How to convert Ansys mechanical result file (.RST) to VTU/VTP format (typically used in paraview)

from ansys.dpf import core as dpf
import pyvista as pv
import os
 
# Inputs
rstpath = r"your path\file.rst"
vtu_directory = r"D:/"
vtu_file_name = "MyFile" # your file name
 
# Initialize data source and model
my_data_sources = dpf.DataSources(rstpath)
my_model = dpf.Model(rstpath)
 
# Get all available result names
available_results = my_model.metadata.result_info.available_results
result_names = [r.name for r in available_results if hasattr(dpf.operators.result, r.name)]
#result_names = ["displacement_Y","stress_X","stress_Y"] #Either specify this or specify all results by commenting this line
 
# Get mesh and time frequencies
my_mesh = my_model.metadata.meshed_region
my_time_scoping = (
    dpf.operators.metadata.time_freq_provider(data_sources=my_data_sources)
    .outputs.time_freq_support.get_data()
    .time_frequencies.data_as_list
)
 
# Define scoping (all nodes)
my_scoping = dpf.Scoping()
my_scoping.location = dpf.locations.nodal
my_scoping.ids = my_mesh.nodes.scoping.ids
 
# Extract result fields
result_fields = []
for result_name in result_names:
    result_operator = dpf.operators.result.__getattribute__(result_name)
    result_field = result_operator(
        time_scoping=my_time_scoping, data_sources=my_data_sources, mesh=my_mesh, mesh_scoping=my_scoping
    ).outputs.fields_container.get_data()[0]
    result_fields.append(result_field)
 
# Generate VTU file
vtu_operator = dpf.operators.serialization.vtu_export(
    directory=vtu_directory, mesh=my_mesh, base_name=vtu_file_name
)
for count, result_field in enumerate(result_fields):
    vtu_operator.connect(count + 3, result_field)
 
vtu_operator.run()
 
# Generate VTP file from VTU
vtu_file_path = os.path.join(vtu_directory, vtu_file_name + "_T0000000-1.vtu")
vtp_file_path = os.path.join(vtu_directory, vtu_file_name + "_surface.vtp")
vtu = pv.read(vtu_file_path)
vtp = vtu.extract_surface()
vtp.save(vtp_file_path)
 

See below:
all results available in .RST is transferred in VTU and VTP

In case you have your own custom result file , you can create your own fields using them before writing a VTU/VTP file . Please refer below link to see how you can create your own custom field:
https://dpf.docs.pyansys.com/version/stable/examples/00-basic/03-create_entities.html#sphx-glr-examples-00-basic-03-create-entities-py

Also if you want to just have solid elements and their results you can filter them out like below:
(This could be very useful for SimAI workflows, which allows only solid elements on VTU, ignoring CONTACT, SURF like elements and corresponding fields )

# Filter to include only solid elements (using 'solid' as the shape type)
solid_element_ids = [
    elem.id for elem in my_mesh.elements#assuming you already have my_mesh from previously executed codes
    if elem.shape == "solid"
]
 
# Define scoping for element ids of solid elements
my_scoping = dpf.Scoping()
my_scoping.location = dpf.locations.elemental
my_scoping.ids = solid_element_ids
 
#Creating mesh from solid element scopings
my_mesh = dpf.operators.mesh.from_scoping(scoping=my_scoping,mesh=my_mesh).outputs.mesh.get_data()
 
# Creating nodal scoping (all nodes of the solid elements only)
my_scoping = dpf.Scoping()
my_scoping.location = dpf.locations.nodal
my_scoping.ids = my_mesh.nodes.scoping.ids