Reduce Model Size by using Mesh External Layer for Result and Mesh extraction#

This example displays post-processing on a mesh external layer for a static analysis. The external layer is the layer of solid elements with at least one facet facing the outside of the geometry. This feature is available for all types of Mechanical simulation, and allows you to reduce the size of the mesh and of the extracted data to improve processing performance. Since larger stress and strains are usually located on the skin of a model, computing the results on the external layer provides equivalent maximum values in most cases.

Perform required imports#

This example uses a supplied file that you can get using the examples module.

from ansys.dpf import post
from import examples

Get Simulation object#

Get the Simulation object that allows access to the result. The Simulation object must be instantiated with the path for the result file. For example, "C:/Users/user/my_result.rst" on Windows or "/home/user/my_result.rst" on Linux.

example_path = examples.download_crankshaft()
# to automatically detect the simulation type, use:
simulation = post.load_simulation(example_path)

# to enable auto-completion, use the equivalent:
simulation = post.StaticMechanicalSimulation(example_path)

# print the simulation to get an overview of what's available
Static Mechanical Simulation.

Data Sources

DPF Model
Static analysis
Unit system: MKS: m, kg, N, s, V, A, degC
Physics Type: Mechanical
Available results:
     -  displacement: Nodal Displacement
     -  velocity: Nodal Velocity
     -  acceleration: Nodal Acceleration
     -  reaction_force: Nodal Force
     -  stress: ElementalNodal Stress
     -  elemental_volume: Elemental Volume
     -  stiffness_matrix_energy: Elemental Energy-stiffness matrix
     -  artificial_hourglass_energy: Elemental Hourglass Energy
     -  thermal_dissipation_energy: Elemental thermal dissipation energy
     -  kinetic_energy: Elemental Kinetic Energy
     -  co_energy: Elemental co-energy
     -  incremental_energy: Elemental incremental energy
     -  elastic_strain: ElementalNodal Strain
     -  structural_temperature: ElementalNodal Structural temperature
DPF  Meshed Region:
  69762 nodes
  39315 elements
  Unit: m
  With solid (3D) elements
DPF  Time/Freq Support:
  Number of sets: 3
Cumulative     Time (s)       LoadStep       Substep
1              1.000000       1              1
2              2.000000       1              2
3              3.000000       1              3

Extract displacement data#

Extract displacement data on the external layer.

displacement_ext = simulation.displacement(
)  # default is external_layer=False

    f"number of nodes with external_layer=True: {len(displacement_ext.index.mesh_index)}"
print(f"number of nodes with external_layer=False: {len(simulation.mesh.node_ids)}")
01 mesh external layer
number of nodes with external_layer=True: 64079
number of nodes with external_layer=False: 69762

Extract stress/strain data#

Extract stress or elastic strain data on the external layer. Averaging, and invariants computation can easily be done on the external layer since the connectivity of the external layer elements remains unchanged.

elemental_stress_ext = simulation.stress_principal_elemental(
    components=[1], external_layer=True

    f"number of elements with external_layer=True: {len(elemental_stress_ext.index.mesh_index)}"
    f"number of elements with external_layer=False: {len(simulation.mesh.element_ids)}"

elastic_strain_eqv_ext = simulation.elastic_strain_eqv_von_mises_nodal(
  • 01 mesh external layer
  • 01 mesh external layer
number of elements with external_layer=True: 31374
number of elements with external_layer=False: 39315

Extract the external layer on a selection of elements#

all_elements = simulation.mesh.element_ids
elements = []
for i in range(0, int(all_elements.size / 2)):
elemental_stress_ext = simulation.stress_principal_elemental(external_layer=elements)
01 mesh external layer

Extract the external layer on a selection of elements for nodal results#

elastic_strain_eqv_ext = simulation.elastic_strain_eqv_von_mises_nodal(
01 mesh external layer

Extract the external layer on a selection of elements and scope results#

sub_elements = []
for i in range(0, int(len(elements) / 2)):
elemental_stress_ext = simulation.stress_principal_elemental(
    external_layer=elements, element_ids=sub_elements
01 mesh external layer

Total running time of the script: ( 0 minutes 8.146 seconds)

Gallery generated by Sphinx-Gallery