DPF Mechanical 2026 R1

Understanding DPF in Ansys Mechanical

Last update: 18.06.2026

Learn the fundamental concepts behind the Data Processing Framework as used in Ansys Mechanical.

What is DPF?

DPF (Data Processing Framework) is a modern infrastructure for accessing and processing simulation data in Ansys Mechanical. It provides:

  • Efficient data access: Optimized for large simulation datasets
  • Flexible processing: Chain operations using operators
  • Integrated with Mechanical: Available in scripting window and Python Results
  • IronPython interface: Python syntax using underlying C# DLLs

Key concepts

Model

The Model is the entry point to your simulation data in DPF. In Mechanical, you typically create it from the current solution's result file:

import Ans.DataProcessing as dpf

# Get result file from Mechanical solution
solution = ExtAPI.DataModel.Project.Model.Analyses[0].Solution
result_file = solution.ResultFileName

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

The Model provides access to:

  • Mesh information
  • Results data
  • Metadata (time steps, result types, etc.)

Fields

A Field is the fundamental data container in DPF. It contains:

  • Data: Numerical values (scalars, vectors, matrices)
  • Scoping: Which entities the data applies to
  • Support: Spatial/temporal context
# Get a field from results (in Mechanical scripting window)
displacement = dpf_model.Results.Displacement.GetOutput(0, dpf.LocationEnum.Nodal)

Operators

Operators are processing units that transform data. They follow a functional programming pattern:

  • Take inputs (fields, meshes, parameters)
  • Perform operations
  • Produce outputs (fields, meshes, etc.)
# Create an operator
norm_op = dpf.Operator("norm")
norm_op.SetInput(0, displacement)
norm_field = norm_op.GetOutput(0, dpf.Field)

Workflows

A Workflow chains multiple operators together for complex processing in Mechanical:

workflow = dpf.Workflow()
workflow.AddOperator(op1)
workflow.AddOperator(op2)
workflow.Connect(op1, 0, op2, 0)
result = workflow.GetOutput(0, dpf.Field)

DPF in Mechanical Architecture

┌─────────────────────┐
│ Ansys Mechanical UI │
│ (User Interface)    │
└──────────┬──────────┘
           │
           ▼
┌─────────────────────┐
│  Python Scripting   │
│  IronPython (.NET)  │
└──────────┬──────────┘
           │
           ▼
┌─────────────────────┐
│   DPF C# DLLs      │
│ (CS_DataProcessing) │
└──────────┬──────────┘
           │
           ▼
┌─────────────────────┐
│   DPF Core Engine   │
│  Data Processing    │
└──────────┬──────────┘
           │
           ▼
┌─────────────────────┐
│  Result Files (.rst)│
│  Solver Output      │
└─────────────────────┘

Data Flow in Mechanical

  1. Solve: Run analysis in Mechanical to generate result file (.rst)
  2. Access: Use DPF to connect to the result file
  3. Query: Request specific results (stress, displacement, etc.)
  4. Process: Use operators to transform data
  5. Display: Show results in Python Result object or extract values

Typical Mechanical Workflow

import Ans.DataProcessing as dpf

# 1. Access Mechanical model
model = ExtAPI.DataModel.Project.Model
solution = model.Analyses[0].Solution

# 2. Create DPF model from result file
data_sources = dpf.DataSources()
data_sources.SetResultFilePath(solution.ResultFileName)
dpf_model = dpf.Model(data_sources)

# 3. Extract result field
stress = dpf_model.Results.Stress.GetOutput(0, dpf.LocationEnum.Elemental)

# 4. Process with operator (von Mises equivalent)
vm_op = dpf.Operator("eqv")
vm_op.SetInput(0, stress)
vm_stress = vm_op.GetOutput(0, dpf.Field)

# 5. Get values
max_stress = max(vm_stress.Data)
print("Max von Mises: {0:.2f}".format(max_stress))

To go further (DPF framework)

Next Steps

Connect with Ansys