DPF-Core has a variety of plotting methods for generating 3D plots of Ansys models directly from Python. These methods use VTK and leverage the PyVista library to simplify plotting. For more information, see the PyVista Documentation.

Plotting the Mesh from the Model Object

The Model.plot() method can be used to plot the mesh of the model immediately after loading it. In this example, a simple pontoon mesh is downloaded from the internet and loaded using the :class:ansys.dpf.core.model` class:

>>> import ansys.dpf.core as dpf
>>> from ansys.dpf.core import examples
>>> filename = examples.download_pontoon()
>>> model = dpf.Model(filename)
>>> model.plot()

The default plotter settings display the mesh with edges shown and lighting enabled. For a list of all keyword arguments, see plot.

Plotting Using the Meshed Region

The MeshedRegion.plot() method plots the meshed region. If the meshed region is generated from the model’s metadata, the plot generated is identical to the plot generated by Model.plot().

Plot the meshed region:

>>> mesh = model.metadata.meshed_region
>>> mesh.plot()

When a field is provided as the first argument, the mesh is plotted using these values. This example extracts the nodal strain in the X direction:

First, extract the X component strain

>>> strain = model.results.elastic_strain()
>>> fields = strain.outputs.fields_container()
>>> field = fields.select_component(0)[0]
>>> print(field)
DPF elastic_strain_1.s0 Field
  Location: ElementalNodal
  8640 entities
  Data:1 components and 69120 elementary data

This ElementalNodal strain must be converted to nodal strain for
it to be plotted.

>>> nodal_field = field.to_nodal()
>>> mesh.plot(nodal_field)


Only fields with Elemental and Nodal locations are supported currently. Use the to_nodal operator to convert to nodal or the ansys.dpf.core.operators.averaging.nodal_to_elemental class to convert to elemental.