Basic DPF-Core usage

This example shows how to open a result file and do some basic postprocessing.

If you have Ansys 2021 R1 or higher installed, starting DPF is quite easy as DPF-Core takes care of launching all the services that are required for postprocessing Ansys files.

# First, import the DPF-Core module as ``dpf`` and import the included examples file.
from ansys.dpf import core as dpf
from ansys.dpf.core import examples

Next, open an example and print out the model object. The Model class helps to organize access methods for the result by keeping track of the operators and data sources used by the result file.

Printing the model displays:

• Analysis type

• Available results

• Size of the mesh

• Number of results

Also, note that the first time you create a DPF object, Python automatically attempts to start the server in the background. If you want to connect to an existing server (either local or remote), use ansys.dpf.core.connect_to_server().

model = dpf.Model(examples.find_simple_bar())
print(model)

DPF Model
------------------------------
Static analysis
Unit system: MKS: m, kg, N, s, V, A, degC
Physics Type: Mechanical
Available results:
     -  displacement: Nodal Displacement
     -  element_nodal_forces: ElementalNodal Element nodal Forces
     -  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
     -  element_euler_angles: ElementalNodal Element Euler Angles
     -  structural_temperature: ElementalNodal Structural temperature
------------------------------
DPF  Meshed Region:
  3751 nodes
  3000 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

Model metadata

Specific metadata can be extracted from the model by referencing the model’s metadata property. For example, to print only the result_info:

metadata = model.metadata
print(metadata.result_info)

Static analysis
Unit system: MKS: m, kg, N, s, V, A, degC
Physics Type: Mechanical
Available results:
     -  displacement: Nodal Displacement
     -  element_nodal_forces: ElementalNodal Element nodal Forces
     -  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
     -  element_euler_angles: ElementalNodal Element Euler Angles
     -  structural_temperature: ElementalNodal Structural temperature

Print the mesh region:

print(metadata.meshed_region)

DPF  Meshed Region:
  3751 nodes
  3000 elements
  Unit: m
  With solid (3D) elements

Print the time or frequency of the results:

print(metadata.time_freq_support)

DPF  Time/Freq Support:
  Number of sets: 1
Cumulative     Time (s)       LoadStep       Substep
1              1.000000       1              1

Extract displacement results

All results of the model can be accessed through the results property, which returns the ansys.dpf.core.results.Results class. This class contains the DPF result operators available to a specific result file, which are listed when printing the object with print(results).

Here, the 'U' operator is connected with data_sources, which takes place automatically when running results.displacement(). By default, the 'U' operator is connected to the first result set, which for this static result is the only result.

results = model.results
displacements = results.displacement()
fields = displacements.outputs.fields_container()

# Finally, extract the data of the displacement field:
disp = fields[0].data
disp

DPFArray([[-1.22753781e-08, -1.20861254e-06, -5.02681396e-06],
          [-9.46666013e-09, -1.19379712e-06, -4.64249826e-06],
          [-1.22188426e-08, -1.19494216e-06, -4.63117832e-06],
          ...,
          [-1.35911608e-08,  1.52559428e-06, -4.29246409e-06],
          [-1.91212290e-08,  1.52577102e-06, -4.28782940e-06],
          [-2.69632909e-08,  1.52485289e-06, -4.27831232e-06]])

model.metadata.meshed_region.plot(fields)