Validate external layer results with the full mesh

This example shows postprocessing comparisons based on how results and the mesh are extracted:

• Results and mesh extracted only on the external layer

• Results and mesh extracted on the entire mesh

The external layer is the layer of solid elements with at least one facet facing the outside of the geometry.

This feature, available for all types of mechanical simulation, allows you to reduce the size of both the mesh and extracted data to improve processing performance. Because larger stresses 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

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/3.10.16/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 over the entire mesh and on the external layer.

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

print(
    f"number of nodes with external_layer=True: {len(displacement_ext.index.mesh_index)}"
)
print(
    f"number of nodes with external_layer=False: {len(displacement.index.mesh_index)}"
)

• 
• 

number of nodes with external_layer=True: 64079
number of nodes with external_layer=False: 69762

Extract stress and strain data

Extract stress and elastic strain data over the entire mesh and on the external layer. You can easily compute averages and invariants on the external layer because the connectivity of the kept elements remains unchanged.

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

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

elastic_strain_eqv_ext = simulation.elastic_strain_eqv_von_mises_nodal(
    external_layer=True
)
elastic_strain_eqv = simulation.elastic_strain_eqv_von_mises_nodal()
elastic_strain_eqv_ext.plot()
elastic_strain_eqv.plot()

• 
• 
• 
• 

number of elements with external_layer=True: 31374
number of elements with external_layer=False: 39315