Static analysis

This example shows how you can postprocess a result file for a static analysis using DPF-Post.

Perform required imports

Perform required imports.

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 a static analysis computed in Ansys Mechanical.

example_path = examples.download_all_kinds_of_complexity()

solution = post.load_solution(example_path)
print(solution)

Static Analysis Solution object.


Data Sources
------------------------------
DPF  DataSources:
  Result files:
     result key: rst and path: /opt/hostedtoolcache/Python/3.8.16/x64/lib/python3.8/site-packages/ansys/dpf/core/examples/testing/allKindOfComplexity.rst
  Secondary files:


DPF Model
------------------------------
Static analysis
Unit system: MKS: m, kg, N, s, V, A, degC
Physics Type: Mechanical
Available results:
     -  displacement: Nodal Displacement
     -  reaction_force: Nodal Force
     -  element_nodal_forces: ElementalNodal Element nodal Forces
     -  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
     -  thermal_strain: ElementalNodal Thermal Strains
     -  thermal_strains_eqv: ElementalNodal Thermal Strains eqv
     -  swelling_strains: ElementalNodal Swelling Strains
     -  structural_temperature: ElementalNodal Temperature
------------------------------
DPF  Meshed Region:
  15129 nodes
  10292 elements
  Unit: m
  With solid (3D) elements, shell (2D) elements, shell (3D) elements, beam (1D) elements
------------------------------
DPF  Time/Freq Support:
  Number of sets: 1
Cumulative     Time (s)       LoadStep       Substep
1              1.000000       1              1

Get Result objects

Get displacement result

Get the displacement Result object.

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

Displacement result.

This result has been computed using dpf.core.Operator objects, which
have been chained together according to the following list:
- U: Result operator. Compute the desired result.

Check number of fields

Check the number of fields.

disp.num_fields

1

Get data from field

Get data from a field.

disp.get_data_at_field(0)

DPFArray([[ 9.84182297e-06,  5.13025031e-06, -6.66435651e-07],
          [ 9.95996777e-06,  4.93526360e-06, -6.25236961e-07],
          [ 9.93154893e-06,  5.88552090e-06, -7.83251832e-07],
          ...,
          [ 5.00000000e-03, -1.54556837e-04,  0.00000000e+00],
          [ 5.00000000e-03, -1.56813550e-04,  0.00000000e+00],
          [ 5.00000000e-03, -1.66125455e-04,  0.00000000e+00]])

Get maximum data value over all fields

Get the maximum data value over all fields.

disp.max_data

DPFArray([[8.50619058e+04, 1.04659292e+01, 3.73620870e+05]])

Get minimum data value over all fields

Get the minimum data value over all fields.

disp.min_data

DPFArray([[-1.82645944e-06, -1.04473039e+01, -2.94677257e-04]])

Get maximum data value over targeted field

Get the maximum data value over a targeted field.

disp.get_max_data_at_field(0)

DPFArray([8.50619058e+04, 1.04659292e+01, 3.73620870e+05])

Get minimum data value over all fields

Get the minimum data value over all fields.

disp.get_min_data_at_field(0)

DPFArray([-1.82645944e-06, -1.04473039e+01, -2.94677257e-04])

Get stress result

Get the stress Result object for a tensor.

stress_result = solution.stress()
stress = stress_result.tensor

Check number of fields

Check the number of shell and solid elements in distinct fields.

stress.num_fields

2

Get shell field

Get the shell field.

shell_field = stress[0]
shell_field.shell_layers

<shell_layers.nonelayer: 5>

Get solid field

Get the solid field.

solid_field = stress[1]

Plot contour

Plot the contour.

stress.plot_contour()

Get elastic strain result

Get an elastic strain result.

elastic_strain_result = solution.elastic_strain()
elastic_strain = elastic_strain_result.tensor

Check number of fields

Check the number of shell and solid elements in distinct fields.

elastic_strain.num_fields

2

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

print(solution.plastic_strain())

Tensor object.

Object properties:
 - location   : Nodal

Plastic strain object.

You can also use this method to get the temperature result.

print(solution.structural_temperature())

Scalar object.

Object properties:
 - location   : Nodal

Structural temperature object.