Applying Boundary Conditions in Abaqus
How to apply physically realistic boundary conditions in Abaqus — encastre, symmetry, coupling constraints, RBE3 and avoiding over-constraint.
Engineering Task
Applying constraints in Abaqus that represent the physical restraints of the real structure without over-constraining or under-constraining the model.
Constraint Types
| Type | Abaqus Keyword | When to Use |
|---|---|---|
| Encastre (fixed) | *BOUNDARY, TYPE=DISPLACEMENT | Truly clamped surface — rarely correct |
| Symmetry | *BOUNDARY (specific DOF) | Geometry and load symmetric about a plane |
| Coupling (distributing) | *COUPLING, DISTRIBUTING | Distribute load from RP to surface — flexible |
| Coupling (kinematic) | *COUPLING, KINEMATIC | Rigid link from RP to surface — stiff |
| Shell-to-solid | *SHELL TO SOLID COUPLING | Connect shell edge to solid face |
| Equation | *EQUATION | Custom MPC between nodes |
Key Settings
- Use distributing coupling (RBE3 equivalent) to distribute loads without over-stiffening — kinematic coupling (RBE2 equivalent) makes the surface rigid
- For symmetry: fix only the DOF normal to the plane and the two rotations about in-plane axes (e.g. U2, RX, RZ for XZ symmetry)
- Use reference points with coupling constraints to apply resultant loads cleanly
- For bolted joints: do not use encastre on the hole surface — use bolt preload with contact
Verification
- Check reaction forces at constrained nodes — must balance applied loads
- Check deformed shape near constraints — no artificial stress concentration at the boundary
- For symmetry: verify every load case is symmetric, not just the first
Common Mistakes
- Using encastre on a bolted surface — over-constrains the model
- Using kinematic coupling where distributing coupling is appropriate — over-stiffens locally
- Applying symmetry to a non-symmetric load case
- Not constraining enough DOF — rigid-body modes in static analysis