fea-composites

name	fea-composites
description	FEA for composite structures — laminate FEA, shell element formulations, progressive failure analysis, cohesive zone models (CZM), virtual crack closure (VCCT), interlaminar stresses, damage modeling.
metadata	{"priority":7,"promptSignals":{"phrases":["composite FEA","laminate FEA","progressive failure","cohesive zone","CZM","VCCT","delamination","interlaminar","composite damage","FEA composite"],"minScore":3}}

FEA for Composite Structures — Complete Skill

Laminate FEA Fundamentals

Shell Elements for Laminates

Most common: shell elements with classical laminate theory (CLT) integration through thickness

ANSYS: SHELL181 / SHELL281 SHELL181: 4-node; 6 DOF/node; Mindlin-Reissner (first-order shear); default for composites SHELL281: 8-node; higher accuracy for curved shells and thick laminates Layer definition: specify stacking sequence, ply angles, thickness per layer

Abaqus: S4 / S4R / S8R S4R: 4-node reduced integration (1 integration point); fast; single hourglass mode S8R: 8-node quadratic; better accuracy for curved geometry

Integration methods: Full integration through thickness: N_layers × 2 Gauss points (accurate, expensive) Composite layup: CLT used analytically — stresses at top/middle/bottom of each ply

Setting Up Composite Layup

1. Define material properties for each ply (E₁, E₂, G₁₂, ν₁₂ for UD; or woven properties)
2. Create composite section: ply angles and thicknesses in stacking sequence
3. Assign material orientation (fiber reference direction on surface)
4. Request output: ply-level stresses (σ₁, σ₂, τ₁₂ in ply coordinate system)

Local vs. global stress: σ_global: in global XYZ (for structural equilibrium) σ_local (ply): in ply 1-2-3 system (for failure criteria) Transform using ply angle rotation: σ_ply = T(θ) × σ_global

Interlaminar Stresses

Why Interlaminar Stresses Matter

At laminate free edges: interlaminar normal (σ_z) and shear (τ_xz, τ_yz) stresses are significant These stresses are NOT captured by CLT (which assumes plane stress) Can cause delamination initiation at free edges (especially tensile σ_z)

Boundary layer effect: stress concentration within ~1 ply thickness from free edge Increases with: large mismatch in θ between adjacent plies (0°/90° worst)

3D Solid Elements for Interlaminar

Use when: delamination is expected; edges are critical Solid elements: SOLID185 (8-node) or SOLID186 (20-node) in ANSYS At least 1 element (preferably 3+) through each ply thickness Element size: Δz ≈ t_ply; ΔX/ΔY ≈ 0.2-0.5 × t_ply in edge zone

Continuum shell elements (Abaqus SC8R, ANSYS SOLSH190): 3D geometry, shell formulation; good for interlaminar AND bending Stack one element per ply or per group of plies

Progressive Failure Analysis (PFA)

Approach

1. Run linear elastic FEA → compute ply stresses σ₁, σ₂, τ₁₂
2. Apply failure criterion → check each ply at each element
3. Degrade failed ply material properties (stiffness reduction)
4. Rerun with degraded properties → redistribution
5. Repeat until global failure (no more load carrying)

Failure Criteria

Maximum stress: Fail if σ₁ > X_T (or X_C), σ₂ > Y_T, τ₁₂ > S₁₂ Simple; no interaction; overconservative for combined loads

Tsai-Wu (interactive): F₁₁ σ₁² + F₂₂ σ₂² + F₆₆ τ₁₂² + F₁ σ₁ + F₂ σ₂ + 2F₁₂ σ₁ σ₂ = 1 F₁₁ = 1/(X_T X_C), F₂₂ = 1/(Y_T Y_C), F₆₆ = 1/S₁₂² F₁ = 1/X_T - 1/X_C, F₂ = 1/Y_T - 1/Y_C F₁₂ ≈ -1/2 √(F₁₁ F₂₂) (biaxial factor, often assumed)

Hashin (mode-specific): Fiber tension (σ₁ > 0): (σ₁/X_T)² + (τ₁₂/S₁₂)² ≥ 1 Fiber compression (σ₁ < 0): (σ₁/X_C)² ≥ 1 or (σ₁/2S₁₂)² + ((Y_C/2S₁₂)²-1)(σ₂/Y_C) + (τ₁₂/S₁₂)² ≥ 1 Matrix tension (σ₂ > 0): (σ₂/Y_T)² + (τ₁₂/S₁₂)² ≥ 1 Matrix compression (σ₂ < 0): similar with Y_C

PUCK (most accurate): Separates fiber failure from inter-fiber failure (IFF) with mode-specific equations Implemented in: Abaqus VUMAT, Ansys ACP (Composite PrepPost)

Property Degradation Methods

Total discount: E₁ → 0, E₂ → 0 (sudden, conservative) Partial discount: reduce E₂ to 0 only (matrix failure, fibers intact) or E₁ to 0 (fiber failure) Exponential: gradual degradation vs. damage variable

Implementation in ANSYS Mechanical: Use Mechanical APDL or Ansys Composite PrepPost (ACP) post-processor MPDELE command or USERFAIL subroutine for custom criteria

Delamination Modeling

Cohesive Zone Model (CZM)

Traction-Separation Law (bilinear): T_n = K_n × δ_n (Mode I: opening) T_s = K_s × δ_s (Mode II: sliding)

Damage initiation: Quads criterion: (T_n / N)² + (T_s / S)² = 1 (mixed-mode) N = Mode I strength [MPa], S = Mode II strength [MPa]

Damage evolution (mixed-mode, Benzeggagh-Kenane): G_C = G_IC + (G_IIC - G_IC)(G_II/(G_I+G_II))^η G_IC, G_IIC = critical strain energy release rates [J/m²] η = BK exponent (typically 1.0-2.5 for CFRP)

CZM elements: Abaqus: COH3D8 (3D cohesive solid), COHAX4 (axisymmetric) ANSYS: INTER205 (3D interface), CONTA174+TARGE170 with CZM behavior Zero-thickness elements inserted at delamination plane

Mesh requirements for CZM: Element size ≤ l_pz/3-5 (l_pz = cohesive process zone length) l_pz = E × G_IC / σ_max² (for Mode I) Typical l_pz = 1-5 mm for CFRP → element size 0.2-1 mm at crack front

Virtual Crack Closure Technique (VCCT)

Strain energy release rate from nodal forces: G_I = F_y × v / (2 Δa × b) G_II = F_x × u / (2 Δa × b) F = nodal force at crack tip, v/u = displacements behind crack tip Δa = crack extension length, b = width

Mixed-mode criterion: G_I/G_IC + G_II/G_IIC = 1 (linear) OR (G_I/G_IC)^m + (G_II/G_IIC)^n = 1 (power law)

Advantages of VCCT: No special elements (uses standard FEA) No softening law needed Computationally efficient

Disadvantages: requires pre-existing crack; does not capture initiation (CZM does)

Abaqus: VCCT implemented via LEFM fracture criterion in contact property or fracture domain

Typical Composite FEA Workflow

Ansys ACP (Composite PrepPost)

1. PrePost/ACP Pre: Import geometry → define plies (material, angle, thickness, draping)
2. Mechanical: Apply loads/BCs → solve → export ply stresses
3. ACP Post: Apply failure criteria → failure reserve factors (FRF = 1/failure index)
4. Review: FRF < 1 = failed; locate first failure (lowest FRF); identify failure mode (fiber/matrix)

Abaqus Composite Analysis

1. Define composite layup in Part module (Composite Layup or individual ply assignments)
2. SHELL section → assign layup
3. Submit → CFRP output: TSAIW (Tsai-Wu), HSNFTCRT (Hashin fiber tension), etc.
4. Delamination: add cohesive layer at interfaces; define mixed-mode CZM law

Output

Provide: ply-level stresses in principal coordinates [σ₁, σ₂, τ₁₂] at critical locations, failure index per ply (and which mode: fiber/matrix/interlaminar), first ply failure load [kN or MPa], delamination G_I/G_IIC vs. G_IC/G_IIC criterion, progressive failure load vs. first-ply-failure ratio, mesh size recommendations for CZM [mm].