Abaqus for Structural Analysis
Engineering-led guide to setting up and running structural analyses in Abaqus — model architecture, procedure selection, step control and result extraction.
Engineering Task
Setting up a structural analysis in Abaqus that produces credible, checkable results for stress, displacement or dynamic response.
Model Architecture
An Abaqus model consists of parts, assemblies, materials, sections, steps, loads and boundary conditions. Understanding the data hierarchy is essential for scripting and for reviewing models built by others.
- Parts define geometry; the Assembly positions them in global space
- Sections assign element properties (solid, shell, beam, connector) to regions
- Steps define the analysis sequence — each step has a procedure (static, frequency, etc.)
- Loads and boundary conditions are associated with steps and can vary between steps
- Field output writes results to the ODB at specified intervals; history output writes at every increment
Procedure Selection
| Procedure | Abaqus Keyword | When to Use |
|---|---|---|
| Static, General | *STATIC | Nonlinear statics — plasticity, contact, large displacement |
| Static, Linear Perturbation | *STATIC, PERTURBATION | Linear statics about a preloaded base state |
| Frequency | *FREQUENCY | Natural frequencies and mode shapes |
| Buckle | *BUCKLE | Linear eigenvalue buckling |
| Dynamic, Implicit | *DYNAMIC | Transient dynamics — low to mid frequency |
| Dynamic, Explicit | *DYNAMIC, EXPLICIT | Crash, impact, high-rate events |
| Coupled Temperature-Displacement | *COUPLED TEMPERATURE-DISPLACEMENT | Thermal stress |
Key Settings
- NLGEOM=ON activates geometric nonlinearity (large displacement) — required if deflections exceed t/2
- Automatic stabilisation controls prevent rigid-body instability in contact problems — but check artificial energy
- Incrementation: set initial, minimum and maximum increment sizes — too large causes divergence, too small wastes time
- Field output frequency: choose at specified time intervals or at every n increments — balance file size vs resolution
Result Extraction
- Reaction forces: RF at constrained nodes — check equilibrium in each direction
- Stress: S (stress tensor) — extract at specific elements or along paths
- Displacement: U — check deformed shape before stress
- Contact: CPRESS, CSHEAR, CSTATUS — verify contact status and pressure
- Strain: E, PE, PEEQ — elastic, plastic and equivalent plastic strain
Verification
- Check .msg and .dat files for warnings — these often indicate modelling errors
- Verify reaction forces balance applied loads to within 1%
- Check deformed shape is physically sensible before reading stress
- For nonlinear: review the load-displacement curve for smooth convergence
Common Mistakes
- Activating NLGEOM without checking whether large displacement is actually needed
- Using default incrementation without checking the convergence history
- Not checking artificial stabilisation energy — can dominate results
- Extracting peak nodal stress without checking for singularities