Extract results on named selections - Modal Simulation

In this script static simulation is processed to extract results like stress, displacement. Selecting sub parts of the results by scoping on specific nodes, elements is also displayed here.

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_modal_frame()
# to automatically detect the simulation type, use:
simulation = post.load_simulation(example_path)

# to enable auto-completion, use the equivalent:
simulation = post.ModalMechanicalSimulation(example_path)

# print the simulation to get an overview of what's available
print(simulation)

Modal Mechanical Simulation.


Data Sources
------------------------------
/opt/hostedtoolcache/Python/3.10.15/x64/lib/python3.10/site-packages/ansys/dpf/core/examples/result_files/modal/frame.rst

DPF Model
------------------------------
Modal analysis
Unit system: NMM: mm, ton, N, s, mV, mA, degC
Physics Type: Mechanical
Available results:
     -  displacement: Nodal Displacement
     -  stress: ElementalNodal Stress
     -  elastic_strain: ElementalNodal Strain
     -  element_euler_angles: ElementalNodal Element Euler Angles
------------------------------
DPF  Meshed Region:
  5886 nodes
  2842 elements
  Unit: mm
  With solid (3D) elements
------------------------------
DPF  Time/Freq Support:
  Number of sets: 6
Cumulative     Frequency (Hz) LoadStep       Substep
1              253.615690     1              1
2              317.918491     1              2
3              329.825709     1              3
4              575.619678     1              4
5              621.973976     1              5
6              667.364882     1              6

Get the available named selections

print(simulation.named_selections)

['BAR_1', 'BAR_2', 'FACES_INTERIOR_PINS', '_FIXEDSU']

Extract displacements on named selections

bar1_tot_displacement = simulation.displacement(named_selections=["BAR_1"], norm=True)
print(bar1_tot_displacement)
bar1_tot_displacement.plot()

bar2_tot_displacement = simulation.displacement(named_selections=["BAR_2"], norm=True)
print(bar2_tot_displacement)
bar2_tot_displacement.plot()

# both
tot_displacement = simulation.displacement(
    named_selections=["BAR_1", "BAR_2"], norm=True
)
print(tot_displacement)
tot_displacement.plot()

• 
• 
• 

 results   U_N (mm)
 set_ids          1
node_ids
      72 6.2179e-01
      73 5.0563e-01
      74 2.4093e-01
      75 2.2909e-01
      76 4.8153e-01
      77 4.7876e+00
     ...        ...


 results   U_N (mm)
 set_ids          1
node_ids
      17 5.0483e-01
      18 7.7196e-01
      19 1.2061e+00
      20 2.1481e+00
      21 3.3862e+00
      22 0.0000e+00
     ...        ...


 results   U_N (mm)
 set_ids          1
node_ids
      72 6.2179e-01
      73 5.0563e-01
      74 2.4093e-01
      75 2.2909e-01
      76 4.8153e-01
      77 4.7876e+00
     ...        ...

Extract stress and averaged stress on named selections

eqv_stress = simulation.stress_eqv_von_mises_nodal(named_selections=["_FIXEDSU"])
print(eqv_stress)

# without selection
elemental_stress = simulation.stress_elemental(named_selections=["BAR_1"])
print(elemental_stress)
elemental_stress.plot()

 results S_VM (MPa)
 set_ids          1
node_ids
      22 8.0765e+02
     349 1.0934e+03
      15 1.0859e+03
     371 7.3710e+02
     406 3.4030e+02
     408 4.1398e+02
     ...        ...


               results    S (MPa)
               set_ids          1
element_ids components
       1137         XX 2.1033e+02
                    YY 1.4585e+02
                    ZZ 6.4862e+02
                    XY 7.8062e+00
                    YZ 3.9888e+01
                    XZ 1.3070e+01
        ...        ...        ...