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

Vishnu

This code:

1. Extracts multiple fields (displacement and stress results) from an Ansys result file (.rst), and exports them to VTU format in a specified directory using DPF module

2. It then reads the VTU file using pyvista, extracts the surface mesh, and saves it as a VTP file.

These files can be used by SimAI

Vishnu

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

Harikrushna

Hello Vishnu,

Thank you for this script, Can you provide same script for extracting modal analysis results to see all frequency?

Harikrushna

@Vishnu said:
This code:

1. Extracts multiple fields (displacement and stress results) from an Ansys result file (.rst), and exports them to VTU format in a specified directory using DPF module

2. It then reads the VTU file using pyvista, extracts the surface mesh, and saves it as a VTP file.

These files can be used by SimAI

Hello Vishnu,

Thank you for this script, Can you provide same script for extracting modal analysis results to see all frequency?

Vishnu

@Harikrushna are you interested in creating a VTU/VTP for your modal analysis?
what information would you need , just the modal frequencies? Typically the frequencies can be embedded by creating a new field

look at the below for how you can extract natural freq using DPF:

https://discuss.ansys.com/discussion/1416/how-do-i-retrieve-natural-frequencies-from-a-modal-analysis-using-dpf-in-mechanical