ANSYS

ANSYS is a leading simulation suite. Learn finite element fundamentals ([K]{u} = {F}), the Workbench workflow, element types, meshing and convergence, boundary conditions, linear static, modal and thermal analyses, APDL scripting and validating results.

Finite element analysis (FEA) divides a complex part into many small elements whose behaviour is simple, then solves thousands or millions of equations to predict stresses, deflections, temperatures and vibration modes.

ANSYS Mechanical (structural/thermal), Fluent/CFX (CFD) and Maxwell/HFSS (electromagnetics) are used across industry. The software is powerful — but results are only as good as the model, mesh, loads and boundary conditions.

An analogy

FEA is like modelling a complicated structure as a huge network of tiny springs: each spring is easy, and the computer balances all of them at once.

The FEA workflow

Geometry → material properties → mesh → boundary conditions (supports) and loads → solve → post-process (deflection, stress, reaction forces) → verify against hand calculations → iterate the design. Workbench links these steps in a project schematic.

Elements and meshing

1D beams/links, 2D shells for thin walls, 3D solids (tetrahedra, hexahedra). Quadratic (mid-side node) elements capture bending far better than linear ones. Refine mesh where stress gradients are high (fillets, holes) and run a mesh-convergence study: refine until results change < 2–5 %.

Boundary conditions and singularities

Over-constraining (fixing whole faces that would really flex) or point loads/sharp re-entrant corners create stress singularities: stress rises forever with refinement. Model realistic supports (bolts, contacts, remote displacements) and read stresses away from singular points or use proper fillet geometry.

Analysis types and verification

Linear static, modal (natural frequencies), harmonic, transient, buckling (eigenvalue), thermal, thermal-stress, fatigue, nonlinear (plasticity, contact, large deflection) and multiphysics. Verification (solving the equations right) and validation (right equations vs test data) — plus sanity checks on reaction forces, units and deformation shape — are essential before trusting results.

Formulas

• Governing equation (linear static): [K]{u} = {F}
• Bar element: k_e = (AE/L) [ 1 −1 ; −1 1 ]
• Modal analysis: ([K] − ω²[M]){φ} = 0
• Stress from strain: {σ} = [D][B]{u}

Worked example: Two-element bar by hand

Given: Element 1: A = 200 mm², L = 300 mm; Element 2: A = 100 mm², L = 200 mm; E = 200 GPa, F = 10 kN at the tip

Find: Tip displacement and stresses.

• k₁ = 200 × 200 000/300 = 133 333 N/mm
• k₂ = 100 × 200 000/200 = 100 000 N/mm
• Series: u₃ = F/k₁ + F/k₂ = 0.075 + 0.100 = 0.175 mm
• σ₁ = 50 MPa, σ₂ = 100 MPa

Answer: 0.175 mm — matches the APDL model

Worked example: Cantilever check

Given: 10 × 50 mm section, L = 500 mm; P = 1 kN, E = 200 GPa

Find: Hand value to validate FEA.

• I = 10 × 50³/12 = 104 167 mm⁴
• δ = 1000 × 500³/(3 × 200 000 × 104 167) = 2.0 mm

Answer: 2.0 mm — FEA should converge to this

APDL: stepped bar under axial load

/PREP7
ET,1,LINK180                 ! 3D spar element
MP,EX,1,200000               ! E in MPa (N, mm units)
MP,PRXY,1,0.3
SECTYPE,1,LINK $ SECDATA,200 ! area 200 mm^2
SECTYPE,2,LINK $ SECDATA,100 ! area 100 mm^2
N,1,0 $ N,2,300 $ N,3,500    ! nodes at x = 0, 300, 500 mm
SECNUM,1 $ E,1,2
SECNUM,2 $ E,2,3
D,1,ALL,0                    ! fix node 1
D,ALL,UY,0 $ D,ALL,UZ,0
F,3,FX,10000                 ! 10 kN at the free end
FINISH
/SOLU $ SOLVE $ FINISH
/POST1
PRNSOL,U,X                   ! expect UX(3) = 0.175 mm
ETABLE,SAX,LS,1 $ PRETAB,SAX ! axial stress: 50 and 100 MPa

APDL scripts give full, repeatable control — Workbench also accepts APDL command snippets.

Common mistakes

• Wrong: Trusting peak stress at a sharp corner or point load. — Right: Recognise singularities; model fillets and realistic supports, check convergence.
• Wrong: Inconsistent units. — Right: Use a consistent set (N, mm, MPa, t, s) — the solver doesn't check.

Applications

• Product development: Stress, stiffness and fatigue checks of brackets, housings and frames.
• Vibration & NVH: Modal and harmonic analysis of machines, vehicles and electronics.
• Thermal & multiphysics: Electronics cooling, turbine blades, battery packs.

Key takeaways

• FEA solves [K]{u} = {F} over a mesh.
• Converge the mesh; prefer quadratic elements.
• Beware singularities and unrealistic supports.
• Always verify with hand calculations.

Going further

• Submodelling: Refine a local region using displacements from a coarse global model.
• Contact & nonlinearity: Frictional contacts, bolt pretension and plasticity require Newton–Raphson iterations and careful convergence control.
• Optimisation: Parametric studies, DesignXplorer response surfaces and topology optimisation automate design improvement.