.keyword_options.get_data())

    # remove unneeded integration points for each element
    strip_operator = Operator("composite::ls_dyna_preparing_results")
    strip_operator.inputs.maxint(int(keyword_options_as_json["maxint"]))
    strip_operator.inputs.fields_container(my_results_container)
    strip_operator.inputs.mesh(composite_model.get_mesh())
    stripped_results_container = strip_operator.outputs.fields_container.get_data()

    return stripped_results_container


stripped_stress_container = prepare_lsdyna_results(
    stress_operator.outputs.fields_container.get_data()
)

Filter data by analysis ply#

Print stresses of a few plies at the last time step. You can use get_all_analysis_ply_names to list all available plies. Note that one integration point per layer and element is available if MAXINT is equal or greater than the number of layers.

stripped_stress_field = stripped_stress_container.get_field({"time": time_ids[-1]})
camera = [
    (-1589.7832333411716, 1670.8197500164952, -328.2144469600579),
    (493.2896802711351, 0.2085447040423768, 763.1274012915459),
    (0.5149806660541146, 0.8152207788520537, 0.26497168776741287),
]

for ply_name in ["P1L1__ModelingPly.1", "P3L2__ModelingPly.1"]:
    print(f"Plotting s1 of ply {ply_name}")
    elemental_values = get_ply_wise_data(
        field=stripped_stress_field,
        ply_name=ply_name,
        mesh=composite_model.get_mesh(),
        component=Sym3x3TensorComponent.TENSOR11,
        spot_reduction_strategy=SpotReductionStrategy.MAX,
        requested_location=dpf.locations.elemental,
    )

    composite_model.get_mesh().plot(
        field_or_fields_container=elemental_values,
        deform_by=displacement,
        cpos=camera,
        zoom="tight",
    )
016 lsdyna bird strike
016 lsdyna bird strike
Plotting s1 of ply P1L1__ModelingPly.1
Plotting s1 of ply P3L2__ModelingPly.1

Plot history variables#

The same procedure can be applied to history variables. In this example, the 2nd history variable (compressive fiber mode) is plotted. 1 stands for elastic, 0 means failed.

hv_operator = dpf.Operator("lsdyna::d3plot::history_var")
hv_operator.inputs.data_sources(composite_model.data_sources.result_files)
hv_operator.inputs.time_scoping(time_ids)

stripped_hv_container = prepare_lsdyna_results(hv_operator.outputs.history_var.get_data())
stripped_hv_field = stripped_hv_container.get_field({"time": time_ids[-1], "ihv": 2})

for ply_name in ["P1L1__ModelingPly.1", "P3L2__ModelingPly.1"]:
    print(f"Plotting history variable 2 of ply {ply_name}")
    elemental_values = get_ply_wise_data(
        field=stripped_hv_field,
        ply_name=ply_name,
        mesh=composite_model.get_mesh(),
        component=0,
        spot_reduction_strategy=SpotReductionStrategy.MAX,
        requested_location=dpf.locations.elemental,
    )

    composite_model.get_mesh().plot(
        field_or_fields_container=elemental_values,
        deform_by=displacement,
        cpos=camera,
        zoom="tight",
    )
016 lsdyna bird strike
016 lsdyna bird strike
Plotting history variable 2 of ply P1L1__ModelingPly.1
Plotting history variable 2 of ply P3L2__ModelingPly.1

Total running time of the script: (0 minutes 11.712 seconds)

Gallery generated by Sphinx-Gallery