StructuralFEA

Open source finite element analysis skill for structural validation of damper components and mechanical parts. Uses CalculiX, FreeCAD FEM, Gmsh, and ParaView.

Workflow Routing

Workflow Trigger Description

QuickStress "quick stress check", "hand calc" Analytical stress calculations before FEA

ComponentFEA "analyze rod", "tube stress", "piston FEA" Full FEA of specific component

BucklingAnalysis "buckling", "column", "stability" Euler and nonlinear buckling

ModalAnalysis "natural frequency", "modal", "vibration" Eigenvalue extraction

FatigueCheck "fatigue", "endurance", "life" Stress-life fatigue assessment

Toolchain Overview

┌─────────────────────────────────────────────────────────────────────┐ │ OPEN SOURCE FEA STACK │ ├─────────────────────────────────────────────────────────────────────┤ │ │ │ ┌─────────────┐ ┌─────────────┐ ┌─────────────┐ │ │ │ FreeCAD │────▶│ Gmsh │────▶│ CalculiX │ │ │ │ (CAD/GUI) │ │ (Meshing) │ │ (Solver) │ │ │ └─────────────┘ └─────────────┘ └──────┬──────┘ │ │ │ │ │ │ │ ┌─────────────┐ │ │ │ └─────────────▶│ ParaView │◀──────────┘ │ │ │ (Post-proc)│ │ │ └─────────────┘ │ │ │ │ Alternative paths: │ │ - FreeCAD FEM Workbench (integrated GUI workflow) │ │ - Salome-Meca (Code_Aster) for advanced nonlinear │ │ - OpenFOAM for CFD (valve flow analysis) │ │ │ └─────────────────────────────────────────────────────────────────────┘

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

Material E (MPa) ν ρ (kg/m³) Sy (MPa) Su (MPa)

6061-T6 68,900 0.33 2,700 276 310

7075-T6 71,700 0.33 2,810 503 572

4140 QT 205,000 0.29 7,850 655-860 810-970

4340 QT 205,000 0.29 7,850 860-1100 950-1200

17-4 PH H900 196,000 0.27 7,780 1,170 1,310

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

Component Global Size Refinement Areas Element Type

Rod (Ø16-25mm) 2-3mm Threads: 0.5mm, Fillet: 0.5mm C3D10 (tet)

Tube (Ø40-60mm) 3-4mm Thread root: 0.5mm C3D10 or C3D20R

Piston 2-3mm Valve ports: 0.3mm C3D10

Eye/Clevis 2-3mm Hole edge: 0.5mm C3D10

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

Create/Import Geometry

• Part Design workbench for new geometry

• Import STEP/IGES for existing CAD

Switch to FEM Workbench

• Analysis → New Analysis

• Model → Solver CalculiX Standard

Assign Material

• Model → Material for Solid

• Select from library or define custom

Apply Constraints

• Model → Constraint Fixed (for supports)

• Model → Constraint Force (for loads)

• Model → Constraint Pressure (for surfaces)

Create Mesh

• Mesh → FEM Mesh from Shape

• Set element size, refinement

Solve

• Solve → Solver Job Control

• Write .inp file, Run CalculiX

View Results

• Results → Show Result

• Filter: Von Mises, displacement, etc.

Result Interpretation

Stress Limits (Design Allowables)

Material Static σ_allow Fatigue σ_allow Note

6061-T6 165 MPa 60 MPa 0.6×Sy, Se=97 MPa

7075-T6 300 MPa 100 MPa 0.6×Sy, Se=159 MPa

4140 QT 400-520 MPa 200-260 MPa Depends on temper

4340 QT 520-660 MPa 260-330 MPa Premium fatigue

17-4 PH 700 MPa 350 MPa H900 condition

Safety Factor Guidelines

Application Static SF Fatigue SF Buckling SF

Road vehicle 2.0 3.0 3.0

Motorsport 1.5 2.0 2.5

Industrial 2.5 4.0 4.0

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

Skill Integration

DamperEngineering Component loads, material selection

PlantCapability Machining feasibility of designs

CuttingParams Surface finish requirements

QuoteEstimator Material costs, machining time

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