StructuralFEA

Name: StructuralFEA
Author: robdtaylor

github.com/robdtaylor其他118 次安装

代码仓库

关于 StructuralFEA

StructuralFEA 是用于减振器部件和机械零件结构验证的开源技能，结合解析检查与有限元分析流程，使用 CalculiX、FreeCAD FEM 和 Gmsh 等工具。

主要功能

01快速解析应力检查
02部件有限元分析流程
03屈曲与模态分析
04疲劳评估
05材料数据与部件模板
06网格划分和结果解读指引

适用场景

01在完整分析前检查杆件应力
02分析内部受压的减振器管
03评估杆件受载时的屈曲
04估算部件疲劳寿命

安装

复制下面的命令，在终端中运行。

$npx skills add https://github.com/robdtaylor/personal-ai-infrastructure --skill structuralfea

安装后在 Claude Code 中输入/structuralfea确认已加载。

包含的文件

除 SKILL.md 外，安装时一起下载的参考资料和脚本。

CLAUDE.md

Workflows/

QuickStress.md

ComponentFEA.md

详细介绍

StructuralFEA

用于减振器组件和机械零件结构验证的开源有限元分析技能。使用 CalculiX、FreeCAD FEM、Gmsh 和 ParaView。

工作流路由

工作流	触发词	描述
QuickStress	“快速应力检查”、“手算”	FEA 前的解析应力计算
ComponentFEA	“分析杆件”、“管件应力”、“活塞 FEA”	对特定组件进行完整 FEA
BucklingAnalysis	“屈曲”、“柱”、“稳定性”	欧拉屈曲和非线性屈曲
ModalAnalysis	“固有频率”、“模态”、“振动”	特征值提取
FatigueCheck	“疲劳”、“耐久性”、“寿命”	应力-寿命疲劳评估

工具链概览

┌─────────────────────────────────────────────────────────────────────┐
│                    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)                         │
│                                                                     │
└─────────────────────────────────────────────────────────────────────┘

安装

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 替代方案（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

注意： CalculiX 是原生 Unix 软件。bConverged 安装程序是最简单的 Windows 选项。为获得最佳兼容性，可考虑在 WSL（适用于 Linux 的 Windows 子系统）中运行 CalculiX，其行为与原生 Linux 完全相同。

验证安装

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

材料数据库

铝合金（用于 CalculiX .inp 文件）

*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

钢材（用于 CalculiX .inp 文件）

*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

材料属性摘要

材料	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

组件模板

活塞杆——轴向载荷 + 弯曲载荷

** ================================================
** 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

管件——内部压力

** ================================================
** 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

屈曲分析模板

** ================================================
** 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

模态分析模板

** ================================================
** 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

网格划分指南

单元尺寸建议

组件	全局尺寸	细化区域	单元类型
杆件（Ø16-25mm）	2-3mm	螺纹：0.5mm，圆角：0.5mm	C3D10（四面体）
管件（Ø40-60mm）	3-4mm	螺纹根部：0.5mm	C3D10 或 C3D20R
活塞	2-3mm	阀孔：0.3mm	C3D10
吊耳/叉耳	2-3mm	孔边缘：0.5mm	C3D10

Gmsh 网格划分脚本

// ================================================
// 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 工作流

创建/导入几何体
- 使用 Part Design 工作台创建新几何体
- 为现有 CAD 导入 STEP/IGES
切换到 FEM 工作台
- Analysis → New Analysis
- Model → Solver CalculiX Standard
指定材料
- Model → Material for Solid
- 从库中选择或定义自定义材料
应用约束
- Model → Constraint Fixed（用于支撑）
- Model → Constraint Force（用于载荷）
- Model → Constraint Pressure（用于表面）
创建网格
- Mesh → FEM Mesh from Shape
- 设置单元尺寸和细化程度
求解
- Solve → Solver Job Control
- 写入 .inp 文件，运行 CalculiX
查看结果
- Results → Show Result
- 筛选：Von Mises、位移等

结果解读

应力限值（设计许用值）

材料	静态 σ_allow	疲劳 σ_allow	备注
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	取决于回火状态
4340 QT	520-660 MPa	260-330 MPa	优异的疲劳性能
17-4 PH	700 MPa	350 MPa	H900 状态

安全系数指南

应用	静态 SF	疲劳 SF	屈曲 SF
道路车辆	2.0	3.0	3.0
赛车运动	1.5	2.0	2.5
工业用途	2.5	4.0	4.0

结果检查清单

## 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

快速应力检查（FEA 前）

杆件轴向应力

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)

杆件屈曲

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 ✓

管材环向应力

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 ✓

与其他技能的集成

技能	集成内容
DamperEngineering	部件载荷、材料选择
PlantCapability	设计的加工可行性
CuttingParams	表面光洁度要求
QuoteEstimator	材料成本、加工时间

示例

示例 1：快速校核杆件

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

示例 2：完整 FEA 工作流

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

示例 3：屈曲分析

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

支持 Markdown

登录后评论

基本信息

作者: robdtaylor
仓库: robdtaylor/personal-ai-infrastructure
分类: 其他
安装次数: 118

报告问题