Extract stress/strain invariants - Static Simulation

In this script a static simulation is used as an example to show how to extract tensor’s invariants.

Perform required imports

Perform required imports. # This example uses a supplied file that you can get by importing the DPF examples package.

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()
simulation = post.load_simulation(example_path)

# for no autocompletion, this line is equivalent to:
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/3.8.16/x64/lib/python3.8/site-packages/ansys/dpf/core/examples/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
     -  structural_temperature: ElementalNodal 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 elemental nodal stress and strain

stress = simulation.stress(all_sets=True)
print(stress)

strain = simulation.elastic_strain(all_sets=True)
print(strain)

                results           S
                set_ids           1           2           3
element_ids  components
      18357      XX (1)  2.7979e+06  4.3949e+06  4.6183e+06
                 YY (1)  8.6092e+06  2.8565e+07  5.9405e+07
                 ZZ (1) -1.0166e+07 -2.6681e+06  2.2825e+07
                 XY (1)  5.9477e+05  7.8847e+05 -3.5088e+05
                 YZ (1) -1.9866e+08 -3.9727e+08 -5.9452e+08
                 XZ (1) -6.6205e+06 -4.0082e+06  7.6945e+06
        ...


                results        EPEL
                set_ids           1           2           3
element_ids  components
      18357      XX (1)  1.6326e-05 -1.6871e-05 -1.0025e-04
                 YY (1)  5.4098e-05  1.4024e-04  2.5586e-04
                 ZZ (1) -6.7943e-05 -6.2781e-05  1.8092e-05
                 XY (1)  7.7320e-06  1.0250e-05 -4.5614e-06
                 YZ (1) -2.5826e-03 -5.1645e-03 -7.7287e-03
                 XZ (1) -8.6066e-05 -5.2106e-05  1.0003e-04
        ...

Compute principal invariant averaged and unaveraged on stress and strain

princ_stress_1 = simulation.stress_principal(components=[1])
print(princ_stress_1)

nodal_princ_stress_2 = simulation.stress_principal_nodal(components=[2])
print(nodal_princ_stress_2)
nodal_princ_stress_2.plot()

nodal_princ_strain_2 = simulation.elastic_strain_principal_nodal(components=[2])
print(nodal_princ_strain_2)
nodal_princ_strain_2.plot()

• 
• 

                results           S
                set_ids           3
element_ids  components
      18357       1 (1)  6.3596e+08
      18357       1 (2)  5.3499e+08
      18357       1 (3)  6.6581e+08
      18357       1 (4)  4.2794e+08
      18357   1 (1) (1)  3.6762e+08
      18357   1 (1) (2)  2.3020e+08
        ...


                results           S
                set_ids           3
   node_ids  components
       4872           2 -1.4818e+06
       9005              3.1627e+05
       9373              4.0889e+07
       9372             -3.2059e+07
       4876              1.9911e+07
       9781             -1.1439e+08
        ...


                results        EPEL
                set_ids           3
   node_ids  components
       4872           2 -1.2351e-04
       9005             -1.2034e-04
       9373             -1.4734e-04
       9372              1.8417e-05
       4876              6.4584e-04
       9781              7.0507e-05
        ...

Compute Von Mises eqv averaged and unaveraged on stress and strain

stress_eqv = simulation.stress_eqv_von_mises(set_ids=[1])
print(stress_eqv)

nodal_stress_eqv = simulation.stress_eqv_von_mises_nodal(set_ids=[1])
nodal_stress_eqv.plot()

nodal_strain_eqv = simulation.elastic_strain_eqv_von_mises_nodal(set_ids=[1])
nodal_strain_eqv.plot()

• 
• 

    results           S
    set_ids           1
element_ids
      18357 (1)  3.4469e+08
      18357 (2)  2.8529e+08
      18357 (3)  3.1625e+08
      18357 (4)  2.8731e+08
      18357 (1)  3.3939e+08
      18357 (2)  2.7271e+08
        ...