Warp the mesh by a field for plotting

This example shows how to warp the mesh by a vector field, enabling to plot on the deformed geometry.

Static Scene

Interactive Scene

Static Scene

Interactive Scene

Static Scene

Interactive Scene

Static Scene

Interactive Scene

Static Scene

Interactive Scene

Static Scene

Interactive Scene

DPF Model
------------------------------
Static analysis
Unit system: MKS: m, kg, N, s, V, A, degC
Physics Type: Mechanical
Available results:
     -  node_orientations: Nodal Node Euler Angles
     -  displacement: Nodal Displacement
     -  nodal_rotation: Nodal Rotation
     -  reaction_force: Nodal Reaction Force
     -  reaction_moment: Nodal Reaction Moment
     -  stress: ElementalNodal Stress
     -  elemental_volume: Elemental Volume
     -  stiffness_matrix_energy: Elemental Energy-stiffness matrix
     -  artificial_hourglass_energy: Elemental Hourglass Energy
     -  kinetic_energy: Elemental Kinetic Energy
     -  co_energy: Elemental co-energy
     -  incremental_energy: Elemental incremental energy
     -  thermal_dissipation_energy: Elemental thermal dissipation energy
     -  elastic_strain: ElementalNodal Strain
     -  elastic_strain_eqv: ElementalNodal Strain eqv
     -  element_orientations: ElementalNodal Element Euler Angles
     -  structural_temperature: ElementalNodal Structural temperature
     -  contact_status: ElementalNodal Contact Status
     -  contact_penetration: ElementalNodal Contact Penetration
     -  contact_pressure: ElementalNodal Contact Pressure
     -  contact_friction_stress: ElementalNodal Contact Friction Stress
     -  contact_total_stress: ElementalNodal Contact Total Stress
     -  contact_sliding_distance: ElementalNodal Contact Sliding Distance
     -  contact_gap_distance: ElementalNodal Contact Gap Distance
     -  contact_surface_heat_flux: ElementalNodal Total heat flux at contact surface
     -  num_surface_status_changes: ElementalNodal Contact status changes
     -  contact_fluid_penetration_pressure: ElementalNodal Fluid Penetration Pressure
------------------------------
DPF  Meshed Region:
  7079 nodes
  4220 elements
  Unit: m
  With solid (3D) elements, shell (2D) elements, shell (3D) elements
------------------------------
DPF  Time/Freq Support:
  Number of sets: 1
Cumulative     Time (s)       LoadStep       Substep
1              1.000000       1              1


([], <pyvista.plotting.plotter.Plotter object at 0x0000020703BBEE50>)

from ansys.dpf import core as dpf
from ansys.dpf.core import examples

# Get and show the initial model
model = dpf.Model(examples.find_multishells_rst())
print(model)
model.plot(title="Model", text="Model.plot()")

# Define a scaling factor and a step for the field to be used for warping.
scale_factor = 0.001
step = 1

# Define a result to deform by
disp_result = model.results.displacement.on_time_scoping([step])
disp_op = disp_result()
# Get the displacement field
disp_fc = disp_result.eval()
disp_field = disp_fc[0]

# Get the mesh and plot it as a deformed geometry using a Result, an Operator,
# a Field or a FieldsContainer
mesh = model.metadata.meshed_region
mesh.plot(
    deform_by=disp_result,
    scale_factor=scale_factor,
    title="MeshedRegion",
    text="MeshedRegion.plot()",
)
# mesh.plot(deform_by=disp_op, scale_factor=scale_factor,
#           title='MeshedRegion', text='MeshedRegion.plot()')
# mesh.plot(deform_by=disp_fc, scale_factor=scale_factor,
#           title='MeshedRegion', text='MeshedRegion.plot()')
# mesh.plot(deform_by=disp_field, scale_factor=scale_factor,
#           title='MeshedRegion', text='MeshedRegion.plot()')

# Plot the displacement field on the deformed geometry directly
disp_field.plot(
    deform_by=disp_result, scale_factor=scale_factor, title="Field", text="Field.plot()"
)
# or by applying it to the mesh
mesh.plot(
    disp_field,
    deform_by=disp_result,
    scale_factor=scale_factor,
    title="MeshedRegion",
    text="MeshedRegion.plot(disp_field)",
)

# Split the model by material and plot the deformed MeshesContainer obtained
split_mesh_op = dpf.operators.mesh.split_mesh(mesh=mesh, property="mat")
meshes_cont = split_mesh_op.get_output(0, dpf.types.meshes_container)
meshes_cont.plot(
    deform_by=disp_result,
    scale_factor=scale_factor,
    title="MeshesContainer",
    text="MeshesContainer.plot()",
)

# Create a corresponding FieldsContainer and plot it on the deformed MeshesContainer
disp_op = dpf.operators.result.displacement(
    data_sources=model.metadata.data_sources, mesh=meshes_cont
)
disp_fc = disp_op.outputs.fields_container()
meshes_cont.plot(
    disp_fc,
    deform_by=disp_result,
    scale_factor=scale_factor,
    title="MeshesContainer",
    text="MeshesContainer.plot(disp_fc)",
)