Load and inspect results in Mechanical

This example shows how to load result data and inspect its properties using the Ansys Mechanical scripting window.

Complete example for scripting window

Open View → Scripting in Mechanical and enter:

import mech_dpf
import Ans.DataProcessing as dpf

# CRITICAL: Set ExtAPI context
mech_dpf.setExtAPI(ExtAPI)

# Get the current Mechanical analysis
analysis = ExtAPI.DataModel.Project.Model.Analyses[0]

# Get result file path from Mechanical
result_file = analysis.ResultFileName

# Create DPF data sources
data_sources = dpf.DataSources()
data_sources.SetResultFilePath(result_file)

# Create DPF model
dpf_model = dpf.Model(data_sources)

# Inspect model properties
print("=== Model Information ===")
print("Result file: {0}".format(result_file))

# Mesh information
mesh = dpf_model.Mesh
print("\n=== Mesh Information ===")
print("Number of nodes: {0}".format(mesh.Nodes.Count))
print("Number of elements: {0}".format(mesh.Elements.Count))

# Time/frequency information
time_freq_support = dpf_model.TimeFreqSupport
print("\n=== Time Information ===")
print("Number of time steps: {0}".format(time_freq_support.TimeFrequencies.Count))

# List available time values
for i in range(time_freq_support.TimeFrequencies.Count):
    time_value = time_freq_support.TimeFrequencies.GetData(i)
    print("  Step {0}: {1} seconds".format(i+1, time_value))

print("\n=== Inspection Complete ===")

Expected output in scripting window

=== Model Information ===
Result file: C:\...\file0.rst

=== Mesh Information ===
Number of nodes: 15623
Number of elements: 3892

=== Time Information ===
Number of time steps: 10
  Step 1: 0.0 seconds
  Step 2: 0.1 seconds
  Step 3: 0.2 seconds
  ...

=== Inspection Complete ===

Using in a Python Result object

You can also inspect results within a Python Result object:

def define_dpf_workflow(analysis):
    import mech_dpf
    import Ans.DataProcessing as dpf

    # CRITICAL: Set ExtAPI context
    mech_dpf.setExtAPI(ExtAPI)

    # Access result file from analysis
    result_file = analysis.ResultFileName

    # Create DPF model
    data_sources = dpf.DataSources()
    data_sources.SetResultFilePath(result_file)
    dpf_model = dpf.Model(data_sources)

    # Get mesh info
    mesh = dpf_model.Mesh
    node_count = mesh.Nodes.Count
    element_count = mesh.Elements.Count

    # Get time steps
    time_count = dpf_model.TimeFreqSupport.TimeFrequencies.Count

    # Display in result text
    this.Text = "Mesh: {0} nodes, {1} elements\nTime steps: {2}".format(
    node_count, element_count, time_count)

Key concepts

• ExtAPI: Mechanical API for accessing the model tree
• DataSources: Points to result files from Mechanical solutions
• Model: DPF model provides access to all data
• Mesh: Contains geometry information
• TimeFreqSupport: Time/frequency metadata

Next steps

• Extract Displacement - Get displacement data
• User Guide - Learn about fields