.. DO NOT EDIT. .. THIS FILE WAS AUTOMATICALLY GENERATED BY SPHINX-GALLERY. .. TO MAKE CHANGES, EDIT THE SOURCE PYTHON FILE: .. "examples\14-lsdyna\01-lsdyna_beam.py" .. LINE NUMBERS ARE GIVEN BELOW. .. only:: html .. note:: :class: sphx-glr-download-link-note :ref:`Go to the end ` to download the full example code. .. rst-class:: sphx-glr-example-title .. _sphx_glr_examples_14-lsdyna_01-lsdyna_beam.py: .. _lsdyna_operators: Beam results manipulations -------------------------- This example provides an overview of the LS-DYNA beam results manipulations. .. note:: This example requires DPF 6.1 (ansys-dpf-server-2023-2-pre0) or above. For more information, see :ref:`ref_compatibility`. .. GENERATED FROM PYTHON SOURCE LINES 36-42 .. code-block:: Python import matplotlib.pyplot as plt from ansys.dpf import core as dpf from ansys.dpf.core import examples, operators as ops .. GENERATED FROM PYTHON SOURCE LINES 43-52 d3plot file data extraction ~~~~~~~~~~~~~~~~~~~~~~~~~~~~ Create the model and print its contents. This LS-DYNA d3plot file contains several individual results, each at different times. The d3plot file does not contain information related to Units. In this case, as the simulation was run through Mechanical, a ''file.actunits'' file is produced. If this file is supplemented in the data_sources, the units will be correctly fetched for all results in the file as well as for the mesh. .. GENERATED FROM PYTHON SOURCE LINES 52-60 .. code-block:: Python d3plot = examples.download_d3plot_beam() my_data_sources = dpf.DataSources() my_data_sources.set_result_file_path(d3plot[0], key="d3plot") my_data_sources.add_file_path(d3plot[3], key="actunits") my_model = dpf.Model(my_data_sources) print(my_model) .. rst-class:: sphx-glr-script-out .. code-block:: none DPF Model ------------------------------ Unknown analysis Unit system: NMM: mm, ton, N, s, mV, mA, degC Physics Type: Unknown Available results: - global_kinetic_energy: TimeFreq_steps Global Kinetic Energy - global_internal_energy: TimeFreq_steps Global Internal Energy - global_total_energy: TimeFreq_steps Global Total Energy - global_velocity: TimeFreq_steps Global Velocity - initial_coordinates: Nodal Initial Coordinates - coordinates: Nodal Coordinates - velocity: Nodal Velocity - acceleration: Nodal Acceleration - stress: Elemental Stress - stress_von_mises: Elemental Stress Von Mises - plastic_strain_eqv: Elemental Plastic Strain Eqv - total_strain: Elemental Total Strain - beam_axial_force: Elemental Beam Axial Force - beam_s_shear_force: Elemental Beam S Shear Force - beam_t_shear_force: Elemental Beam T Shear Force - beam_s_bending_moment: Elemental Beam S Bending Moment - beam_t_bending_moment: Elemental Beam T Bending Moment - beam_torsional_moment: Elemental Beam Torsional Moment - beam_axial_stress: Elemental Beam Axial Stress - beam_rs_shear_stress: Elemental Beam Rs Shear Stress - beam_tr_shear_stress: Elemental Beam Tr Shear Stress - beam_axial_plastic_strain: Elemental Beam Axial Plastic Strain - beam_axial_total_strain: Elemental Beam Axial Total Strain - history_variablesihv__[1__10]: Elemental History Variables(ihv: [1, 10]) - displacement: Nodal Displacement ------------------------------ DPF Meshed Region: 1940 nodes 2056 elements Unit: mm With solid (3D) elements, beam (1D) elements ------------------------------ DPF Time/Freq Support: Number of sets: 12 Cumulative Time (s) LoadStep Substep 1 0.000000 1 1 2 0.997460 2 1 3 1.997818 3 1 4 2.998237 4 1 5 3.998657 5 1 6 4.999076 6 1 7 5.999496 7 1 8 6.999915 8 1 9 7.997509 9 1 10 8.997929 10 1 11 9.998348 11 1 12 10.001174 12 1 .. GENERATED FROM PYTHON SOURCE LINES 61-72 Exploring the mesh ~~~~~~~~~~~~~~~~~~ The model has solid (3D) elements and beam (1D) elements. Some of the results only apply to one type of elements (such as the stress tensor for solids, or the axial force for beams, for example). By splitting the mesh by element shape we see that the ball is made by the solid 3D elements and the plate by the beam 1D elements - Define the analysis mesh .. GENERATED FROM PYTHON SOURCE LINES 72-85 .. code-block:: Python my_meshed_region = my_model.metadata.meshed_region # - Get separate meshes for each body my_meshes = ops.mesh.split_mesh( mesh=my_meshed_region, property=dpf.common.elemental_properties.element_shape ).eval() # - Define the meshes for each body in separate variables ball_mesh = my_meshes.get_mesh(label_space_or_index={"body": 1, "elshape": 1}) plate_mesh = my_meshes.get_mesh(label_space_or_index={"body": 2, "elshape": 2}) print(my_meshes) .. rst-class:: sphx-glr-script-out .. code-block:: none DPF Meshes Container with 2 mesh(es) defined on labels: body elshape with: - mesh 0 {body: 1, elshape: 1, } with 1651 nodes and 1512 elements. - mesh 1 {body: 2, elshape: 2, } with 289 nodes and 544 elements. .. GENERATED FROM PYTHON SOURCE LINES 86-87 Plate mesh .. GENERATED FROM PYTHON SOURCE LINES 87-91 .. code-block:: Python print("Plate mesh", "\n", plate_mesh) plate_mesh.plot(title="Plate mesh", text="Plate mesh") .. image-sg:: /examples/14-lsdyna/images/sphx_glr_01-lsdyna_beam_001.png :alt: 01 lsdyna beam :srcset: /examples/14-lsdyna/images/sphx_glr_01-lsdyna_beam_001.png :class: sphx-glr-single-img .. rst-class:: sphx-glr-script-out .. code-block:: none Plate mesh DPF Meshed Region: 289 nodes 544 elements Unit: mm With beam (1D) elements .. GENERATED FROM PYTHON SOURCE LINES 92-93 Ball mesh .. GENERATED FROM PYTHON SOURCE LINES 93-97 .. code-block:: Python print("Ball mesh", "\n", ball_mesh, "\n") ball_mesh.plot(title="Ball mesh", text="Ball mesh") .. image-sg:: /examples/14-lsdyna/images/sphx_glr_01-lsdyna_beam_002.png :alt: 01 lsdyna beam :srcset: /examples/14-lsdyna/images/sphx_glr_01-lsdyna_beam_002.png :class: sphx-glr-single-img .. rst-class:: sphx-glr-script-out .. code-block:: none Ball mesh DPF Meshed Region: 1651 nodes 1512 elements Unit: mm With solid (3D) elements .. GENERATED FROM PYTHON SOURCE LINES 98-102 Scoping ~~~~~~~ - Define the mesh scoping to use it with the operators .. GENERATED FROM PYTHON SOURCE LINES 102-104 .. code-block:: Python my_meshes_scoping = ops.scoping.split_on_property_type(mesh=my_meshed_region).eval() .. GENERATED FROM PYTHON SOURCE LINES 105-106 - Define the mesh scoping for each body/element shape in separate variables .. GENERATED FROM PYTHON SOURCE LINES 106-109 .. code-block:: Python ball_scoping = my_meshes_scoping.get_scoping(label_space_or_index={"elshape": 1}) plate_scoping = my_meshes_scoping.get_scoping(label_space_or_index={"elshape": 2}) .. GENERATED FROM PYTHON SOURCE LINES 110-112 - We will plot the results in a mesh deformed by the displacement. The displacement is in a nodal location, so we need to define a nodal scoping for the plate .. GENERATED FROM PYTHON SOURCE LINES 112-116 .. code-block:: Python plate_scoping_nodal = dpf.operators.scoping.transpose( mesh_scoping=plate_scoping, meshed_region=my_meshed_region ).eval() .. GENERATED FROM PYTHON SOURCE LINES 117-139 Beam results ~~~~~~~~~~~~ The next manipulations can be applied to the following beam operators that handle the correspondent results : - beam_axial_force: Beam Axial Force - beam_s_shear_force: Beam S Shear Force - beam_t_shear_force: Beam T Shear Force - beam_s_bending_moment: Beam S Bending Moment - beam_t_bending_moment: Beam T Bending Moment - beam_torsional_moment: Beam Torsional Moment - beam_axial_stress: Beam Axial Stress - beam_rs_shear_stress: Beam Rs Shear Stress - beam_tr_shear_stress: Beam Tr Shear Stress - beam_axial_plastic_strain: Beam Axial Plastic Strain - beam_axial_total_strain: Beam Axial Total Strain We do not demonstrate separately how to use each of them in this example once they have similar methods. So, if you want to operate on other operator, uou just need to change their scripting name in the code lines. .. GENERATED FROM PYTHON SOURCE LINES 141-143 Comparing results in different time steps ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~ .. GENERATED FROM PYTHON SOURCE LINES 143-229 .. code-block:: Python # 1) Define the time steps set time_steps_set = [2, 6, 12] # 2) Prepare the collections to store the results for each time step # a. To compare the results in the same image you have to copy the mesh for each plot plate_meshes = dpf.MeshesContainer() plate_meshes.add_label("time") # b. The displacements for each time steps to deform the mesh accordingly plate_displacements = dpf.FieldsContainer() plate_displacements.add_label(label="time") # c. The axial force results for each time steps. Here plate_axial_force = dpf.FieldsContainer() plate_axial_force.add_label(label="time") # 3) Use the Plotter class to add the plots in the same image comparison_plot = dpf.plotter.DpfPlotter() # Side bar arguments definition side_bar_args = dict( title="Beam axial force (N)", fmt="%.2e", title_font_size=15, label_font_size=15 ) # 4) As we want to compare the results in the same plot we will need this variable. # It represents the distance between the meshes j = -400 # 5) Copy the mesh of interest. Here it is the plate mesh that we copy along the X axis # Here we use a loop where each iteration correspond to the manipulations for a given time step for i in time_steps_set: # Loop through the time steps # Copy the mesh plate_meshes.add_mesh(label_space={"time": i}, mesh=plate_mesh.deep_copy()) # 6) Get the plot coordinates that will be changed (so we can compare the results side by side) coords_to_update = plate_meshes.get_mesh( label_space_or_index={"time": i} ).nodes.coordinates_field # 7) Define the coordinates where the new mesh will be placed overall_field = dpf.fields_factory.create_3d_vector_field( num_entities=1, location=dpf.locations.overall ) overall_field.append(data=[j, 0.0, 0.0], scopingid=1) # 8) Define the updated coordinates new_coordinates = ops.math.add(fieldA=coords_to_update, fieldB=overall_field).eval() coords_to_update.data = new_coordinates.data # 9) Extract the result, here we start by getting the beam_rs_shear_stress plate_axial_force.add_field( label_space={"time": i}, field=my_model.results.beam_axial_force( time_scoping=i, mesh_scoping=plate_scoping_nodal ).eval()[0], ) # 10) We will also get the displacement to deform the mesh plate_displacements.add_field( label_space={"time": i}, field=my_model.results.displacement( time_scoping=i, mesh_scoping=plate_scoping_nodal ).eval()[0], ) # 11) Add the result and the mesh to the plot comparison_plot.add_field( field=plate_axial_force.get_field(label_space_or_index={"time": i}), meshed_region=plate_meshes.get_mesh(label_space_or_index={"time": i}), deform_by=plate_displacements.get_field(label_space_or_index={"time": i}), scalar_bar_args=side_bar_args, ) comparison_plot.add_node_labels( nodes=[289], labels=[f"Time step = {i}"], meshed_region=plate_meshes.get_mesh(label_space_or_index={"time": i}), font_size=10, ) # 12) Increment the coordinate value for the loop j = j - 400 # Visualise the plot comparison_plot.show_figure() .. image-sg:: /examples/14-lsdyna/images/sphx_glr_01-lsdyna_beam_003.png :alt: 01 lsdyna beam :srcset: /examples/14-lsdyna/images/sphx_glr_01-lsdyna_beam_003.png :class: sphx-glr-single-img .. GENERATED FROM PYTHON SOURCE LINES 230-238 Plot a graph over time for the elements with max and min results values ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~ Here we make a workflow with a more verbose approach. This is useful because we use operators having several matching inputs or outputs. So the connexions are more clear, and it is easier to use and reuse the workflow. The following workflow finds the element with the max values over all the time steps and return its ID .. GENERATED FROM PYTHON SOURCE LINES 238-261 .. code-block:: Python # Define the workflow object max_workflow = dpf.Workflow() max_workflow.progress_bar = False # Define the norm operator max_norm = ops.math.norm_fc() # Define the max of each entity with the evaluated norm as an input max_per_ent = ops.min_max.min_max_by_entity(fields_container=max_norm.outputs.fields_container) # Define the max over all entities global_max = ops.min_max.min_max(field=max_per_ent.outputs.field_max) # Get the scoping max_scop = ops.utility.extract_scoping(field_or_fields_container=global_max.outputs.field_max) # Get the id max_id = ops.scoping.scoping_get_attribute( scoping=max_scop.outputs.mesh_scoping_as_scoping, property_name="ids" ) # Add the operators to the workflow max_workflow.add_operators(operators=[max_norm, max_per_ent, global_max, max_scop, max_id]) max_workflow.set_input_name("fields_container", max_norm.inputs.fields_container) max_workflow.set_output_name("max_id", max_id.outputs.property_as_vector_int32_) max_workflow.set_output_name("max_entity_scoping", max_scop.outputs.mesh_scoping_as_scoping) .. GENERATED FROM PYTHON SOURCE LINES 262-265 Using the workflow to the stresses results on the plate: - Extract the results .. GENERATED FROM PYTHON SOURCE LINES 265-280 .. code-block:: Python # Get all the time steps time_all = my_model.metadata.time_freq_support.time_frequencies # Extract all the stresses results on the plate plate_beam_axial_stress = my_model.results.beam_axial_stress( time_scoping=time_all, mesh_scoping=plate_scoping ).eval() plate_beam_rs_shear_stress = my_model.results.beam_rs_shear_stress( time_scoping=time_all, mesh_scoping=plate_scoping ).eval() plate_beam_tr_shear_stress = my_model.results.beam_tr_shear_stress( time_scoping=time_all, mesh_scoping=plate_scoping ).eval() .. GENERATED FROM PYTHON SOURCE LINES 281-283 - As we will use the workflow for different results operators we group them and use a loop through the group. Here we prepare where the workflow outputs will be stored .. GENERATED FROM PYTHON SOURCE LINES 283-299 .. code-block:: Python # List of operators to be used in the workflow beam_stresses = [plate_beam_axial_stress, plate_beam_rs_shear_stress, plate_beam_tr_shear_stress] graph_labels = [ "Beam axial stress", "Beam rs shear stress", "Beam tr shear stress", ] # List of elements ids that we will get from the workflow max_stress_elements_ids = [] # Scopings container max_stress_elements_scopings = dpf.ScopingsContainer() max_stress_elements_scopings.add_label("stress_result") .. GENERATED FROM PYTHON SOURCE LINES 300-304 - The following loop: a) Goes through each stress result and get the element id with maximum solicitation b) Re-escope the fields container to keep only the data for this element c) Plot a stress x time graph .. GENERATED FROM PYTHON SOURCE LINES 304-343 .. code-block:: Python for j in range(0, len(beam_stresses)): # Loop through each stress result # Use the pre-defined workflow to define the element with maximum solicitation max_workflow.connect(pin_name="fields_container", inpt=beam_stresses[j]) max_stress_elements_ids.append( max_workflow.get_output(pin_name="max_id", output_type=dpf.types.vec_int) ) max_stress_elements_scopings.add_scoping( label_space={"stress_result": j}, scoping=max_workflow.get_output( pin_name="max_entity_scoping", output_type=dpf.types.scoping ), ) # Re-scope the results to keep only the data for the identified element beam_stresses[j] = ops.scoping.rescope_fc( fields_container=beam_stresses[j], mesh_scoping=max_stress_elements_scopings.get_scoping( label_space_or_index={"stress_result": j} ), ).eval() # The d3plot file gives us fields containers labeled by time. So in each field we have the stress value in a # given time for the chosen element. We need to rearrange the fields container into fields. beam_stresses[j] = ops.utility.merge_to_field_matrix(fields1=beam_stresses[j]).eval() plt.plot( time_all.data, beam_stresses[j].data[0], label=f"{graph_labels[j]}, element id:{max_stress_elements_ids[j][0]}", ) # Graph formatting plt.title("Beam stresses evolution") plt.xlabel("Time (s)") plt.ylabel("Beam stresses (MPa)") plt.legend() plt.show() .. image-sg:: /examples/14-lsdyna/images/sphx_glr_01-lsdyna_beam_004.png :alt: Beam stresses evolution :srcset: /examples/14-lsdyna/images/sphx_glr_01-lsdyna_beam_004.png :class: sphx-glr-single-img .. GENERATED FROM PYTHON SOURCE LINES 344-360 Results coordinates system ~~~~~~~~~~~~~~~~~~~~~~~~~~ The general results are given in the Cartesian coordinates system by default. The beam results are given directly in the local directions as scalars. For example the beam stresses we have: - The axial stress, given in the beam axis - The stresses defined in the cross-section directions: tr stress in the transverse direction (t) and rs stress perpendicular to the tr direction (s). Unfortunately there are no operators for LS-DYNA files that directly allows you to: - Rotate results from local coordinate system to global coordinate system; - Extract the rotation matrix between the local and global coordinate systems; .. rst-class:: sphx-glr-timing **Total running time of the script:** (0 minutes 7.123 seconds) .. _sphx_glr_download_examples_14-lsdyna_01-lsdyna_beam.py: .. only:: html .. container:: sphx-glr-footer sphx-glr-footer-example .. container:: sphx-glr-download sphx-glr-download-jupyter :download:`Download Jupyter notebook: 01-lsdyna_beam.ipynb <01-lsdyna_beam.ipynb>` .. container:: sphx-glr-download sphx-glr-download-python :download:`Download Python source code: 01-lsdyna_beam.py <01-lsdyna_beam.py>` .. container:: sphx-glr-download sphx-glr-download-zip :download:`Download zipped: 01-lsdyna_beam.zip <01-lsdyna_beam.zip>` .. only:: html .. rst-class:: sphx-glr-signature `Gallery generated by Sphinx-Gallery `_