Get data from a static simulation

This example shows how to get data from a previously stored static simulation. The available results can be listed to see what results can be retrieved.

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 that allows access to the result. The Solution 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.

simulation = post.load_simulation(examples.static_rst)
print(simulation)

Static Mechanical Simulation.


Data Sources
------------------------------
DPF  DataSources:
  Result files:
     result key: rst and path: /opt/hostedtoolcache/Python/3.10.16/x64/lib/python3.10/site-packages/ansys/dpf/core/examples/result_files/static.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
     -  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:
  81 nodes
  8 elements
  Unit: m
  With solid (3D) elements
------------------------------
DPF  Time/Freq Support:
  Number of sets: 1
Cumulative     Time (s)       LoadStep       Substep
1              1.000000       1              1

Get and plot displacements

displacement = simulation.displacement()

Print information

print(displacement._fc)

DPF displacement(s)Fields Container
  with 1 field(s)
  defined on labels: time

  with:
  - field 0 {time:  1} with Nodal location, 3 components and 81 entities.

Plot displacements

displacement._fc[0].plot()

Get and plot stresses

Get the “XY” stress component averaged on nodes.

stress = simulation.stress_nodal(components="XY")

Print information.

print(stress._fc)

DPF stress(s)Fields Container
  with 1 field(s)
  defined on labels: time

  with:
  - field 0 {time:  1} with Nodal location, 1 components and 81 entities.

Plot available stresses.

stress._fc[0].plot()

Get stresses at only five nodes

Get stresses at only the first five nodes using their IDs.

stress_nodes = simulation.stress_nodal(node_ids=range(1, 6))

Print information.

print(stress_nodes._fc)

DPF stress(s)Fields Container
  with 1 field(s)
  defined on labels: time

  with:
  - field 0 {time:  1} with Nodal location, 6 components and 5 entities.

Plot stresses.

stress_nodes._fc[0].plot()

Get stresses in a named selection

Get the name of the first named selection in the simulation.

ns = simulation.named_selections[0]
# Get nodal stresses for this named selection
stress_named_sel = simulation.stress_nodal(named_selections=ns)

Print information.

print(stress_named_sel._fc)

DPF stress(s)Fields Container
  with 1 field(s)
  defined on labels: time

  with:
  - field 0 {time:  1} with Nodal location, 6 components and 21 entities.

Plot stresses.

stress_named_sel._fc[0].plot()

Get stresses in a few elements

Get stresses only for a few elements selected by their IDs.

stress_elements = simulation.stress_nodal(element_ids=[1, 2, 3])

Print information.

print(stress_elements._fc)

DPF stress(s)Fields Container
  with 1 field(s)
  defined on labels: time

  with:
  - field 0 {time:  1} with Nodal location, 6 components and 44 entities.

Plot stresses.

stress_elements._fc[0].plot()

Get elemental streses and raw stresses

Get elemental stresses and print information.

stress_elements = simulation.stress_elemental()
print(stress_elements._fc)

DPF stress(s)Fields Container
  with 1 field(s)
  defined on labels: time

  with:
  - field 0 {time:  1} with Elemental location, 6 components and 8 entities.

Get raw stresses (ElementalNodal) and print information.

stress_raw = simulation.stress()
print(stress_raw._fc)

DPF stress(s)Fields Container
  with 1 field(s)
  defined on labels: time

  with:
  - field 0 {time:  1} with ElementalNodal location, 6 components and 8 entities.