fea-mesh

name	fea-mesh
description	FEA meshing strategy — mesh quality metrics (aspect ratio, skewness, Jacobian), mesh density rules, singularities, contact meshing, submodeling, adaptive refinement.
metadata	{"priority":7,"promptSignals":{"phrases":["mesh","meshing","mesh quality","element size","mesh density","mesh convergence","aspect ratio","skewness"],"minScore":4}}

FEA Meshing Strategy — Complete Skill

Mesh Quality Metrics

Aspect Ratio

AR = longest edge / shortest edge (element) Target: AR < 5 (ideal), AR < 10 (acceptable), AR > 20 (poor — avoid) High-AR elements distort stress in transverse direction Acceptable exception: 1D beams, thin shells along fiber direction

Skewness (Angular Deviation from Ideal)

For triangles: skewness = (θ_max - 60°)/120° or (60° - θ_min)/60° — take max For quads: deviation from 90° angles Target: < 0.5 (good), < 0.85 (acceptable), > 0.9 (unacceptable)

Jacobian (Determinant)

J > 0 everywhere in element → valid element J < 0 → inverted element → SOLVE FAILS For higher-order elements: check at all Gauss points Target: Jacobian ratio (max/min) < 10

Warping (Quads)

Deviation from planarity of quad element ANSYS WF: < 1° (excellent), < 5° (acceptable), > 30° (fails) Highly warped quads: split into triangles

Orthogonal Quality (Fluent/CFD)

0 = worst, 1 = perfect (reversed from skewness) Target for CFD: > 0.15 (minimum), > 0.5 (good)

Mesh Density Rules

Stress Analysis

• Baseline: 4–6 elements across any cross-section dimension
• Stress concentration: 6–10 elements across fillet radius (r)
• Fillet mesh: element size ≤ r/4 at notch tip
• Bending: minimum 4 elements through thickness (for solid elements)
• Pressure vessel: 3+ elements through wall thickness t (HEX recommended)

Fatigue-Critical Locations

• 8–12 elements across stress concentration radius
• Local mesh refinement around weld toes, holes, keyways
• Sub-model approach for global/local mesh split

Contact Zones

• Matching mesh preferred (same element size on both surfaces)
• Non-matching: slave surface element size ≤ master surface element size/2
• Hertz contact: elements across contact zone ≈ 10 (zone width 2a)
  • 2a = 2√(2FR/π L E*) for line contact — pre-calculate, set element size
• Normal contact: penalty stiffness sensitive to mesh; use augmented Lagrange

Thin Walls (Shells)

• Minimum 4 elements across unsupported span between stiffeners
• 6 elements across radius of curvature for curved shells
• Element size ≈ √(R×t) / 2 (characteristic bending length of shell)

Singularities (Mesh-Independent Results)

Sharp re-entrant corners: σ → ∞ with refinement → NOT converging to physical value Identifiable by: stress keeps increasing with mesh refinement (no convergence)

Strategies:

1. Add fillet radius (best — matches reality)
2. Use fracture mechanics K_I approach (see fracture-mechanics skill)
3. Apply hot-spot stress method (IIW fatigue design)
4. Saint-Venant: stress > 3× characteristic dimension from singularity is unaffected

Pin-in-hole: stress at contact point is singular → Use contact elements (not bonded); report bearing stress σ_b = P/(d×t)

Submodeling (Global-Local)

Purpose: detailed stress in small region without meshing entire structure finely

Procedure:

1. Run coarse global model
2. Cut out region of interest
3. Apply interpolated displacements from global model to cut boundary
4. Run fine local model with applied boundary displacements
5. Check: local model boundary far enough from high-stress region (Saint-Venant ≥ 2-3 characteristic lengths)

Validity check: stress at cut boundary of local model ≈ global model (within 5%) Software: ANSYS submodel, Abaqus submodeling, NASTRAN SOL 400 SUPORT

Mesh Types

Structured (Mapped)

Hexahedral (3D), quadrilateral (2D) dominant More accurate per DOF, but harder to create for complex geometry Best for: uniform prismatic regions, thin walls, pressure vessels

Unstructured (Free)

Tetrahedral dominant (TET10 for accuracy) Easy to automate for complex geometry Less accurate per DOF → need finer mesh than hex

Hybrid

Hex-dominated core with tet fill at transitions Best practice for CAD-imported industrial models

Inflation Layers (Boundary Layer Meshing — CFD/Thermal)

For fluid simulation near walls: very thin elements to resolve boundary layer First cell height y₁ from wall: y₁ = y⁺ × ν / u_τ y⁺ = dimensionless wall distance (target: y⁺ < 1 for k-ω SST, y⁺ = 30-300 for k-ε + wall functions) u_τ = √(τ_w/ρ) (friction velocity, estimate from Cf × ½ρU²) Growth ratio: 1.2–1.3 per layer (gradual, 10–20 inflation layers typical)

Element Count Estimation

For stress analysis convergence study: Coarse: ~50,000 DOF Medium: ~200,000 DOF Fine: ~1,000,000 DOF Compare result: if < 5% change from Medium→Fine → Medium is sufficient

Mesh Transition

Avoid abrupt mesh size jumps > 3:1 ratio between adjacent elements Gradual size grading: 1.2–2× growth rate per element layer Pyramid/prism wedge elements for hex-to-tet transition

Practical Workflow (ANSYS)

1. Geometry cleanup: suppress small features (holes < 1mm for structural, unless critical)
2. Set global element size (based on expected stress gradient)
3. Add local sizing at stress concentrations, contact, fillets
4. Check mesh metrics: element quality, skewness, aspect ratio
5. Run coarse study first → identify high-stress regions → refine
6. Convergence study: medium vs. fine at critical location

Output

Provide: recommended element type, element size at critical locations [mm], aspect ratio check, expected DOF count, submodel strategy if applicable, mesh quality targets.