Structuralfea

Installation

macOS (Homebrew)

# FreeCAD with FEM workbench
brew install --cask freecad

# Gmsh mesher
brew install gmsh

# CalculiX solver (requires tap)
brew tap costerwi/calculix
brew install calculix-ccx     # Solver
brew install calculix-cgx     # Pre/post (optional, requires XQuartz on macOS)

# ParaView post-processor
brew install --cask paraview

# Optional: OpenFOAM for CFD
brew install openfoam

macOS Alternative (Conda)

# If you prefer conda
conda install conda-forge::calculix
conda install conda-forge::gmsh

Linux (Ubuntu/Debian)

# FreeCAD
sudo apt install freecad

# Gmsh
sudo apt install gmsh

# CalculiX
sudo apt install calculix-ccx calculix-cgx

# ParaView
sudo apt install paraview

# Salome-Meca (alternative, more powerful)
# Download from https://www.code-aster.org/

Windows

# FreeCAD - via winget or download from freecad.org
winget install FreeCAD.FreeCAD

# Gmsh - via winget or download from gmsh.info
winget install -e --id Gmsh.Gmsh

# CalculiX - multiple options:

# Option 1: bConverged installer (recommended, includes GUI)
# Download from http://www.bconverged.com/calculix.php
# Provides ccx.exe and optional cgx.exe

# Option 2: Chocolatey (if installed)
choco install calculix

# Option 3: WSL (most reliable, identical to Linux)
# Install WSL, then: sudo apt install calculix-ccx calculix-cgx

# ParaView - via winget or download from paraview.org
winget install Kitware.ParaView

Note: CalculiX is Unix-native software. The bConverged installer is the easiest Windows option. For maximum compatibility, consider running CalculiX in WSL (Windows Subsystem for Linux) which provides identical behaviour to native Linux.

Verify Installation

# Check versions
freecad --version
gmsh --version
ccx -v
paraview --version

Material Database

Aluminium Alloys (for CalculiX .inp files)

*MATERIAL, NAME=AL6061T6
*ELASTIC
68900, 0.33
*DENSITY
2700E-12
*EXPANSION
23.6E-6

*MATERIAL, NAME=AL7075T6
*ELASTIC
71700, 0.33
*DENSITY
2810E-12
*EXPANSION
23.4E-6

*MATERIAL, NAME=AL2024T351
*ELASTIC
72400, 0.33
*DENSITY
2780E-12
*EXPANSION
23.2E-6

Steels (for CalculiX .inp files)

*MATERIAL, NAME=STEEL4140
*ELASTIC
205000, 0.29
*DENSITY
7850E-12
*EXPANSION
12.3E-6
*PLASTIC
655, 0.0
860, 0.10

*MATERIAL, NAME=STEEL4340
*ELASTIC
205000, 0.29
*DENSITY
7850E-12
*EXPANSION
11.7E-6
*PLASTIC
860, 0.0
1100, 0.08

*MATERIAL, NAME=STEEL174PH
*ELASTIC
196000, 0.27
*DENSITY
7780E-12
*EXPANSION
10.8E-6
*PLASTIC
1170, 0.0
1310, 0.06

Material Properties Summary

Component Templates

Piston Rod - Axial + Bending Load

** ================================================
** PISTON ROD FEA - COMBINED LOADING
** ================================================
**
*HEADING
Damper Piston Rod - Axial Load with Side Force
**
*NODE, NSET=ALLNODES
** Node data imported from mesh file
*INCLUDE, INPUT=rod_mesh.inp
**
** ------------------------------------------------
** MATERIAL DEFINITION
** ------------------------------------------------
*MATERIAL, NAME=STEEL4140
*ELASTIC
205000, 0.29
*DENSITY
7850E-12
**
*SOLID SECTION, ELSET=EALL, MATERIAL=STEEL4140
**
** ------------------------------------------------
** BOUNDARY CONDITIONS
** ------------------------------------------------
** Fixed end (piston attachment)
*BOUNDARY
FIXED_END, 1, 3, 0.0
**
** ------------------------------------------------
** LOADING
** ------------------------------------------------
** Axial load (compression)
*CLOAD
LOAD_NODE, 3, -5000.0
**
** Side load (bending from misalignment)
*CLOAD
LOAD_NODE, 1, 500.0
**
** ------------------------------------------------
** ANALYSIS
** ------------------------------------------------
*STEP
*STATIC
**
*NODE FILE
U
*EL FILE
S, E
**
*END STEP

Tube - Internal Pressure

** ================================================
** DAMPER TUBE - INTERNAL PRESSURE
** ================================================
**
*HEADING
Damper Tube Hoop Stress Analysis
**
*INCLUDE, INPUT=tube_mesh.inp
**
*MATERIAL, NAME=AL6061T6
*ELASTIC
68900, 0.33
**
*SOLID SECTION, ELSET=EALL, MATERIAL=AL6061T6
**
** Fixed end cap
*BOUNDARY
END_FIXED, 1, 3, 0.0
**
** Internal pressure (20 MPa = 200 bar)
*DLOAD
INNER_SURFACE, P, 20.0
**
*STEP
*STATIC
*NODE FILE
U
*EL FILE
S, E
*END STEP

Buckling Analysis Template

** ================================================
** ROD BUCKLING ANALYSIS
** ================================================
**
*HEADING
Piston Rod Linear Buckling
**
*INCLUDE, INPUT=rod_mesh.inp
**
*MATERIAL, NAME=STEEL4340
*ELASTIC
205000, 0.29
**
*SOLID SECTION, ELSET=EALL, MATERIAL=STEEL4340
**
** Pinned bottom
*BOUNDARY
BOTTOM, 1, 2, 0.0
BOTTOM, 3, 3, 0.0
**
** Guided top (can move axially)
*BOUNDARY
TOP, 1, 2, 0.0
**
** Unit load for eigenvalue extraction
*CLOAD
TOP, 3, -1.0
**
** ------------------------------------------------
** LINEAR BUCKLING (EIGENVALUE)
** ------------------------------------------------
*STEP
*BUCKLE
5
**
*NODE FILE
U
*EL FILE
S
**
*END STEP

Modal Analysis Template

** ================================================
** COMPONENT MODAL ANALYSIS
** ================================================
**
*HEADING
Natural Frequency Extraction
**
*INCLUDE, INPUT=component_mesh.inp
**
*MATERIAL, NAME=STEEL4140
*ELASTIC
205000, 0.29
*DENSITY
7850E-12
**
*SOLID SECTION, ELSET=EALL, MATERIAL=STEEL4140
**
*BOUNDARY
FIXED, 1, 3, 0.0
**
*STEP
*FREQUENCY
10
**
*NODE FILE
U
*EL FILE
S
**
*END STEP

Meshing Guidelines

Element Size Recommendations

Gmsh Meshing Script

// ================================================
// GMSH SCRIPT FOR DAMPER ROD
// ================================================

// Load geometry (STEP file from CAD)
Merge "piston_rod.step";

// Define mesh size
Mesh.CharacteristicLengthMax = 2.0;  // mm
Mesh.CharacteristicLengthMin = 0.3;  // mm

// Refine at threads (identify surfaces by number)
Field[1] = Distance;
Field[1].FacesList = {5, 6};  // Thread surfaces
Field[1].NNodesByEdge = 100;

Field[2] = Threshold;
Field[2].IField = 1;
Field[2].LcMin = 0.5;
Field[2].LcMax = 2.0;
Field[2].DistMin = 0.5;
Field[2].DistMax = 5.0;

Background Field = 2;

// Generate 3D mesh
Mesh.Algorithm3D = 1;  // Delaunay
Mesh 3;

// Save for CalculiX
Save "rod_mesh.inp";

FreeCAD FEM Workflow

1. Create/Import Geometry

   • Part Design workbench for new geometry
   • Import STEP/IGES for existing CAD

2. Switch to FEM Workbench

   • Analysis → New Analysis
   • Model → Solver CalculiX Standard

3. Assign Material

   • Model → Material for Solid
   • Select from library or define custom

4. Apply Constraints

   • Model → Constraint Fixed (for supports)
   • Model → Constraint Force (for loads)
   • Model → Constraint Pressure (for surfaces)

5. Create Mesh

   • Mesh → FEM Mesh from Shape
   • Set element size, refinement

6. Solve

   • Solve → Solver Job Control
   • Write .inp file, Run CalculiX

7. View Results

   • Results → Show Result
   • Filter: Von Mises, displacement, etc.

Result Interpretation

Stress Limits (Design Allowables)

Safety Factor Guidelines

Result Checklist

## FEA Result Verification

□ Mesh convergence check (refine 2x, stress change <5%)
□ Displacement magnitude reasonable
□ Stress concentrations identified and acceptable
□ von Mises < σ_allowable everywhere
□ No yielding in critical regions
□ Buckling factor > required SF
□ Natural frequencies away from excitation frequencies
□ Reaction forces balance applied loads
□ No mesh distortion warnings

Quick Stress Checks (Before FEA)

Rod Axial Stress

σ = F / A = F / (π × d²/4)

Example:
F = 5000 N, d = 20 mm
σ = 5000 / (π × 20²/4) = 15.9 MPa

For 4140 steel (Sy = 700 MPa):
SF = 700 / 15.9 = 44 ✓ (very conservative)

Rod Buckling

Pcr = π² × E × I / (K × L)²

I = π × d⁴ / 64

Example:
d = 20 mm, L = 200 mm, K = 0.7 (guided)
E = 205,000 MPa

I = π × 20⁴ / 64 = 7854 mm⁴
Pcr = π² × 205000 × 7854 / (0.7 × 200)²
Pcr = 809,000 N = 809 kN

For F = 5000 N:
SF = 809,000 / 5000 = 162 ✓

Tube Hoop Stress

σ_hoop = P × r / t

Example:
P = 20 MPa, r = 20 mm (inner), t = 3 mm
σ_hoop = 20 × 20 / 3 = 133 MPa

For 6061-T6 (Sy = 276 MPa):
SF = 276 / 133 = 2.1 ✓

Integration with Other Skills

Examples

Example 1: Quick rod check

User: "Check if 16mm rod can handle 4000N"
→ Run analytical calculation
→ Check axial stress vs allowable
→ Check buckling if stroke > 100mm
→ Report pass/fail with SF

Example 2: Full FEA workflow

User: "Run FEA on piston rod with thread detail"
→ Generate CalculiX template
→ Provide meshing guidance
→ Define boundary conditions
→ Interpret results
→ Recommend design changes if needed

Example 3: Buckling analysis

User: "Will this long rod buckle under max load?"
→ Euler calculation first
→ Set up CalculiX buckling analysis
→ Extract eigenvalue (buckling factor)
→ Report margin