| 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:
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:
