abaqus-coupled-analysis
GitHub用于Abaqus热-结构耦合分析的完整工作流，处理热应力、热膨胀变形等问题。通过判断耦合类型（单向/双向）和材料属性，指导用户选择全耦合或顺序耦合方法，定义边界条件与网格，实现温度与机械响应的交互分析。
Trigger Scenarios
Install
npx skills add Cai-aa/CAE-Agent-Hub --skill abaqus-coupled-analysis -g -y
SKILL.md
Frontmatter
{
"name": "abaqus-coupled-analysis",
"description": "Complete workflow for coupled thermomechanical analysis. Use when user mentions thermal stress, thermal expansion, or temperature causing deformation.",
"allowed-tools": [
"Read",
"Write",
"Edit",
"Glob",
"Grep",
"Bash(abaqus:*)",
"Skill"
]
}
Abaqus Coupled Thermomechanical Analysis Workflow
Analyze problems where temperature and mechanical response interact. Use for thermal stress, expansion-induced deformation, and high-temperature structural components.
When to Use This Skill
Natural language triggers:
- "Thermal stress analysis"
- "Thermomechanical coupling"
- "Temperature causes stress/deformation"
- "Thermal expansion effects"
- "Heat causes deformation"
- "Thermal shock"
- "High temperature component"
- "Thermal gradient stress"
Route elsewhere:
- Heat transfer only (no stress) ->
/abaqus-thermal-analysis - Structural only (no thermal) ->
/abaqus-static-analysis
Prerequisites
Before starting coupled analysis:
- Working thermal OR structural analysis that converges
- Material must have BOTH thermal and mechanical properties
- Understand whether coupling is one-way or two-way
Workflow: Coupled Thermomechanical Analysis
Step 1: Determine Coupling Type
Ask if unclear: "Does mechanical deformation affect the temperature field?"
| Scenario | Coupling Type | Approach |
|---|---|---|
| Heat causes stress, no feedback | One-way | Sequential coupling |
| Friction or plastic work generates heat | Two-way | Fully coupled |
| Large deformation changes heat path | Two-way | Fully coupled |
| Simple thermal expansion | One-way | Sequential is simpler |
Decision rule: If only temperature affects stress -> Sequential. If deformation affects temperature -> Fully coupled.
Step 2: Define Complete Material Properties
Material must include BOTH sets:
Mechanical: E (Young's modulus), nu (Poisson's ratio)
Thermal: k (conductivity), alpha (expansion coefficient), T_ref (reference temperature)
For transient: Also need cp (specific heat) and rho (density)
Typical steel values (SI-mm units):
- E = 210000 MPa, nu = 0.3
- k = 50 mW/(mm*K), alpha = 12e-6 /K
- cp = 5.0e11 mJ/(tonne*K), rho = 7.85e-9 tonne/mm^3
Step 3: Choose Analysis Type
Fully Coupled (simultaneous):
- Use
CoupledTempDisplacementStep - Response: STEADY_STATE or TRANSIENT
- Elements: C3D8T, C3D8RT, or C3D10MT (coupled elements)
Sequential (thermal first, then structural):
- Run thermal analysis with
HeatTransferStep - Import temperature results into structural model
- Run structural analysis with
StaticStep
Step 4: Set Initial Conditions
- Define initial temperature (should match T_ref for zero initial stress)
- Thermal strain = alpha * (T - T_ref)
Step 5: Apply Boundary Conditions
Thermal BCs: Temperature, heat flux, convection, or radiation
Mechanical BCs: Fixed supports (prevent rigid body motion)
Step 6: Mesh with Appropriate Elements
| Element | Description | Use |
|---|---|---|
| C3D8T | 8-node coupled brick | General coupled |
| C3D8RT | Reduced integration | Faster, watch hourglassing |
| C3D10MT | 10-node tet | Complex geometry |
For sequential: Use standard thermal elements (DC3D8) then structural elements (C3D8R).
Step 7: Request Coupled Output Variables
Key variables to request:
- S: Mechanical stress
- U: Displacement
- NT: Temperature (nodal)
- THE: Thermal strain
- E: Total strain
- EE: Elastic strain (mechanical only)
What to Ask User
If requirements unclear, ask:
- Is the coupling one-way (heat->stress) or two-way (mutual interaction)?
- Steady-state or transient thermal conditions?
- What is the reference temperature (zero thermal strain)?
- What temperatures will be applied?
- Are there any mechanical loads in addition to thermal effects?
Validation Checklist
After setup, verify:
- Expansion coefficient (alpha) defined with correct T_ref
- Initial temperature matches T_ref (for zero initial stress)
- Both mechanical and thermal BCs applied
- Using coupled elements (C3D*T) for fully coupled
- Thermal strain (THE) appears in output requests
Troubleshooting
| Problem | Likely Cause | Solution |
|---|---|---|
| Large/unrealistic thermal strain | Wrong alpha units | alpha should be ~1e-5/K for metals |
| Zero thermal stress | Missing Expansion property | Add material.Expansion() |
| Non-convergence | Large temperature change | Reduce time increments or deltmx |
| No thermal expansion effect | Wrong element type | Use coupled elements (C3D8T not C3D8) |
| Cannot import ODB | Path or step name wrong | Verify ODB exists and step name matches |
Related Skills
/abaqus-thermal-analysis- Thermal-only (heat transfer without stress)/abaqus-static-analysis- Structural-only (no thermal effects)/abaqus-field- Import temperature fields from external sources/abaqus-material- Material property definitions/abaqus-step- Analysis step configuration
Code Patterns
For API syntax and code examples, see:
Version History
- 2178ed3 Current 2026-07-24 17:38
