Postprocess the result file for a harmonic analysis

This example shows how to use the legacy PyDPF-Post API to postprocess a result file for a harmonic analysis.

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 Solution object

Get the Solution object. This example loads a result file for an harmonic analysis computed in Ansys Mechanical.

example_path = examples.download_all_kinds_of_complexity()

solution = post.load_solution(examples.complex_rst)
print(solution)

Harmonic Analysis Solution object.


Data Sources
------------------------------
DPF  DataSources:
  Result files:
     result key: rst and path: /opt/hostedtoolcache/Python/3.10.18/x64/lib/python3.10/site-packages/ansys/dpf/core/examples/result_files/complex.rst
  Secondary files:


DPF Model
------------------------------
Harmonic analysis
Unit system: MKS: m, kg, N, s, V, A, degC
Physics Type: Mechanical
Available results:
     -  displacement: Nodal Displacement
     -  electric_potential: Nodal Electric Potential
     -  reaction_force: Nodal Force
     -  stress: ElementalNodal Stress
     -  elemental_volume: Elemental Volume
     -  stiffness_matrix_energy: Elemental Energy-stiffness matrix
     -  artificial_hourglass_energy: Elemental Hourglass Energy
     -  kinetic_energy: Elemental Kinetic Energy
     -  co_energy: Elemental co-energy
     -  incremental_energy: Elemental incremental energy
     -  thermal_dissipation_energy: Elemental thermal dissipation energy
     -  electric_field: ElementalNodal Electric field
     -  elastic_strain: ElementalNodal Strain
     -  elastic_strain_eqv: ElementalNodal Strain eqv
     -  electric_flux_density: ElementalNodal Electric flux density
     -  current_density: Elemental Current Density
     -  nmisc: Elemental Elemental Non Summable Miscellaneous Data
     -  elemental_heat_generation: Elemental Elemental Heat Generation
     -  structural_temperature: ElementalNodal Structural temperature
------------------------------
DPF  Meshed Region:
  4802 nodes
  657 elements
  Unit: m
  With solid (3D) elements
------------------------------
DPF  Time/Freq Support:
  Number of sets: 1
  With complex values

Cumulative     Frequency (Hz) LoadStep       Substep        RPM
1              343478.200000  1              1              0.000000

This may contain complex results.

Get Result objects

Get displacement result

The displacement result contains a field for real values and a field for imaginary values.

disp_result = solution.displacement()
disp = disp_result.vector

Get number of fields

disp.num_fields

2

Get data from field

disp.get_data_at_field(0)

DPFArray([[ 2.65783929e-09, -5.98949034e-10,  8.34267891e-11],
          [ 2.63846617e-09, -3.00204960e-10,  8.27306877e-11],
          [ 2.50179982e-09, -2.86371281e-10,  6.29386453e-11],
          ...,
          [-1.70840238e-09, -2.73504676e-09,  3.48706947e-11],
          [-1.57038405e-09, -2.71125223e-09,  6.79105278e-11],
          [-1.57311157e-09, -2.71904943e-09,  0.00000000e+00]],
         shape=(4802, 3))

Get maximum data value over all fields

disp.max_data

DPFArray([[2.76941713e-09, 2.76940199e-09, 4.10914311e-10],
          [6.53706736e-13, 6.53416337e-13, 9.25220948e-14]])

Get minimum data value over all fields

disp.min_data

DPFArray([[-2.76946046e-09, -2.76952549e-09,  0.00000000e+00],
          [-6.53727285e-13, -6.53452004e-13, -1.66091913e-13]])

Get maximum data value over targeted field

disp.get_max_data_at_field(0)

DPFArray([2.76941713e-09, 2.76940199e-09, 4.10914311e-10])

Get minimum data value over all fields

disp.get_min_data_at_field(0)

DPFArray([-2.76946046e-09, -2.76952549e-09,  0.00000000e+00])

Get stress result

Get a stress result that deals with amplitude. It contains a field for real values and a field for imaginary values.

stress_result = solution.stress()

Check if support has complex frequencies

stress_result.has_complex_frequencies()

True

Get tensor result

stress = stress_result.tensor

Get number of fields

Get the number of shell and solid elements in distinct fields. Because shell and solid elements are in distinct fields, you get four fields: the solid-real one, the solid-imaginary one, the shell-real one, and the shell-imaginary one.

stress.num_fields

2

Get shell field

shell_field = stress[0]
shell_field.shell_layers

<shell_layers.nonelayer: 5>

Get solid field

solid_field = stress[1]

Plot amplitude contour

amplitude = stress_result.tensor_amplitude
amplitude.plot_contour()

Get elastic strain result

Get an elastic strain result that deals with phase. It contains a field for real values and a field for imaginary values.

elastic_strain_result = solution.elastic_strain()
elastic_strain = elastic_strain_result.tensor
# shell and solid elements are in distinct fields.
elastic_strain.num_fields

2

The phase must be a float value. The unit is degrees.

es_at_phase = elastic_strain_result.tensor_at_phase(39.0)
es_at_phase.max_data
es_at_phase.num_fields
real_field = elastic_strain_result.tensor_at_phase(0.0)
img_field = elastic_strain_result.tensor_at_phase(90.0)

If the result file contains results, use this method to get the elastic strain result.

print(solution.elastic_strain())

Complex tensor object.

Tensor object.

Object properties:
 - location   : Nodal

Complex elastic strain object.