Reduce Model Size by using Mesh Skin for Result and Mesh extraction

This example displays post-processing on a mesh skin for a static analysis. The skin mesh is rebuilt with new surface elements connecting the nodes on the external skin of the solid mesh. These surface elements types are chosen with respect to the solid elements facets having all their nodes on the skin. 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 results on the skin gives equivalent maximum values in most cases. Post-processing of elemental or elemental nodal results requires element solid to skin mapping to get from a solid element result to a facet result. The connectivity of the new surface elements built on the skin being different from the connectivity of the solid elements, small differences can be found after result averaging.

Perform required imports

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

from ansys.dpf import post
from ansys.dpf.post 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
print(simulation)

Static Mechanical Simulation.


Data Sources
------------------------------
/opt/hostedtoolcache/Python/3.10.14/x64/lib/python3.10/site-packages/ansys/dpf/core/examples/result_files/crankshaft/crankshaft.rst

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
     -  element_euler_angles: ElementalNodal Element Euler Angles
     -  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 skin.

displacement_skin = simulation.displacement(skin=True)
displacement_skin.plot()

print(f"number of nodes with skin=True: {len(displacement_skin.index.mesh_index)}")
print(f"number of nodes with skin=False: {len(simulation.mesh.node_ids)}")

number of nodes with skin=True: 32922
number of nodes with skin=False: 69762

Extract stress/strain data

Extract stress or elastic strain data and on the skin. Averaging, and invariants computation are done through a solid to skin connectivity mapping.

elemental_stress_skin = simulation.stress_principal_elemental(components=[1], skin=True)
elemental_stress_skin.plot()

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


elastic_strain_eqv_skin = simulation.elastic_strain_eqv_von_mises_nodal(skin=True)
elastic_strain_eqv_skin.plot()

• 
• 

number of elements with skin=True: 16460
number of elements with skin=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)):
    elements.append(all_elements[i])
elemental_stress_skin = simulation.stress_principal_elemental(skin=elements)
elemental_stress_skin.plot()