Finite Element Analysis cover
Interactive book · Semester 5-7

Finite Element Analysis

Watch a stiffness matrix assemble spring by spring, distort a quad until its Jacobian goes negative, and see why an explicit crash solver needs microsecond time steps

21 chapters, 21 interactives, few words. Every chapter is mapped to the Anna University, VTU, SPPU, Mumbai University and KTU units it covers: discretisation and convergence, the elasticity matrix, Rayleigh-Ritz and Galerkin methods, spring, bar and truss elements, elimination and penalty boundary conditions, thermal loads, beam elements with Hermite shape functions, the constant strain triangle, axisymmetric problems, higher-order and isoparametric elements, Gauss quadrature, mesh quality, heat transfer, natural frequencies, explicit and implicit time integration, Newton-Raphson for nonlinear problems and checking the results.

  • AUCME367Computational Solid Mechanics
  • VTUBME701Finite Element Methods
  • SPPU302050Computer Aided Engineering
  • MUMEC504Finite Element Analysis
  • KTUMET433Finite Element Method

By Skill-Lync · Updated 17 Nov 2026 · 21 chapters · 21 interactives · free, no sign-up

Chapter 1

What FEM does: discretisation, steps and convergence

Which syllabus covers thisAU CME367 Unit IIVTU BME701 Module 1SPPU 302050 Unit 1MU MEC504 Modules 1, 2KTU MET433 Module 1

What does the finite element method actually do?

It replaces a field you cannot solve for exactly (displacement in a bracket, temperature in a piston, pressure in a duct) by many small pieces, the elements, inside each of which the field is a simple polynomial fixed by its values at a few nodes. Writing equilibrium or energy balance for every element and joining them turns a differential equation into a set of algebraic equations, [K]{u} = {F}, that a computer solves. The same machinery handles structures, heat transfer, fluid flow and electromagnetics; only the meaning of u and K changes.

How is FEM different from FDM, FVM and BEM?

The finite difference method replaces derivatives by differences on a grid: simple, but awkward on curved boundaries. The finite volume method balances fluxes through the faces of small cells, so it conserves mass and energy exactly per cell, which is why most CFD codes use it. The finite element method approximates the field inside elements of any shape and works from energy or weighted-residual statements, so it dominates solid mechanics. The boundary element method meshes only the surface, which suits infinite domains and acoustics but gives dense matrices and needs a known fundamental solution.

What are the steps of an analysis, and where do the software tools fit?

Discretise the geometry into elements; choose the element type and its interpolation; form each element's stiffness matrix and load vector; assemble them into the global system; apply the boundary conditions; solve for the nodal unknowns; then post-process strains, stresses, reactions and checks. Commercial packages split this into a pre-processor (geometry clean-up, meshing, loads: HyperMesh, Ansys Mechanical), a solver (Ansys, Abaqus, LS-DYNA for crash, or free ones such as CalculiX and Code_Aster) and a post-processor for plots. Every number must be in one consistent unit system; mm-N-MPa-tonne is common for structures.

What are nodes, DOF, primary and secondary variables, and the two kinds of boundary condition?

A node is a point where the unknowns live; each unknown at a node is a degree of freedom: one axial displacement for a bar node, two (u, v) for a plane-stress node, three for a solid, and for a beam node a deflection and a rotation. The primary variable is what you solve for (displacement, temperature); secondary variables come from its derivatives (strain, stress, heat flux). An essential boundary condition prescribes the primary variable, such as u = 0 at a support. A natural boundary condition prescribes the secondary one, such as a force or heat flux, and enters through the load vector.

Does the answer get better with more elements, and how fast?

For a well-posed model, yes: refining the mesh (h-refinement) makes the answer converge to the exact solution of the mathematical model. With linear elements the displacement error falls roughly as h², so halving the element size cuts it to about a quarter, once the mesh is fine enough. For a steel hanger tapering from 600 to 150 mm², with each element given the average of its end areas, one element is 13% too stiff, two are 4.9% and four 1.5% off. Strong tapers converge more slowly at first, so always check with a refined mesh rather than trust one run.

Tapered bar by FEM: how the tip displacement converges to the exact answer as you add elements: interactive loads as you scroll
Predict, then check

A tapered bar is modelled with 4 linear elements and the tip displacement is 1.45% low. With 8 elements the error will be about

Worked examples

Tapered steel hanger with 1, 2 and 4 elements · Steel (E 200 GPa) hanger, area 600 mm² at the top falling linearly to 150 mm² at the tip, length 900 mm, tip load 18 kN (illustrative); each element uses the average of its end areas
  1. Exact: u = PL ln(A1/A0)/(E(A1 − A0)) = 18,000 × 900 × ln 0.25/(2,00,000 × (−450)) = 0.2495 mm
  2. 1 element: Ā = 375 mm², k = 2,00,000 × 375/900 = 83,333 N/mm, u = 18,000/83,333 = 0.2160 mm (−13.4%)
  3. 2 elements: Ā = 487.5 and 262.5 mm², k = 2,16,667 and 1,16,667 N/mm in series, u = 0.2374 mm (−4.9%)
  4. 4 elements: u = 0.2459 mm (−1.45%); 8 elements: 0.2486 mm (−0.39%)

Answer: Errors −13.4%, −4.9%, −1.45%, −0.39%: always too stiff, falling towards a factor of 4 per halving (3.76 from 4 to 8 elements)

Setting up a model in mm-N-MPa-tonne · A 100 × 50 × 20 mm steel block (density 7.82 g/cm³) and, separately, a 2 kg mass on a 50 N/mm spring, both modelled in mm
  1. Consistent set: length mm, force N, stress MPa (N/mm²), mass tonne, time s; then density is in tonne/mm³ and g = 9,810 mm/s²
  2. Density 7.82 g/cm³ = 7.82 × 10⁻⁹ t/mm³; volume 1,00,000 mm³ gives mass 7.82 × 10⁻⁴ t = 0.782 kg
  3. Weight = 7.82 × 10⁻⁴ × 9,810 = 7.67 N
  4. Spring: ω = √(k/m) = √(50/0.002) = 158.1 rad/s, f = 25.16 Hz; in SI √(50,000/2) gives the same

Answer: Mass 0.782 kg is entered as 7.82 × 10⁻⁴ t; the spring-mass frequency comes out in Hz (25.16) only because the units are consistent

Counting degrees of freedom · A plane-stress model of a pump bracket plate meshed with 12 × 4 four-node quadrilaterals, left edge fixed; and a solid model with 10 × 4 × 2 eight-node bricks
  1. Plate: (12 + 1) × (4 + 1) = 65 nodes × 2 DOF = 130 DOF
  2. Fixed left edge: 5 nodes × 2 = 10 DOF removed, 120 unknowns remain
  3. Solid: 11 × 5 × 3 = 165 nodes × 3 DOF = 495 DOF

Answer: 120 unknowns for the plate, 495 DOF for the brick mesh before supports

Chapter 2

Elasticity for FEA: strain-displacement, the [D] matrix, plane stress and plane strain

Which syllabus covers thisAU CME367 Unit IVTU BME701 Module 1SPPU 302050 Unit 4MU MEC504 Module 5KTU MET433 Module 3

How does an element get strain from nodal displacements?

Strain is the rate at which displacement changes: εx = ∂u/∂x, εy = ∂v/∂y, and the shear strain γxy = ∂u/∂y + ∂v/∂x is the loss of a right angle. In 3D three displacements give six strains. An element interpolates u and v from its nodes and differentiates them, packed as {ε} = [B]{d}. Differentiation loses one polynomial order, so strains and stresses are always less accurate than displacements, and with linear elements they are constant or linear inside each element.

What does 3D Hooke's law need for an isotropic material?

Only two constants, E and ν. Each normal strain is its own stress over E minus ν times the other two: εx = [σx − ν(σy + σz)]/E, and each shear strain is τ/G with G = E/2(1 + ν). Inverted, it is a 6 × 6 [D] matrix, often written with the Lamé constants λ and μ (μ = G). For steel, E 200 GPa and ν 0.3 give G = 76.9 GPa, λ = 115.4 GPa and bulk modulus K = E/3(1 − 2ν) = 166.7 GPa. As ν approaches 0.5, K grows without limit: rubber-like materials are nearly incompressible.

When is a 2D model plane stress, and when is it plane strain?

Plane stress suits thin parts loaded in their own plane, such as a bracket plate or a gusset: the faces are free, so σz = 0 and the plate thins by εz = −ν(εx + εy)/(1 − ν). Plane strain suits long bodies with the same section and load all along, such as a dam, a tunnel lining or a long roller: the length cannot change, so εz = 0 and a stress σz = ν(σx + σy) appears. Plane strain is stiffer, and as ν nears 0.5 its D11 runs away, which is why nearly incompressible materials need special elements.

Elasticity matrix [D]: plane stress and plane strain, strains to stresses and von Mises stress: interactive loads as you scroll

Why do FE plots show von Mises stress, and how is it found?

A ductile metal yields when its distortion energy reaches the value in a tensile test, which reduces any 3D stress state to one number: σvm = √{½[(σ1 − σ2)² + (σ2 − σ3)² + (σ3 − σ1)²]}. Compare it with the yield strength. The principal stresses come from the in-plane Mohr circle (the Strength of Materials book draws it) plus σz, which is zero in plane stress but not in plane strain. Von Mises is always positive, so it hides whether a region is in tension or compression: check the principal stresses for that.

How does temperature enter the stress calculation?

A free part heated by ΔT grows by α ΔT in every direction without stress. Stress comes only from the part of the strain the material is not allowed to take freely: {σ} = [D]({ε} − {ε0}) with ε0 = α ΔT for the normal strains and zero for shear. FE codes turn ε0 into equivalent nodal loads. A steel plate (α about 12 × 10⁻⁶/°C) fully held in its plane and heated 40 °C reaches −137 MPa: thermal stress needs no external load at all.

Predict, then check

Equal strains εx = εy = 500 µε are applied to a material with ν = 0.49. Compared with plane stress, the plane-strain σx is

Worked examples

Plane-stress stresses on a steel bracket plate · Strains from a strain-gauge rosette on a thin steel plate: εx = 600 µε, εy = −150 µε, γxy = 300 µε; E = 200 GPa, ν = 0.30
  1. E/(1 − ν²) = 2,00,000/0.91 = 2,19,780 MPa
  2. σx = 2,19,780 × (600 − 0.3 × 150) × 10⁻⁶ = 122.0 MPa; σy = 2,19,780 × (−150 + 0.3 × 600) × 10⁻⁶ = 6.59 MPa
  3. τxy = G γxy = 76,923 × 300 × 10⁻⁶ = 23.08 MPa
  4. Principal: 64.29 ± 62.14 = 126.4 and 2.15 MPa at 10.9° to x; σz = 0
  5. von Mises √(σ1² + σ2² − σ1σ2) = 125.4 MPa; the plate thins by εz = −193 µε

Answer: σx 122.0, σy 6.6, τxy 23.1 MPa; σvm 125 MPa, well below the 250 MPa yield of A36 steel

Plane strain in a long aluminium section · A long aluminium extrusion held at its ends so it cannot change length; strains in the section εx = 400 µε, εy = 100 µε, γxy = 0; E = 69 GPa, ν = 0.33
  1. E/((1 + ν)(1 − 2ν)) = 69,000/(1.33 × 0.34) = 1,52,587 MPa; so D11 = 1,02,234 MPa and D12 = 50,354 MPa
  2. σx = 45.93 MPa, σy = 30.36 MPa
  3. σz = ν(σx + σy) = 0.33 × 76.29 = 25.18 MPa (the ends must push to keep εz = 0)
  4. Plane stress with the same strains: σx = 33.53, σy = 17.96 MPa
  5. von Mises (plane strain, with σz) = 18.71 MPa

Answer: Plane strain: σx 45.9, σy 30.4, σz 25.2 MPa; plane stress would report σx only 33.5 MPa, so the choice of idealisation changes the answer by about 37%

A restrained steel plate heated by 40 °C · Thin steel plate held on all edges so εx = εy = 0; heated uniformly by 40 °C; E = 200 GPa, ν = 0.30, α = 12 × 10⁻⁶/°C (inside the 10.8-12.5 range)
  1. Initial strain ε0 = α ΔT = 12 × 10⁻⁶ × 40 = 480 µε in x and y
  2. Mechanical strain = total − ε0 = −480 µε in both directions
  3. σx = σy = E/(1 − ν²) × (1 + ν) × (−480 µε) = −E α ΔT/(1 − ν) = −137.1 MPa
  4. Out of plane the plate is free: εz = α ΔT − ν(σx + σy)/E = 891 µε

Answer: σx = σy = −137 MPa compression with no external load; von Mises 137 MPa

Chapter 3

Total potential energy and the Rayleigh-Ritz method

Which syllabus covers thisAU CME367 Unit IIVTU BME701 Module 1SPPU 302050 Unit 3MU MEC504 Module 2KTU MET433 Module 1

What is total potential energy, and why is it a minimum at equilibrium?

Total potential energy Π = U − W is the strain energy stored in the body minus the work the loads do as they move with it. Of all displacement fields that respect the supports, the one in equilibrium makes Π stationary, and for a stable elastic body that stationary point is a minimum. A 10 N/mm spring under 50 N: Π(u) = 5u² − 50u is smallest at u = 5 mm, where Π = −125 N·mm, exactly −½ × load × deflection. That last result, Π = −½W, holds for every linear elastic solution.

What makes a trial function admissible?

The Ritz method guesses the deflection as v = a1 φ1 + a2 φ2 + … and finds the coefficients that make Π stationary. Each φ must satisfy the essential (geometric) boundary conditions: zero deflection and zero slope at a fixed end, zero deflection at a pin. Natural conditions, such as zero moment at a free end, need not be built in; the energy statement enforces them approximately. The functions must be smooth enough for the strain energy to exist (slopes continuous for beams) and, as terms are added, able to approach any shape: ξ², ξ³, ξ⁴ for a cantilever, sin πξ, sin 3πξ for a simply supported beam.

How good is a one-, two- or three-term Ritz answer?

It depends on whether the trial functions can reach the exact shape. A cantilever with a tip load has a cubic deflection: one term (ξ²) gives a tip deflection 25% low, two terms (ξ², ξ³) are exact. Under a UDL the exact curve is quartic: one term is 33% low, three terms are exact. A simply supported beam with one sine is 0.39% high at mid-span, three sines are within 0.01%. An axial bar under a uniform load gets the tip right with one linear term but halves the stress at the support.

Rayleigh-Ritz method: beam and bar deflections from 1, 2 and 3 trial terms against the exact curve: interactive loads as you scroll

Why is a displacement-based Ritz answer too stiff?

Limiting the shape to a few functions is like adding hidden constraints: the structure cannot deform in the way it really wants, so it behaves stiffer. Since Π at the solution is −½ × work of the loads and Π can only be higher than the true minimum, the load-weighted deflection is always under-estimated, and adding terms can only lower Π. A single point load means its own deflection is under-estimated. Local values elsewhere can overshoot slightly (one sine on the simply supported beam is 0.39% high at mid-span) and stresses converge more slowly than deflections.

How does piecewise Rayleigh-Ritz become the finite element method?

Global trial functions get awkward for real shapes, so FEM uses local ones: each shape function is non-zero only over the elements around one node and equals 1 at that node. The Ritz coefficients become the nodal displacements, so they have a physical meaning, and the Π integral splits into a sum over elements. Making Π stationary element by element gives the element stiffness matrices; adding them by node numbers is assembly. Everything in the convergence argument (too stiff, Π falls with refinement) carries over to a displacement-based finite element mesh.

Predict, then check

A cantilever with a tip load is solved by Ritz with the single trial function v = a x². The tip deflection will be

Worked examples

Steel cantilever with a tip load: one and two terms · Steel cantilever (E 200 GPa) 1.2 m long, 50 × 100 mm section (I = 4.17 × 10⁶ mm⁴), tip load 3 kN (illustrative)
  1. EI = 2,00,000 × 41,66,667 = 8.333 × 10¹¹ N·mm²; exact tip PL³/(3EI) = 2.0736 mm
  2. One term v = a x²: U = ½EI ∫(2a)² dx = 2EI L a², W = P a L², dΠ/da = 0 → a = PL/(4EI) = 1.08 × 10⁻⁶ /mm
  3. Tip = a L² = 1.5552 mm (−25%); Π = −½ P v = −2,332.8 N·mm against exact −3,110.4 N·mm
  4. Two terms v = a1 x² + a2 x³: EI[4L 6L²; 6L² 12L³]{a} = P{L²; L³} → a1 = 2.16 × 10⁻⁶ /mm, a2 = −6.0 × 10⁻¹⁰ /mm²
  5. Tip = a1 L² + a2 L³ = 3.1104 − 1.0368 = 2.0736 mm

Answer: One term 1.555 mm (25% low), two terms 2.0736 mm = exact, because the exact deflection is a cubic

Simply supported beam under a UDL with sine terms · Steel I-beam over a 4 m span, 6 kN/m (6 N/mm) floor load, I = 2.5 × 10⁷ mm⁴ (illustrative); trial v = Σ ak sin(kπx/L), k = 1, 3, 5
  1. Exact mid-span: 5wL⁴/(384EI) = 5 × 6 × 4,000⁴/(384 × 2,00,000 × 2.5 × 10⁷) = 4.0000 mm
  2. The sines are orthogonal, so each coefficient is found alone: ak = 4wL⁴/(EI π⁵ k⁵)
  3. a1 = 4.0154 mm, a3 = 0.01652 mm, a5 = 0.001285 mm
  4. Mid-span (sin kπ/2 = +1, −1, +1): 4.0154, 3.9989, 4.0002 mm
  5. Π one term = −30,676 N·mm, exact = −w²L⁵/(240EI) = −30,720 N·mm

Answer: One sine: 4.015 mm (+0.39%); three sines: 4.0002 mm (+0.005%). Π stays above the exact value even when the mid-span deflection overshoots

A hanging rod: right deflection, wrong stress · Steel rod 20 mm diameter, 6 m long, hanging from the top under its own weight (density 7.82 g/cm³); one-term Ritz u = a x
  1. A = 314.2 mm²; load per length q = ρ g A = 7.82 × 10⁻⁹ × 9,810 × 314.2 = 0.02410 N/mm
  2. Exact: u(L) = qL²/(2EA) = 0.00690 mm; stress at the top qL/A = ρgL = 0.460 MPa, zero at the bottom
  3. Ritz: Π = ½EA a² L − q a L²/2 → a = qL/(2EA); tip = aL = 0.00690 mm, exact
  4. Ritz stress E a = 0.230 MPa everywhere: half the true value at the top; Π is 0.75 of exact

Answer: Tip deflection exact (6.90 µm), but the stress is a constant 0.230 MPa against a true 0.460 MPa at the support

Chapter 4

Strong and weak forms, weighted residuals and Galerkin's method

Which syllabus covers thisAU CME367 Unit IIVTU BME701 Module 1SPPU not in syllabusMU MEC504 Module 1KTU MET433 Module 5

What is the strong form of a problem?

It is the differential equation plus its boundary conditions, demanded at every point. For a bar with a distributed axial load q(x): −d/dx(EA du/dx) = q, with u = 0 at a support (essential) and EA du/dx = P at a loaded end (natural). For 1D conduction with heat generation it is the same equation with k in place of EA and temperature in place of u. Solving the strong form exactly needs u to have a second derivative everywhere, which is easy for a uniform bar and hopeless for a real component.

What is a residual, and what does 'weighted' mean?

Put an approximate solution ũ = Σ ai φi into the equation and it does not balance: what is left over, R(x) = q + (EA ũ′)′, is the residual. It cannot be zero everywhere with a few unknowns, so we ask for zero in an average sense: ∫ w R dx = 0 for as many weighting functions w as there are unknowns. Each choice of weights is a different method, and each gives a set of linear equations for the coefficients ai.

How do collocation, subdomain, least squares and Galerkin differ?

Point collocation makes R zero at chosen points: cheap, but the answer depends on the points. Subdomain makes the average of R zero over each region. Least squares minimises ∫R² dx, using weights ∂R/∂ai. Galerkin uses the trial functions themselves as weights. For −u″ = sin πx with one term x(1 − x), the mid-point value is +23.4% off by collocation, −21.5% by subdomain and least squares, but only −4.5% by Galerkin. For a symmetric problem Galerkin gives the best fit in strain energy, which is why FEM uses it.

Weighted residuals: collocation, subdomain, least squares and Galerkin on the same problem: interactive loads as you scroll

What does integrating by parts buy, and what is the weak form?

Multiply the strong form by a weight w and integrate by parts once. The second derivative of u becomes first derivatives on both u and w, so piecewise-linear functions with kinks at nodes become usable: only C0 continuity is needed. The boundary term [EA u′ w] is exactly the end force, so natural conditions enter the equations by themselves, while essential ones are built into the trial functions. With Galerkin's choice w = φi the matrix is symmetric, the same [K] the Rayleigh-Ritz energy method gives.

How does Galerkin's method give the element equations of a bar or a wall?

Use linear shape functions N1 = 1 − x/h, N2 = x/h on each element of length h as both trial and weight functions. The weak form gives (EA/h)[1 −1; −1 1]{u} = (q h/2){1; 1} for a bar with a uniform load, and (k/h)[1 −1; −1 1]{T} = (q‴ h/2){1; 1} per unit area for a plane wall with heat generation. Assemble, apply the end values, solve. For these 1D equations the nodal values come out exact; between nodes the answer is only a straight line. The Heat and Mass Transfer book solves the same wall by finite differences.

Predict, then check

Solve −u″ = x, u(0) = u(1) = 0 with the trial functions x(1 − x) and x²(1 − x). Which weighted-residual methods give the exact answer?

Worked examples

Four methods on a wall with a sine-shaped heat source · Carbon-steel wall (k = 54 W/mK) 40 mm thick, both faces held at 30 °C, heat generated as q0 sin(πx/L) with q0 = 4 × 10⁶ W/m³ (illustrative, induction heating); one trial term T − 30 = a1 ξ(1 − ξ), ξ = x/L
  1. Scale: T − 30 = (q0 L²/k) ũ(ξ) with −ũ″ = sin πξ; q0 L²/k = 4 × 10⁶ × 0.04²/54 = 118.52 °C
  2. Residual R = sin πξ − 2a1. Collocation at ξ = ½: a1 = 0.5000. Subdomain ∫R = 0: a1 = 1/π = 0.3183. Least squares (weight −2): same, 0.3183
  3. Galerkin: ∫R ξ(1 − ξ) dξ = 4/π³ − a1/3 = 0 → a1 = 12/π³ = 0.3870
  4. Centre rise = 118.52 × a1/4: collocation 14.81, subdomain 9.43, Galerkin 11.47 °C; exact 118.52/π² = 12.01 °C

Answer: Centre temperature: exact 42.01 °C; Galerkin 41.47 (−4.5% on the rise), collocation 44.81 (+23%), subdomain and least squares 39.43 (−21%)

Two-term Galerkin for a bar with a growing load · Steel bar (E 200 GPa, A = 400 mm²) 2 m long, both ends fixed, axial load rising linearly from 0 to q0 = 30 N/mm (illustrative); trial u = (q0 L²/EA)[a1 ξ(1 − ξ) + a2 ξ²(1 − ξ)]
  1. Dimensionless form −ũ″ = ξ; Galerkin after integrating by parts: Σ aj ∫φi′φj′ dξ = ∫ξ φi dξ
  2. [K] = [1/3 1/6; 1/6 2/15], {F} = {1/12; 1/20}
  3. Solve: a1 = 0.1667, a2 = 0.1667, so ũ = (ξ − ξ³)/6, the exact solution
  4. Scale q0 L²/EA = 30 × 2,000²/(2,00,000 × 400) = 1.50 mm; mid-length u = 1.5 × 0.0625 = 0.09375 mm
  5. End forces EA u′: left q0L/6 = 10 kN, right q0L/3 = 20 kN; total load q0L/2 = 30 kN

Answer: u(L/2) = 0.0938 mm, exact; reactions 10 kN and 20 kN, the far end carries twice as much

Galerkin finite elements for a heated wall · Carbon-steel wall (k = 54 W/mK) 60 mm thick with uniform heat generation 5 × 10⁶ W/m³ (illustrative), both faces at 30 °C; two linear elements of h = 30 mm, per m² of wall
  1. Element: (k/h)[1 −1; −1 1]{T} = (q h/2){1; 1} with k/h = 1,800 W/m²K and q h/2 = 75,000 W/m²
  2. Assembled middle row: −1,800 T1 + 3,600 T2 − 1,800 T3 = 1,50,000
  3. With T1 = T3 = 30: T2 = (1,50,000 + 3,600 × 30)/3,600 = 71.67 °C
  4. Exact centre: 30 + qL²/(8k) = 71.67 °C, the same. At x = 15 mm: FE 50.83 °C (straight line) against exact 61.25 °C

Answer: Centre 71.67 °C, exact at the node; between nodes the linear element is 10.4 °C low at the quarter point, so refine where the gradient matters

Chapter 5

Direct stiffness method: spring elements, assembly and the properties of [K]

Which syllabus covers thisAU not in syllabusVTU BME701 Module 2SPPU 302050 Unit 3MU MEC504 Modules 2, 3KTU MET433 Module 1

What is a spring element, and where does its matrix come from?

A spring element has two nodes, one displacement each, and a rate k. Pull node 2 by u₂ with node 1 held and the spring pushes back on node 2 with k u₂ and on node 1 with −k u₂. Doing the same for u₁ fills the other column. So the element force vector is k[1 −1; −1 1] times {u₁, u₂}. Each column is the set of nodal forces needed for a unit displacement of one node, which is what every stiffness matrix in FEM means, from bars to shells. Units here: N and mm, so k is in N/mm.

How does the direct stiffness method build the global [K]?

Number every node. Each element knows its two global node numbers, so its four terms are added into the global matrix at those rows and columns: k₁₁ goes to (i, i), k₁₂ to (i, j) and so on. Where two springs share a node, both add to that diagonal term, which is why a node between springs of 150 and 300 N/mm has K = 450. The load vector is filled the same way. Then supports are applied, K u = F is solved, and reactions and spring forces are recovered. Watch the matrix fill spring by spring below.

Direct stiffness method: watch a global stiffness matrix assemble spring by spring: interactive loads as you scroll

What properties does the global [K] have, and why is it singular before supports?

It is symmetric (Kij = Kji, from Maxwell's reciprocal theorem), its diagonal terms are positive, and for a structure with no supports each row sums to zero: moving every node by the same amount stretches nothing, so K times a uniform displacement is zero. That rigid-body motion makes the determinant zero, so [K] cannot be inverted until enough supports stop it. A solver that reports a zero pivot is almost always telling you a part is free to fly away. After supports, [K] is positive definite and usually sparse and banded.

Why does node numbering matter?

Non-zero terms sit only where two nodes share an element, so they cluster near the diagonal. A banded solver stores and works only inside the half-bandwidth, which is set by the largest difference between node numbers in any element. Number a 6-node spring chain in order and the half-bandwidth is 2; number it 1, 4, 2, 5, 3, 6 and it becomes 4, doubling storage and much more than doubling work on big models. Commercial codes renumber nodes automatically (the reverse Cuthill-McKee idea), but hand problems and exam answers still use the formula.

Predict, then check

You assemble [K] for three springs in series but forget to fix the wall node, then ask the solver for the displacements. What happens?

Worked examples

Three springs in series · A wall, then springs k₁ = 150, k₂ = 300 and k₃ = 100 N/mm in a row (nodes 1-4, node 1 at the wall); P = 600 N pulls node 4. Rates and load illustrative
  1. Assemble: [K] = [150 −150 0 0; −150 450 −300 0; 0 −300 400 −100; 0 0 −100 100] N/mm; each row sums to 0
  2. Fix node 1 (strike row and column 1): [450 −300 0; −300 400 −100; 0 −100 100]{u₂ u₃ u₄} = {0 0 600}
  3. Solve: u₂ = 4 mm, u₃ = 6 mm, u₄ = 12 mm
  4. Check: 600 × (1/150 + 1/300 + 1/100) = 12 mm, the series-spring answer
  5. Reaction R₁ = −150 × 4 = −600 N; every spring carries 600 N of tension

Answer: u₄ = 12 mm, wall reaction −600 N, 600 N in each spring

Two carts between walls · Wall, k₁ = 200 N/mm, cart 1, k₂ = 100 N/mm, cart 2, k₃ = 300 N/mm, wall; P = 900 N pushes cart 1 towards cart 2 (illustrative)
  1. Both walls fixed, so only the two cart rows remain: [300 −100; −100 400]{u₁ u₂} = {900 0}
  2. Determinant 300 × 400 − 100² = 1,10,000; u₁ = 900 × 400/1,10,000 = 3.273 mm, u₂ = 900 × 100/1,10,000 = 0.818 mm
  3. Check: k₁ in parallel with k₂, k₃ in series is 275 N/mm; 900/275 = 3.273 mm
  4. Reactions: left wall −200 × 3.273 = −654.5 N, right wall −300 × 0.818 = −245.5 N; they sum to −900 N
  5. Spring forces: k₁ 654.5 N tension, k₂ and k₃ 245.5 N compression

Answer: Cart 1 moves 3.27 mm, cart 2 0.82 mm; walls take 654.5 N and 245.5 N

Half-bandwidth and node numbering · Five springs in a chain, six nodes, one DOF per node. Numbering A along the chain: 1, 4, 2, 5, 3, 6. Numbering B: 1 to 6 in order
  1. Numbering A: elements join 1-4, 4-2, 2-5, 5-3, 3-6; the largest difference is 3, so NBW = (3 + 1) × 1 = 4
  2. Numbering B: every element joins consecutive numbers, difference 1, so NBW = 2
  3. Banded storage 6 × NBW: 24 terms for A, 12 for B, against 36 for the full matrix
  4. As a plane truss with 2 DOF per node the same numberings give NBW = 8 and 4

Answer: Number along the short direction of a structure: here it halves the half-bandwidth from 4 to 2

Chapter 6

Linear bar element: shape functions, stepped bars, elimination and penalty methods

Which syllabus covers thisAU CME367 Unit VVTU BME701 Module 2SPPU 302050 Unit 3MU MEC504 Module 3KTU MET433 Module 1

What are the shape functions of a 2-node bar element?

Inside an element of length L the displacement is taken as a straight line between the nodal values: u(x) = N₁u₁ + N₂u₂. N₁ is 1 at node 1 and 0 at node 2, N₂ the reverse, and they add to 1 everywhere so a rigid shift is reproduced exactly. In the natural coordinate ξ from −1 to 1 they are (1 − ξ)/2 and (1 + ξ)/2. Differentiating gives the strain ε = [B]{q} with [B] = (1/L)[−1 1], so strain and stress σ = E[B]{q} are constant inside each element.

Where do the bar stiffness matrix and load vectors come from?

Strain energy in the element is ½∫εEεA dx. With ε = [B]{q} this becomes ½{q}ᵀ(AE/L)[1 −1; −1 1]{q}, so the bar behaves exactly like a spring of rate AE/L. Loads spread along the bar are shared out with the same shape functions: a uniform axial load q per unit length gives qL/2 at each node, and self-weight gives ρgAL/2 at each node. Point loads go straight onto the node they act at. In mm-N-MPa units AE/L comes out in N/mm.

How are stepped and tapered bars modelled?

A stepped bar needs a node at every change of area, material or load, and one element per piece is exact for end loads because each piece has constant force. A tapered bar is usually split into several elements, each given the average of its end areas. That is an approximation: two elements on a 3:1 taper under a tip load are about 2.9% too stiff, four elements about 0.8%, falling roughly as the square of the element size, and always on the stiff side here.

Elimination or penalty: how are supports applied?

Elimination strikes out the rows and columns of supported DOFs and solves what is left; it is exact and the reactions follow from R = K u − F. The penalty method keeps every equation and adds a very stiff spring C at each support, so the support moves by a tiny amount, about reaction/C, and the reaction is −C times that movement. It is easy to program, handles prescribed non-zero displacements and contact the same way, but the error falls only as 1/C, and a C far too large spoils round-off. C ≈ 10⁴ × the largest diagonal term is a common rule of thumb.

Stepped bar: elimination against the penalty method for boundary conditions, and how big C must be: interactive loads as you scroll
Predict, then check

A bar is fixed at one end and loaded at the other. You apply the support by the penalty method with C = 10⁴ × the largest diagonal term of [K]. How far does the 'fixed' node move, compared with the loaded tip?

Worked examples

Steel and aluminium stepped bar · Fixed at the left: steel A₁ = 300 mm², L₁ = 250 mm (E 200 GPa), then aluminium A₂ = 600 mm², L₂ = 400 mm (E 69 GPa); P = 24 kN pulls the free tip. Units mm, N, MPa; sizes illustrative
  1. Element rates: AE/L = 300 × 2,00,000/250 = 2,40,000 N/mm and 600 × 69,000/400 = 1,03,500 N/mm
  2. [K] = 10³ × [240 −240 0; −240 343.5 −103.5; 0 −103.5 103.5] N/mm
  3. Eliminate node 1, solve [343.5 −103.5; −103.5 103.5] × 10³ {u₂ u₃} = {0 24,000}: u₂ = 0.100 mm, u₃ = 0.3319 mm
  4. Stresses σ = E(u₂ − u₁)/L: steel 80 MPa, aluminium 40 MPa (= P/A, as they must be)
  5. Reaction R₁ = K₁₂u₂ = −2,40,000 × 0.1 = −24,000 N

Answer: Tip moves 0.332 mm; steel 80 MPa, aluminium 40 MPa, wall reaction 24 kN

Same bar between two walls, by penalty · Both ends fixed; 30 kN pushes the step towards the aluminium. Supports by penalty with C = 10⁴ × max Kii (rule of thumb)
  1. Exact (elimination): u₂ = 30,000/(2,40,000 + 1,03,500) = 0.08734 mm; R₁ = −20,960.7 N, R₃ = −9,039.3 N
  2. Penalty: C = 10⁴ × 3,43,500 = 3.435 × 10⁹ N/mm added to K₁₁ and K₃₃; solve the full 3 × 3 system
  3. Result: u₂ = 0.08734 mm, wall nodes move 6.10 × 10⁻⁶ and 2.63 × 10⁻⁶ mm
  4. Reactions −C·u: −20,960.4 N and −9,039.6 N, summing to −30,000 N
  5. Error in u₂: 0.0058 %

Answer: Penalty matches elimination to 0.0058 %: the steel side takes 20.96 kN, the aluminium side 9.04 kN

Tapered bar by average-area elements · Steel bar, 600 mm long, area 600 mm² at the fixed end tapering linearly to 200 mm² at the free end; P = 20 kN at the tip
  1. Exact: δ = PL ln(A₀/A₁)/(E(A₀ − A₁)) = 20,000 × 600 × ln 3/(2,00,000 × 400) = 0.1648 mm
  2. Two elements (300 mm each), average areas 500 and 300 mm²: δ = 20,000 × 300/2,00,000 × (1/500 + 1/300) = 0.1600 mm, error −2.91 %
  3. Four elements, areas 550, 450, 350, 250 mm²: δ = 0.1635 mm, error −0.81 %
  4. Halving the element size cut the error by 3.6 times, close to the 4 expected for an h² method

Answer: Tip movement 0.165 mm exact; average-area elements are slightly stiff (−2.9 % with 2, −0.8 % with 4)

Chapter 7

Quadratic bar elements, temperature loads and support gaps

Which syllabus covers thisAU not in syllabusVTU BME701 Module 2SPPU 302050 Unit 3MU MEC504 Module 3KTU not in syllabus

What does a 3-node (quadratic) bar element add?

A middle node lets the displacement inside the element be a parabola, so strain and stress can vary linearly instead of being constant. With the end nodes at ξ = ∓1 and the middle node at 0, the shape functions are −ξ(1 − ξ)/2, ξ(1 + ξ)/2 and 1 − ξ². Each is 1 at its own node and 0 at the others, and they add to 1. Integrating BᵀAEB over the element gives the matrix below, for node order end 1, end 2, middle. Its rows still sum to zero.

When is one quadratic element exact?

Whenever the true displacement is a polynomial of degree two or less, the element can reproduce it, so its answer is exact. A bar with a uniform axial load (a rod carrying its own weight, or a uniform friction drag) has exactly that: linear force, linear stress, parabolic displacement. One quadratic element then gives the right displacement everywhere and the right stress at both ends. One linear element gets the tip displacement right too, but its single constant stress is only half the peak at the support.

How does a temperature change enter a bar element?

Heating by ΔT gives an initial strain ε₀ = αΔT that needs no stress. Stress comes only from the part of the strain the bar is not allowed to have: σ = E(ε − αΔT). In the FE equations the initial strain appears as an equivalent load, EAαΔT pulling the two nodes apart: [−1, 1] times that force. Add it to the load vector, solve as usual, then subtract αΔT when recovering stress. A free bar gets displacement and no stress; a fully held bar gets −EαΔT, about −120 MPa for steel at 50 °C.

Bar with a temperature rise and a gap to the wall: does the gap close, and what stress follows: interactive loads as you scroll

How do you handle a gap between the bar and a wall?

A gap is the simplest contact problem, and it is solved by checking an assumption. First assume the gap stays open: solve with the far end free and find how far it moves. If that movement is less than the gap, you are done. If it is more, the bar touches the wall, so solve again with the far-end displacement prescribed equal to the gap (by elimination, or by a penalty spring). The wall force from the second solve must push back on the bar; if it pulled, the first assumption was the right one.

Predict, then check

A steel bar is held between two rigid walls and heated by 50 °C. You double its length and heat it by the same 50 °C. What happens to the thermal stress?

Worked examples

One quadratic element for a rod under uniform load · Steel rod, L = 600 mm, A = 250 mm², fixed at x = 0, uniform axial load q = 20 N/mm along its length (illustrative). Units mm, N, MPa
  1. AE/3L = 250 × 2,00,000/1,800 = 27,777.78 N/mm; consistent load qL[1/6, 1/6, 2/3] = [2,000, 2,000, 8,000] N
  2. End 1 fixed: [7 −8; −8 16] × 27,777.78 {u₂ u₃} = {2,000 8,000} (u₂ the free end, u₃ the middle)
  3. Solve: free end u₂ = 0.072 mm, middle u₃ = 0.054 mm; exact qL²/2EA = 0.072 and 3qL²/8EA = 0.054
  4. Stress σ = E(2/L) Σ (dNᵢ/dξ) uᵢ: 48 MPa at the support, 0 at the free end; exact qL/A = 48 MPa
  5. One linear element: same tip movement, but one constant stress E u₂/L = 24 MPa

Answer: The quadratic element is exact: tip 0.072 mm, stress 48 MPa at the support; a linear element shows only 24 MPa

Aluminium bar heated against a wall · Aluminium bar, L = 400 mm, A = 300 mm², fixed at the left, gap Δ = 0.15 mm to a rigid wall on the right, heated by 40 °C; E 69 GPa, α 23 × 10⁻⁶/°C
  1. Free growth αΔT L = 23 × 10⁻⁶ × 40 × 400 = 0.368 mm > 0.15 mm: the gap closes, at ΔT = 0.15/(23 × 10⁻⁶ × 400) = 16.3 °C
  2. FE with one element: AE/L = 51,750 N/mm, thermal load EAαΔT = 19,044 N on [−1, 1]
  3. Prescribe u₂ = 0.15 mm: wall force R₂ = (AE/L)u₂ − F₂ = 51,750 × 0.15 − 19,044 = −11,281.5 N
  4. Stress σ = E(Δ/L − αΔT) = 69,000 × (0.15/400 − 9.2 × 10⁻⁴) = −37.6 MPa

Answer: The wall pushes back with 11.28 kN; the bar is at −37.6 MPa, well inside aluminium's 95 MPa yield

Steel and copper bar with a gap · Fixed at the left: steel L₁ = 300 mm, A₁ = 400 mm², then copper L₂ = 200 mm, A₂ = 600 mm² (E 117 GPa, α 16.5 × 10⁻⁶/°C); gap 0.1 mm to a wall; ΔT = 50 °C
  1. Free growth (12 × 300 + 16.5 × 200) × 10⁻⁶ × 50 = 0.345 mm: the gap closes at ΔT = 14.5 °C
  2. Compatibility: 0.345 − R(L₁/A₁E₁ + L₂/A₂E₂) = 0.1, with flexibilities 3.750 and 2.849 × 10⁻⁶ mm/N
  3. R = 0.245/6.599 × 10⁶ = 37,127 N; the FE solve with u₃ = 0.1 mm gives the same
  4. Stresses: steel −92.8 MPa, copper −61.9 MPa; the joint moves 0.0408 mm

Answer: Wall force 37.1 kN; steel −93 MPa (yield 250), copper −62 MPa, close to copper's 70 MPa yield

Chapter 8

Plane truss elements: local and global coordinates, transformation and member stress

Which syllabus covers thisAU not in syllabusVTU BME701 Module 3SPPU 302050 Unit 3MU MEC504 Module 3KTU MET433 Module 2

What does a truss element assume?

Members are straight, joined by frictionless pins, and loaded only at the joints, so each member carries a single axial force, tension or compression, and no bending. Each joint has two DOFs, u and v. The element is the bar element of the last chapter, turned to point in any direction. Unlike the method of joints, FEM does not care whether the truss is statically determinate: it solves stiffness equations, not equilibrium alone, so redundant members cost nothing extra. A real welded bracket that bends needs beam elements instead.

How are local and global coordinates linked?

Along the member (local x′) the element is a bar with two DOFs. In the global x-y plane each node has two. The direction cosines l = cos θ and m = sin θ, computed from the node coordinates, connect them: the stretch-direction displacement of a node is q′ = l·u + m·v. Writing this for both nodes gives the 2 × 4 transformation matrix [L] = [l m 0 0; 0 0 l m], and the global element stiffness is [L]ᵀ k′ [L]. No angle needs to be measured; coordinates are enough.

What is the truss element stiffness matrix, and how is a truss solved?

Multiplying out [L]ᵀ(EA/L)[1 −1; −1 1][L] gives (EA/L) times a 4 × 4 matrix whose top-left 2 × 2 block is [l² lm; lm m²], with the same block negated off the diagonal. Assemble it at the two nodes' four global DOFs, exactly as with springs, strike out the pinned DOFs, and solve. A horizontal member (l = 1, m = 0) adds stiffness only in x; two members in a straight line leave the joint free to swing sideways, and [K] turns singular.

Plane truss by FEM: direction cosines, assembly, node displacement and member stresses: interactive loads as you scroll

How are member stresses and reactions recovered?

Pick the element's four global displacements from the solution, project them on the member to get the stretch, and multiply by E/L: σ = (E/L)(−l u₁ − m v₁ + l u₂ + m v₂). Positive is tension. The member force is σA. Reactions come from the rows that were struck out: R = K u − F at each pinned DOF. A quick check: reactions plus applied loads must sum to zero in x and in y, and moments must balance too.

Predict, then check

A two-bar wall bracket (statically determinate) is made of steel. You remake both bars in aluminium of the same size (E 69 GPa against 200 GPa). What happens?

Worked examples

Two-bar wall bracket · Pump bracket on a wall: joint 800 mm from the wall; bar 1 horizontal to a wall pin; bar 2 from a pin 600 mm lower (1,000 mm long); both steel, A = 200 mm²; 12 kN hangs from the joint. Sizes illustrative; mm, N, MPa
  1. Bar 1: l = 1, m = 0, EA/L = 50,000 N/mm. Bar 2: l = 0.8, m = 0.6 (from its pin to the joint), EA/L = 40,000 N/mm
  2. Joint stiffness (pins struck out): [50,000 + 40,000 × 0.64, 40,000 × 0.48; 40,000 × 0.48, 40,000 × 0.36] = [75,600 19,200; 19,200 14,400] N/mm
  3. Solve with F = {0, −12,000}: u = 0.32 mm, v = −1.26 mm
  4. σ₁ = (2,00,000/800)(1 × 0.32) = 80 MPa; σ₂ = (2,00,000/1,000)(0.8 × 0.32 + 0.6 × (−1.26)) = −100 MPa
  5. Method of joints check: bar 2 carries 12/0.6 = 20 kN compression, bar 1 20 × 0.8 = 16 kN tension: 80 and −100 MPa

Answer: Joint moves 0.32 mm out and 1.26 mm down; bar 1 80 MPa tension, bar 2 100 MPa compression

Stiffness and stress of one inclined member · Steel member at 30° to the x axis, L = 1,500 mm, A = 150 mm². Solved nodal displacements: node 1 (0, 0), node 2 (0.6, −0.2) mm
  1. EA/L = 150 × 2,00,000/1,500 = 20,000 N/mm; l = cos 30° = 0.8660, m = 0.5
  2. l² = 0.75, lm = 0.4330, m² = 0.25, so the top-left block is 10³ × [15 8.66; 8.66 5] N/mm, repeated with signs in the 4 × 4
  3. σ = (E/L)(l × 0.6 + m × (−0.2)) = 133.3 × (0.5196 − 0.1) = 55.9 MPa
  4. Member force σA = 8,392 N; the nodal forces [k]{q} at node 2 have exactly this resultant, along the member

Answer: Stress 55.9 MPa tension, force 8.39 kN

Three-bar fan (indeterminate) · A joint hangs 1,200 mm below a ceiling from a vertical middle bar (A = 300 mm²) and two outer bars at 30° from the vertical (A = 200 mm² each), all steel; P = 30 kN down
  1. Middle bar EA/L = 50,000 N/mm; outer bars L = 1,200/cos 30° = 1,385.6 mm, EA/L = 28,867.5 N/mm
  2. Vertical stiffness of the joint: 50,000 + 2 × 28,867.5 × cos² 30° = 93,301.3 N/mm; the horizontal terms cancel by symmetry
  3. v = 30,000/93,301.3 = 0.3215 mm down
  4. Middle bar force 16,077 N (53.6 MPa); outer bars 8,038 N each (40.2 MPa)
  5. Check: 16,077 + 2 × 8,038 × cos 30° = 30,000 N

Answer: The stiff vertical bar takes 54% of the load; joint sags 0.322 mm

Chapter 9

Beam element: Hermite shape functions, stiffness and equivalent nodal loads

Which syllabus covers thisAU CME367 Unit VVTU BME701 Module 3SPPU 302050 Unit 1MU MEC504 Module 3KTU MET433 Module 2

Why does a beam node carry a slope as well as a deflection?

An Euler-Bernoulli beam (plane sections stay plane and normal to the axis, shear deformation ignored) stores energy in bending, ½∫EI(v″)² dx. That integral needs v″, so the deflection and its slope must both be continuous across nodes: C1 continuity. If neighbouring elements met only in v, a kink at a node would have infinite curvature. So each node gets two DOFs, deflection v and rotation θ = dv/dx, and a 2-node element has four. Four conditions fix exactly four coefficients: a cubic, v = a0 + a1x + a2x² + a3x³. Shear-flexible (Timoshenko) beams, used for deep sections, interpolate v and θ separately.

What are the Hermite shape functions?

With s = x/L, H1 = 1 − 3s² + 2s³ and H3 = 3s² − 2s³ give unit deflection at one end with zero slope at both; H2 = L(s − 2s² + s³) and H4 = L(s³ − s²) give unit slope at one end with no deflection at either. Then v(x) = H1v1 + H2θ1 + H3v2 + H4θ2. H1 + H3 = 1 everywhere, so a rigid translation costs no strain energy, and any cubic is reproduced exactly. Because v″ of a cubic is linear, the bending moment EI v″ inside one element is linear and the shear EI v‴ is constant.

Beam element: the four Hermite shape functions and the equivalent nodal loads of a UDL: interactive loads as you scroll

Where does the beam stiffness matrix come from?

Put v = [H]{d} into the strain energy ½∫EI(v″)² dx and differentiate with respect to the nodal DOFs: k = ∫EI [H″]ᵀ[H″] dx. For a uniform element this integrates to the familiar 4 × 4 matrix with entries 12, 6L, 4L² and 2L² times EI/L³. Each column is the set of end forces and moments that holds one DOF at 1 and the others at 0, the same numbers as the slope-deflection equations. The matrix is symmetric and singular until supports are applied: a rigid translation (1, 0, 1, 0) and a rigid rotation (0, 1, L, 1) both give zero force.

How are loads between nodes put on the nodes?

As consistent (work-equivalent) loads: f_i = ∫N_i q dx, so the nodal loads do the same virtual work as the real load. A uniform load w gives wL/2 at each node plus end moments wL²/12 of opposite sense. A point load P at distance a gives P times the Hermite values there, which equal the fixed-end forces with the signs reversed, for example Pab²/L² as a moment. Dropping the moments (lumping wL/2 per node) is simpler but less accurate. After solving, the true member end forces are k d minus these equivalent loads, and the moment and shear follow from v″ and v‴.

Predict, then check

A cantilever is modelled with one beam element and a load at its tip. How good is the FE tip deflection?

Worked examples

Deflection and moments from nodal values · One element, L = 2.5 m; EI = 200 GPa × 3 × 10⁷ mm⁴ (illustrative I) = 6 × 10¹² N mm²; nodal values from a solution: v1 = 0, θ1 = 0, v2 = −5 mm, θ2 = −2.4 × 10⁻³ rad. Units N, mm, MPa
  1. At mid-span s = 0.5: H3 = 0.5, H4 = L(0.125 − 0.25) = −312.5 mm
  2. v(mid) = 0.5 × (−5) + (−312.5) × (−0.0024) = −1.75 mm
  3. v″(0) = 6v2/L² − 2θ2/L = −4.80 × 10⁻⁶ + 1.92 × 10⁻⁶ = −2.88 × 10⁻⁶ /mm, so M1 = EI v″ = −17.28 kN m
  4. v″(L) = −6v2/L² + 4θ2/L = 0.96 × 10⁻⁶ /mm, so M2 = 5.76 kN m
  5. Shear EI v‴ = (M2 − M1)/L = 9.22 kN, constant along the element

Answer: v(mid) = −1.75 mm; the moment runs linearly from −17.28 to 5.76 kN m

Consistent loads for a UDL and an off-centre point load · Element L = 3 m carrying a downward UDL of 12 kN/m, and separately a downward 30 kN point load 1 m from node 1 (illustrative)
  1. UDL: forces wL/2 = 18 kN down at each node; moments wL²/12 = 9 kN m, clockwise at node 1 and counter-clockwise at node 2
  2. Point load, s = a/L = 1/3: H1 = 20/27, H2 = 4L/27, H3 = 7/27, H4 = −2L/27
  3. Forces: 30 × 20/27 = 22.22 kN and 30 × 7/27 = 7.78 kN, summing to 30 kN
  4. Moments: 30 × 4 × 3/27 = 13.33 kN m at node 1 and 30 × 2 × 3/27 = 6.67 kN m at node 2, opposite senses
  5. Check: Pab²/L² = 30 × 1 × 2²/3² = 13.33 kN m, the fixed-end moment

Answer: UDL: 18 kN and 9 kN m at each end; point load: 22.22 kN + 13.33 kN m and 7.78 kN + 6.67 kN m

One-element cantilever · Cantilever 1.8 m long, EI = 200 GPa × 1.2 × 10⁷ mm⁴ = 2.4 × 10¹² N mm² (illustrative I), 6 kN down at the tip
  1. Fix v1 = θ1 = 0; keep rows 3 and 4: (EI/L³)[12 −6L; −6L 4L²]{v2; θ2} = {−6,000; 0}
  2. Solve: v2 = −PL³/3EI = −4.86 mm, θ2 = −PL²/2EI = −4.05 × 10⁻³ rad
  3. Reactions from rows 1 and 2: 6.0 kN up and 10.8 kN m at the wall
  4. Mid-span by interpolation: 0.5 × −4.86 + (−225) × (−0.00405) = −1.519 mm; beam theory Px²(3L − x)/6EI gives −1.519 mm

Answer: Tip −4.86 mm and mid-span −1.52 mm, both exact: the true curve is a cubic

Chapter 10

Solving beams by FEM: point loads, UDL, couples and spring supports

Which syllabus covers thisAU CME367 Unit VVTU BME701 Module 3SPPU not in syllabusMU MEC504 Module 3KTU MET433 Module 2

What are the steps for solving a beam by FEM?

Put nodes at every support, every point load or couple and every change of section or load. Number the DOFs (v and θ per node), build each element's 4 × 4 stiffness and consistent load vector, and assemble them into [K]{u} = {F}. Point forces and couples at nodes go straight into {F}. Apply the supports by striking out fixed DOFs: a pin fixes v, a built-in end fixes v and θ. Solve the reduced system, then get reactions from the full system, R = K u − F, and each element's end forces from k d minus its equivalent loads. Units here: N, mm and MPa.

How are couples, spring supports and indeterminate beams handled?

A couple at a node is simply a load on that node's rotation DOF. An elastic support of stiffness k adds k to the diagonal term of its deflection DOF, and the spring force is k times that deflection. A tip spring on a cantilever acts in parallel with the beam's own tip stiffness 3EI/L³, so the tip moves P/(k + 3EI/L³). Statically indeterminate beams (propped, fixed-fixed and continuous) need no extra compatibility equations: the stiffness method is the same for all of them, which is why commercial codes never ask whether a structure is determinate.

Beams by FEM: propped, fixed, continuous and spring-supported beams against the exact deflection: interactive loads as you scroll

Where is a beam FE solution exact and where is it not?

With consistent loads, the nodal deflections and rotations of Euler-Bernoulli beam elements are exact, even with loads inside elements, because the true deflection between loads is a cubic, which the element contains. Reactions and end moments from K u − F are exact too. Between nodes, the FE curve is only the Hermite interpolation of the nodal values: under a UDL the true curve is quartic, so one element of a propped cantilever shows exactly half the true mid-span deflection. The FE moment EI v″ is linear inside each element and jumps at nodes; under a UDL it needs several elements to approach the parabola.

What does a two-span continuous beam teach?

Two equal spans of a beam carrying a uniform load w, simply supported at three points, would need a compatibility equation by hand. By FEM it is two elements and three rotation unknowns. By symmetry the middle support does not rotate, so each span acts like a propped cantilever: the end reactions are 3wL/8, the middle one 10wL/8 = 1.25wL, and the hogging moment over the middle support is wL²/8. The middle support carries 25% more than two simply supported spans would hand it. Cutting the beam over the middle support leaves the peak moment at wL²/8 but makes the largest deflection 2.4 times bigger.

Predict, then check

A propped cantilever with a UDL is modelled with one beam element. How does the FE deflection at mid-span compare with the exact value?

Worked examples

Propped cantilever with a UDL, one element and two · Span 4 m, fixed at A, propped at B; UDL 10 kN/m; EI = 200 GPa × 5 × 10⁷ mm⁴ = 10¹³ N mm² (illustrative I). Units N, mm
  1. One element: only θB is free. Row 4: (4EI/L) θB = −(−w)L²/12 = wL²/12
  2. θB = wL³/48EI = 10 × 4,000³/(48 × 10¹³) = 1.333 × 10⁻³ rad
  3. Reactions R = K u − F: RA = 25 kN, MA = 20 kN m, RB = 15 kN (5wL/8, wL²/8, 3wL/8)
  4. Mid-span by interpolation: 0.667 mm; exact 1.333 mm
  5. Two elements: the mid-span node gives 1.333 mm, now exact; the true maximum is 1.387 mm, 2.31 m from A

Answer: Reactions 25 kN, 20 kN m and 15 kN are exact with one element; mid-span needs a node there (1.33 mm)

Cantilever resting on a spring · Cantilever 2 m, EI = 200 GPa × 10⁷ mm⁴ = 2 × 10¹² N mm² (illustrative I), tip on a spring k = 500 N/mm (illustrative), 5 kN down at the tip
  1. Spring: add k to the diagonal term of v2. Reduced [K] = [12EI/L³ + k, −6EI/L²; −6EI/L², 4EI/L]
  2. 12EI/L³ = 3,000 N/mm, 6EI/L² = 30,00,000 N, 4EI/L = 4 × 10⁹ N mm
  3. Solve with F = {−5,000; 0}: v2 = −4.00 mm; check P/(k + 3EI/L³) = 5,000/(500 + 750) = 4 mm
  4. Spring force k × 4 = 2.0 kN; wall: 3.0 kN and 6.0 kN m

Answer: Tip moves 4.0 mm; the spring takes 2 kN and the wall 3 kN

Two-span continuous beam · Two equal spans of 5 m, pinned at three supports, UDL 8 kN/m, EI = 200 GPa × 10⁸ mm⁴ = 2 × 10¹³ N mm² (illustrative I)
  1. Two elements; v1 = v2 = v3 = 0, unknowns θ1, θ2, θ3
  2. Solve: θ2 = 0 by symmetry, θ1 = −θ3 = −1.0417 × 10⁻³ rad (wL³/48EI)
  3. Reactions R = K u − F: 15, 50 and 15 kN (3wL/8, 10wL/8, 3wL/8)
  4. Moment over the middle support from element 1's end forces: −25 kN m (wL²/8, hogging)

Answer: Middle support 50 kN, ends 15 kN each, support moment 25 kN m hogging

Chapter 11

Constant strain triangle: area coordinates, the [B] matrix and element stiffness

Which syllabus covers thisAU CME367 Unit IIVTU BME701 Module 4SPPU 302050 Unit 4MU MEC504 Modules 4, 5KTU MET433 Module 3

What is a constant strain triangle?

The simplest 2D solid element: three corner nodes, two displacements (u, v) at each, six DOFs. Inside, each displacement is linear, u = α1 + α2x + α3y, and three nodal values fix the three coefficients. Differentiate a linear field and you get a constant, so the strains, and with them the stresses, are the same everywhere in the element. Triangles mesh any 2D shape automatically, which is why the CST was the first general 2D element, and it is still the easiest one to work by hand. It is used for plane stress (thin plates) and plane strain (long bodies) through the [D] matrix.

What are area coordinates?

A point P inside the triangle splits it into three smaller triangles. The area of the one opposite node i, divided by the whole area A, is Li. So L1 + L2 + L3 = 1, Li = 1 at node i and 0 at the other two, and Li falls linearly in between: they are exactly the CST shape functions. In Cartesian form Ni = (ai + bi x + ci y)/2A, with bi and ci the coordinate differences of the other two nodes and 2A the determinant of the node coordinates. A point outside the triangle gets a negative Li, a quick inside test used by mesh search codes.

Constant strain triangle: area coordinates, the [B] matrix and why the strain is constant: interactive loads as you scroll

How is the CST stiffness built?

Differentiate the shape functions: εx = Σ bi ui/2A, εy = Σ ci vi/2A and γxy = Σ (ci ui + bi vi)/2A. These sit in the 3 × 6 matrix [B], whose entries are only the bi and ci divided by 2A, so [B] is constant. The stiffness integral then needs no numerical integration: k = t A [B]ᵀ[D][B], a 6 × 6 symmetric matrix with three zero-energy (rigid body) modes. Stress is σ = [D][B]{u}. A body force splits a third to each node; a uniform edge traction splits half to each node of that edge.

Why does a CST mesh need so many elements in bending?

Bending needs a strain that varies across the depth, but a CST can carry only one value. Worse, when it is forced into a bending shape it shows a shear strain that the real beam does not have, and that spurious shear soaks up energy and makes the mesh too stiff (shear locking). In the third example, 20 CSTs one layer deep give under a quarter of the tip deflection of a cantilever; 320 elements still miss by almost a fifth. Use quadratic triangles (T6) or quads in bending regions, and keep CSTs for nearly uniform stress fields.

Predict, then check

Under any nodal displacements, where in a CST is the strain largest?

Worked examples

[B] and stiffness of one triangle · Nodes 1 (0, 0), 2 (40, 0), 3 (10, 30) mm; thickness 4 mm; steel, E = 200 GPa, ν = 0.3, plane stress. Units N, mm, MPa
  1. bi = yj − yk: b1 = 0 − 30 = −30, b2 = 30 − 0 = 30, b3 = 0. ci = xk − xj: c1 = 10 − 40 = −30, c2 = 0 − 10 = −10, c3 = 40
  2. 2A = 40 × 30 − 10 × 0 = 1,200 mm², A = 600 mm²
  3. [B] = (1/1,200) × [−30 0 30 0 0 0; 0 −30 0 −10 0 40; −30 −30 −10 30 40 0]
  4. [D] = E/(1 − ν²) [1 ν 0; ν 1 0; 0 0 (1 − ν)/2]: D11 = 219,780, G = 76,923 MPa
  5. k11 = t A (D11 b1² + G c1²)/(2A)² = 4 × 600 × (2,19,780 × 900 + 76,923 × 900)/1,200² = 4,45,055 N/mm

Answer: k11 = k22 = 4,45,055 N/mm, k55 = 2,05,128 N/mm, k66 = 5,86,081 N/mm; each row sums to zero over the x DOFs and over the y DOFs

Strains and stresses from nodal displacements · Same triangle; nodal displacements (u1, v1, u2, v2, u3, v3) = (0, 0, 0.020, 0, 0.008, −0.010) mm
  1. εx = (b2 u2 + b3 u3)/2A = 30 × 0.020/1,200 = 500 µε
  2. εy = c3 v3/2A = 40 × (−0.010)/1,200 = −333 µε
  3. γxy = (c2 u2 + c3 u3)/2A = (−10 × 0.020 + 40 × 0.008)/1,200 = 100 µε
  4. σ = [D]ε: σx = 87.9 MPa, σy = −40.3 MPa, τxy = 7.69 MPa
  5. von Mises √(σx² − σxσy + σy² + 3τ²) = 114.3 MPa

Answer: σx = 87.9, σy = −40.3, τxy = 7.7 MPa, von Mises 114 MPa, the same at every point of the element

How stiff is a CST cantilever? · Steel cantilever 200 mm long, 20 mm deep, 10 mm thick, plane stress, fixed end, 1 kN tip shear spread over the end-edge nodes. Meshes of right triangles, 1, 2 and 4 layers deep
  1. Beam theory: PL³/3EI = 2.000 mm with I = 10 × 20³/12 = 6,667 mm⁴; adding shear PL/(κGA), κ = 5/6, gives 2.016 mm
  2. 10 × 1 mesh, 20 CSTs: 0.462 mm, 23% of it
  3. 20 × 2 mesh, 80 CSTs: 1.083 mm, 54%
  4. 40 × 4 mesh, 320 CSTs (205 nodes): 1.654 mm, 82%

Answer: Even 320 triangles give only 82% of the deflection: CSTs converge slowly in bending and always from the stiff side

Chapter 12

Axisymmetric problems: a thick cylinder with radial elements

Which syllabus covers thisAU not in syllabusVTU BME701 Module 4SPPU 302050 Unit 4MU MEC504 Module 5KTU not in syllabus

When can a 3D solid be solved as an axisymmetric 2D model?

When the geometry, the loads, the supports and the material are all the same at every angle around one axis: pressure vessels and pipes under pressure, flywheels and discs spinning about their own axis, pistons, nozzles, bolts in tension and press-fitted hubs. The model is then the r-z cross-section, one half of the section drawn on one side of the axis, meshed in 2D, with the circumferential direction handled by the formulation. A bolt hole, a side load or a keyway breaks the symmetry; such parts need 3D models or harmonic (Fourier) elements.

Why is there a hoop strain even though nothing moves around the ring?

A point that moves outwards by u sits on a bigger circle: its circumference grows from 2πr to 2π(r + u), a strain of u/r. So an axisymmetric element has four strains, εr = ∂u/∂r, εz = ∂w/∂z, γrz and the hoop strain εθ = u/r, which needs no derivative. Each element is really a ring of volume 2πr̄A, so stiffness and loads are integrated with 2πr dr dz, and a pressure on a ring of radius r gives a nodal force p × 2πr per unit length. Nodes on the axis (r = 0) must have u = 0.

How do radial elements model a thick cylinder?

Far from its ends, a long pressurised cylinder has u depending only on r, so one row of 2-node radial elements is enough. A long cylinder is plane strain (εz = 0); a thin ring is plane stress (σz = 0). The Lamé solution gives σθ = A + B/r² and σr = A − B/r² for both; only the displacement differs. Because 1/r is not a polynomial, the element integral is done with 2-point Gauss in r. No support is needed: the hoop strain alone resists a rigid radial movement. Stresses read at the bore node are the least accurate; element-centre values converge much faster.

Axisymmetric thick cylinder with radial elements against the Lame solution: interactive loads as you scroll

What changes in an axisymmetric triangle?

The 3-node ring element (VTU's axisymmetric triangle) uses the same linear shape functions as a CST in r and z, but its [B] gains a fourth row for the hoop strain, Ni/r. That row varies through the element, so [B] is no longer constant. The usual hand method evaluates [B] at the centroid r̄ = (r1 + r2 + r3)/3 and multiplies by the ring volume 2πr̄A (Pappus' theorem). A uniform radial movement u of all three nodes then gives εr = εz = 0 but a hoop strain u/r̄: an axisymmetric mesh must never be checked with a rigid-body test in r.

Predict, then check

A hydraulic cylinder with a 100 mm bore radius and a 50 mm wall is made twice as thick (100 mm wall), same pressure. What happens to the hoop stress at the bore?

Worked examples

Lamé stresses in a hydraulic cylinder · Bore radius 100 mm, outer radius 150 mm, internal pressure 40 MPa (illustrative); steel E = 200 GPa, ν = 0.3
  1. A = p ri²/(ro² − ri²) = 40 × 10,000/12,500 = 32 MPa; B = A ro² = 7,20,000 MPa mm²
  2. Bore: σθ = 32 + 72 = 104 MPa, σr = −40 MPa; outside: σθ = 64 MPa, σr = 0
  3. Thin-wall estimate p r/t: 80 MPa on the bore radius, 100 MPa on the mean radius: both low
  4. Bore movement: plane stress (r/E)[(1 − ν)A + (1 + ν)B/r²] = 58.0 µm; plane strain 55.1 µm

Answer: Hoop stress 104 MPa at the bore falling to 64 MPa outside; the bore grows by about 58 µm in radius (plane stress)

The same cylinder with radial elements · As above, plane stress, steel; linear radial elements, k = ∫BᵀDB r dr per radian by 2-point Gauss; load p ri = 4,000 N per mm of length per radian at the bore node
  1. One element, h = 50 mm: Gauss points at r = 125 ∓ 50/(2√3) = 110.57 and 139.43 mm
  2. k11 = 0.5162 × 10⁶; solve the 2 × 2 system: u at the bore = 56.26 µm (−3.0%)
  3. σθ read at the bore node: 111.2 MPa against 104 (+7%); at the element centre r = 125 mm: 78.22 against 78.08 MPa
  4. Four elements: u bore 57.88 µm, σθ at the bore node 107.2 MPa

Answer: Displacements converge fast (−3% with one element); read stresses at element centres, not at the bore node

Ring volume and hoop strain of an axisymmetric triangle · Triangle in the r-z section with nodes (100, 0), (130, 0), (100, 40) mm; all three nodes move outwards by 0.05 mm
  1. Area A = ½ × 30 × 40 = 600 mm²; centroid r̄ = (100 + 130 + 100)/3 = 110 mm
  2. Ring volume 2π r̄ A = 4,14,690 mm³ (Pappus; a fine-grid integral of 2πr over the triangle gives 4,14,690)
  3. Hoop row of [B] at the centroid: Ni/r̄ = 1/(3 × 110) = 0.00303 per mm for each node
  4. Uniform outward movement: εr = εz = 0, but εθ = 0.05/110 = 455 µε

Answer: Ring volume 4,14,690 mm³; a 'rigid' radial shift of 0.05 mm still strains the ring by 455 µε

Chapter 13

Higher-order elements: Pascal's triangle, Lagrange and serendipity families, convergence requirements

Which syllabus covers thisAU CME367 Unit IIVTU BME701 Module 4SPPU 302050 Unit 1MU MEC504 Module 4KTU MET433 Modules 2, 4

Which polynomial terms should an element carry?

An element approximates displacement with a polynomial that has exactly one coefficient per node. Pascal's triangle lists the candidate terms row by row: 1; x, y; x², xy, y²; and so on. Take whole rows where you can, so the element is complete to that degree: 3 nodes give a complete linear field (T3), 6 a complete quadratic (T6), 10 a complete cubic (T10), since a complete degree p needs (p + 1)(p + 2)/2 terms. When a row must be cut, pick terms symmetrically (x²y with xy², never one alone) so the element behaves the same whichever way it is drawn: geometric isotropy.

Pascal's triangle and element families: which polynomial terms each element carries: interactive loads as you scroll

What is the difference between Lagrange and serendipity quads?

Lagrange quads are tensor products of 1D Lagrange polynomials: Q4 is linear × linear (1, ξ, η, ξη), Q9 is quadratic × quadratic and needs a node in the middle for its ξ²η² term. Serendipity quads keep nodes on the boundary only: Q8 has 4 corners and 4 mid-sides, carrying ξ²η and ξη² but not ξ²η². Both are complete only to degree 2. Q8 is cheaper (no interior node) and is the usual 8-node choice in commercial codes; Q9 behaves better when badly distorted. The triangle family T3, T6, T10 uses area coordinates and is complete row by row.

What must shape functions satisfy for the answers to converge?

Completeness: the element must reproduce rigid-body motion (no strain) and a state of constant strain exactly, so as elements shrink the field can match any smooth solution; a complete linear polynomial does both. Compatibility (conformity): displacement must be continuous across element edges, which C0 shape functions give for bars and plane elements; beams and plates need slopes continuous too (C1). Every proper shape function set has two checks: N_i = 1 at its own node and 0 at the others (Kronecker delta), and ΣN_i = 1 everywhere (partition of unity), so a rigid shift moves the whole element.

What is the patch test?

Bruce Irons's practical check: build a small patch of elements, deliberately distorted, with at least one interior node. Apply boundary displacements taken from a linear field such as u = 0.001x + 0.0005y. A good element reproduces that field exactly, and so a constant strain everywhere, with zero error at the interior node. Elements that fail can converge to a wrong answer however fine the mesh. Passing it is a strong practical sign, though mathematicians have shown it is neither strictly necessary nor sufficient for convergence. Software developers run it on every new element formulation.

Predict, then check

An 8-node serendipity quad: what is the value of a CORNER node's shape function at the element centre?

Worked examples

Interpolating inside an 8-node quad · Q8 element with nodal displacements u (mm): corners 1-4: 0, 0.020, 0.050, 0.030; mid-sides 5-8 (bottom, right, top, left): 0.010, 0.035, 0.040, 0.015. Find u at ξ = η = 0.5
  1. Corners ¼(1 + ξξi)(1 + ηηi)(ξξi + ηηi − 1): N1 = −0.1250, N2 = −0.1875, N3 = 0.0, N4 = −0.1875
  2. Mid-sides: N5 = ½(1 − ξ²)(1 − η) = 0.1875, N6 = ½(1 + ξ)(1 − η²) = 0.5625, N7 = 0.5625, N8 = 0.1875
  3. Check: ΣN = 1.0000 and ΣN ξi = 0.5000 = ξ
  4. u = Σ N u = 0.03750 mm

Answer: u = 0.0375 mm; three corner functions are negative at this point, so the interpolation is not a simple weighted average

What a higher-order mesh costs · A 200 × 80 mm plate (say a bracket web, illustrative) meshed 10 × 4 for plane stress, 2 DOF per node. Compare Q4, Q8 and Q9
  1. Q4: (10 + 1)(4 + 1) = 55 nodes, 110 DOF
  2. Q9: every element edge and centre gets a node: (2 × 10 + 1)(2 × 4 + 1) = 189 nodes, 378 DOF
  3. Q8: Q9 minus the 40 centre nodes = 149 nodes, 298 DOF
  4. Splitting each quad into two T6 triangles gives the same 189-node grid as Q9

Answer: 110, 298 and 378 DOF: Q8 saves 21% of the nodes of Q9 with the same complete degree

Strain inside a 3-node bar · 3-node bar element, L = 120 mm; end nodes u1 = 0 and u2 = 0.090 mm, mid node u3 = 0.050 mm. Find u and strain at x = 30 mm (ξ = −0.5) and the strain at x = 90 mm
  1. N1 = ξ(ξ − 1)/2 = 0.375, N2 = ξ(ξ + 1)/2 = −0.125, N3 = 1 − ξ² = 0.75
  2. u(30) = −0.125 × 0.090 + 0.75 × 0.050 = 0.02625 mm
  3. ε = (2/L) Σ (dN/dξ) u: at ξ = −0.5, (2/120)(0 + 0 + 1 × 0.050) = 833 µε; at ξ = +0.5, (2/120)(0.090 − 0.050) = 667 µε
  4. A 2-node element over the same length sees only 0.090/120 = 750 µε everywhere

Answer: u = 0.0263 mm; strain falls linearly from 833 to 667 µε, where the linear element can only show the average 750 µε

Chapter 14

Isoparametric elements: natural coordinates, mapping and the Jacobian

Which syllabus covers thisAU CME367 Unit IIVTU BME701 Module 4SPPU 302050 Unit 2MU MEC504 Module 5KTU MET433 Module 4

Why describe every element in natural coordinates?

Each real element, whatever its size and shape, is drawn as the image of one parent element: a square with ξ and η running from −1 to 1 (a triangle with area coordinates for T3 and T6). Shape functions, their derivatives and the integration points are then written once, in ξ and η, and reused for every element of the mesh. Isoparametric means the same shape functions describe the geometry and the displacement. Sub-parametric uses fewer geometry nodes than displacement nodes (straight-sided Q8 used as Q4 geometry); super-parametric uses more, which is rare because it can fail the constant-strain test.

What does the Jacobian do?

The mapping x = ΣN_i x_i, y = ΣN_i y_i links the two spaces, and the Jacobian matrix [J] holds its derivatives: how far x and y move per unit step in ξ and η. det J is the local area scale, so an element's area is ∫∫det J dξ dη. For a Q4, det J is linear in ξ and η, and at a corner it equals a quarter of the cross product of the two edges meeting there, so a rectangle has det J = area/4 everywhere. Strains need derivatives in x and y, which come from J⁻¹ times the ξ, η derivatives.

Isoparametric mapping of a 4-node quad: distort the element and watch the Jacobian: interactive loads as you scroll

When does the mapping break down?

det J must stay positive everywhere in the element. Pull one corner inwards until the quad is concave (an interior angle above 180°) and det J at that corner goes negative: the mapping folds over itself and the element would claim negative area near that node. Number the nodes clockwise and det J is negative everywhere. Solvers stop on a negative Jacobian. A quad whose angles approach 0° or 180° is already poor because det J varies strongly across it, which is why pre-processors report the Jacobian ratio, min/max det J, and flag values below about 0.7 (HyperMesh's guidance).

How is the stiffness of an isoparametric element computed?

Build [B] at a point from the x, y derivatives of the shape functions (found through J⁻¹), then integrate BᵀDB times thickness over the parent square, multiplying by det J to convert dξ dη into real area. Because J⁻¹ divides by det J, the integrand of a distorted element is a ratio of polynomials, which is why it is done numerically by Gauss quadrature (next chapter). The same mapping lets a Q8 have curved edges: put the mid-side node off the straight line and the edge becomes a parabola, which models a hole or fillet with far fewer elements than straight-sided Q4s.

Predict, then check

A 4-node quad is a parallelogram (not a rectangle). How does det J vary over it?

Worked examples

Jacobian, area and a mapped point · Q4 with nodes 1 (0, 0), 2 (80, 0), 3 (90, 50), 4 (10, 40) mm. Find [J] and det J at the centre, the area, the corner det J values and the point at ξ = 0.5, η = −0.5
  1. At ξ = η = 0: ∂N/∂ξ = ¼[−1 1 1 −1], ∂N/∂η = ¼[−1 −1 1 1]
  2. ∂x/∂ξ = ¼(80 + 90 − 10) = 40, ∂y/∂ξ = ¼(50 − 40) = 2.5, ∂x/∂η = ¼(−80 + 90 + 10) = 5, ∂y/∂η = ¼(50 + 40) = 22.5
  3. det J = 40 × 22.5 − 2.5 × 5 = 887.5 mm² per unit ξη area; area = 4 × 887.5 = 3,550 mm² (shoelace: 3,550 mm²)
  4. Corner det J (quarter of the edge cross products): 800, 1000, 975, 775; at the 2 × 2 Gauss points 822.5 to 952.5, Jacobian ratio 0.86
  5. N at (0.5, −0.5) = [0.1875, 0.5625, 0.1875, 0.0625] → x = 62.500 mm, y = 11.875 mm

Answer: det J = 887.5 at the centre, area 3,550 mm², Jacobian ratio 0.86 (above 0.7); the point maps to (62.50, 11.88) mm

Strains through the inverse Jacobian · Same element; nodal x-displacements u = 0, 0.040, 0.050, 0.010 mm. Find εx = ∂u/∂x and ∂u/∂y at the centre
  1. ∂u/∂ξ = ¼(−0 + 0.040 + 0.050 − 0.010) = 0.020 mm; ∂u/∂η = ¼(−0 − 0.040 + 0.050 + 0.010) = 0.005 mm
  2. J⁻¹ = (1/887.5)[22.5 −2.5; −5 40]
  3. ∂u/∂x = (22.5 × 0.020 − 2.5 × 0.005)/887.5 = 493.0 × 10⁻⁶
  4. ∂u/∂y = (−5 × 0.020 + 40 × 0.005)/887.5 = 112.7 × 10⁻⁶

Answer: εx = 493 µε and ∂u/∂y = 113 × 10⁻⁶ (∂u/∂y is one of the two terms of γxy; the other, ∂v/∂x, comes from the v displacements)

A concave quad the Gauss points do not catch · Q4 with nodes (0, 0), (60, 0), (25, 20), (0, 50) mm: node 3 pulled inwards past the line from node 2 to node 4
  1. Corner det J: 750.0, 300.0, −137.5, 312.5: negative at node 3, whose interior angle exceeds 180°
  2. At the 2 × 2 Gauss points det J = 562.4, 302.6, 50.1, 309.9: all positive, so a solver that checks only the Gauss points runs
  3. Area = Σ Gauss det J = 1,225 mm² = shoelace area 1,225 mm²
  4. Jacobian ratio at the Gauss points = 50.1/562.4 = 0.089, far below the 0.7 HyperMesh guidance

Answer: Invalid element: det J = −137.5 at node 3. The stiffness would still be computed, but strains near node 3 are meaningless; move the node to make the quad convex

Chapter 15

Numerical integration: Gauss quadrature, full and reduced integration

Which syllabus covers thisAU CME367 Unit IIVTU not in syllabusSPPU not in syllabusMU not in syllabusKTU MET433 Module 4

Why are element integrals done numerically?

Stiffness, mass and load integrals of isoparametric elements contain J⁻¹, and J⁻¹ divides by det J, so for any element that is not a parallelogram the integrand is a ratio of polynomials with no tidy closed form. A rule that samples the integrand at a few points and adds weighted values is fast, easy to code once for every element, and exact whenever the integrand happens to be a polynomial of low enough degree. A Q4 stiffness matrix, for example, needs the 3 × 8 [B] matrix at only 4 points.

How does Gauss-Legendre quadrature choose its points?

With n points there are 2n unknowns, n positions and n weights, so they can be chosen to integrate 1, ξ, ξ², … up to ξ^(2n−1) exactly on [−1, 1]. The points turn out to be the roots of the Legendre polynomial P_n: n = 1 uses ξ = 0 with weight 2; n = 2 uses ±1/√3 with weights 1; n = 3 uses 0 (8/9) and ±√0.6 (5/9). Newton-Cotes rules (trapezoid, Simpson) fix equally spaced points and only tune the weights, so with the same n points they are exact to degree n − 1, or n for odd n.

Gauss quadrature: points, weights and the degree each rule integrates exactly: interactive loads as you scroll

How many points does an element need?

In 2D the rule is applied in each direction: an n × n grid of points with weights w_i w_j. For an undistorted Q4, BᵀDB contains terms up to ξ² and η², so 2 × 2 points integrate it exactly: this is full integration. A rectangular Q8 needs 3 × 3; a 2 × 2 rule is often used instead. A 1D quadratic bar needs 2 points, a cubic Hermite beam 2 points for stiffness. Distorted elements are never integrated exactly, but the error stays small while the element shape is reasonable. Loads and mass matrices may need one more point than stiffness.

What are reduced integration, hourglassing and shear locking?

Reduced integration uses fewer points than full, such as one point for a Q4 or 2 × 2 for a Q8. It is cheaper and often more accurate, because fully integrated linear quads in bending pick up spurious shear strain and become far too stiff: shear locking. The danger is the opposite: with one point, some deformation patterns produce zero strain at that point, so they cost no energy. These zero-energy hourglass modes make the mesh zig-zag. Explicit crash codes use one-point elements for speed and add hourglass control; always check the hourglass energy stays a small fraction of the internal energy.

Predict, then check

What is the fewest Gauss points that integrate ξ⁵ + ξ⁴ exactly over [−1, 1]?

Worked examples

One, two and three points on a quartic · I = ∫ (3ξ⁴ + 2ξ² − ξ + 1) dξ from −1 to 1
  1. Exact: 3 × 2/5 + 2 × 2/3 + 0 + 2 = 4.5333
  2. 1 point (ξ = 0, w = 2): 2 × f(0) = 2.0000
  3. 2 points (±0.57735, w = 1): f(±1/√3) = 2 ∓ 0.57735 → sum 4.0000, error −11.8%
  4. 3 points: (5/9)(f(−√0.6) + f(√0.6)) + (8/9) f(0) = (5/9)(6.56) + 8/9 = 4.5333

Answer: Degree 4 needs 2n − 1 ≥ 4, so 3 points give the exact 4.5333; 2 points miss by 11.8%

Extension of a conical steel pin · Solid round bar tapering from D1 = 20 mm to D2 = 10 mm over L = 200 mm, axial load P = 10 kN, E = 2,00,000 MPa (round illustrative steel value). δ = (P/E) ∫ dx/A(x)
  1. Exact: δ = 4PL/(πE D1 D2) = 4 × 10,000 × 200/(π × 2,00,000 × 20 × 10) = 0.06366 mm
  2. Map x = 100(1 + ξ), dx = 100 dξ; 1/A is not a polynomial in ξ, so no rule is exact
  3. 1 point (D = 15 mm at mid-length): 0.05659 mm, error −11.1%
  4. 2 points: 0.06329 mm (−0.59%); 3 points: 0.06365 mm (−0.025%)

Answer: δ = 0.0637 mm; 2 Gauss points are within 0.6% and 3 within 0.03%

Second moment of area over a trapezoidal element · Q4 with nodes (0, 0), (60, 0), (50, 40), (10, 40) mm. Find Ix = ∫∫ y² dA = ∫∫ y(ξ, η)² det J dξ dη
  1. Exact, by strips: width 60 − y/2, Ix = ∫₀⁴⁰ y²(60 − y/2) dy = 9,60,000 mm⁴
  2. y = 20(1 + η) does not depend on ξ, and det J = 500 − 100η here, so the integrand is a cubic in η: 2 points per direction are enough
  3. 2 × 2 Gauss: 9,60,000 mm⁴ (exact); 3 × 3 adds nothing
  4. 1 point: y = 20 mm at the centre × area 2,000 mm² = 8,00,000 mm⁴: one sample cannot see how y² grows across the element

Answer: Ix = 9,60,000 mm⁴ with 2 × 2 points; the 1-point rule gives 8,00,000 mm⁴, 17% low

Chapter 16

Meshing and element quality: aspect ratio, skew, Jacobian, symmetry and mesh independence

Which syllabus covers thisAU not in syllabusVTU not in syllabusSPPU 302050 Unit 2MU MEC504 Module 4KTU MET433 Module 5

How do you choose the elements and the mesh density?

Match the element to the physics: beams for slender frames, shells for sheet metal and thin castings, solids for chunky parts. In solids, hexahedra give more accuracy per node, but tetrahedra mesh any CAD shape automatically; use quadratic (10-node) tets, since linear tets are far too stiff. Put small elements where stress changes fast, at fillets, holes and contact edges, and large ones elsewhere. A common rule of thumb (typical, not a law) is at least 3 quadratic elements across a fillet or through a thickness in bending. Grade sizes smoothly between regions.

How does symmetry shrink a model?

If the geometry, material, loads and supports are all mirror-symmetric about a plane, model one side and replace the other with a boundary condition: zero displacement normal to the plane and zero rotation about the two in-plane axes for shells and beams. A plate with a central hole under tension needs only a quarter model: four times fewer elements, or a finer mesh for the same cost. Axisymmetry goes further and reduces a 3D body to its 2D section. Do not use symmetry for buckling or vibration modes, which can be unsymmetric.

Which element-quality checks matter, and what limits are used?

Definitions follow Altair HyperMesh's help. Aspect ratio: longest edge over the shortest edge or height, "should rarely exceed 5:1". Skew: how far the lines joining opposite mid-sides are from 90°. Jacobian ratio: min/max det J at the Gauss points, 0.7 and above generally acceptable. Warpage: angle between the two triangles a diagonal splits a quad into, up to 5°. Taper: how unequal the corner triangles are. Min/max interior angles and tetra collapse complete the list. Limits on angles and skew vary between companies: treat 45-135° for quads as illustrative.

Element quality: aspect ratio, skew, angles, Jacobian ratio and warpage against typical limits: interactive loads as you scroll

How do you prove the answer does not depend on the mesh?

Refine and re-solve. h-refinement makes elements smaller; p-refinement raises their polynomial order. Track the quantity you will report, such as peak stress at a fillet or a natural frequency, over three or more meshes, each about twice as fine. Stop when the change between the last two falls below a chosen tolerance, typically 2-5%. Small change is not the same as small error: with a known convergence rate, Richardson extrapolation estimates the converged value. A stress that keeps rising with every refinement is a singularity, such as a sharp corner or point load, not a result.

How are bolts and welds represented in a mesh?

Rarely in full detail. A bolt is often a beam element joining two spider patches of rigid (RBE2-type) or averaging (RBE3-type) links on the hole edges, with pretension if needed; a detailed solid bolt with contact is kept for the critical joint. Spot welds become short beams or small solid hex clusters between shell flanges; seam welds become shared nodes or a row of shell or solid elements along the weld line. The aim is the right stiffness and a clean force path, then local detail where the joint itself must be assessed.

Predict, then check

A quarter model of a plate with a central hole, loaded along x. What boundary condition goes on the cut edge lying along the y-axis (x = 0)?

Worked examples

Quality report for one quad · Shell quad with nodes (0, 0), (30, 0), (34, 12), (2, 10) mm. Use the HyperMesh definitions
  1. Edges 30.00, 12.65, 32.06, 10.20 mm; the minimal height (shortest of 4 edges and 8 corner-to-opposite-leg distances) is 9.86 mm
  2. Aspect ratio = 32.06/9.86 = 3.25 (limit 5)
  3. Interior angles 78.7, 108.4, 68.0, 104.9°: min 68.0°, max 108.4°
  4. Skew: the mid-side lines meet at 72.9°, skew = 90 − 72.9 = 17.1°
  5. det J at the 2 × 2 Gauss points 79.0 to 90.0: Jacobian ratio 0.88 (limit 0.7)
  6. Taper: corner triangles 150, 180, 188, 158 mm² against half the area 169 mm²: taper = 1 − 150/169 = 0.112

Answer: AR 3.25, skew 17.1°, angles 68-108°, Jacobian 0.88, taper 0.11: a usable element

A mesh-convergence study that stops too early · Bar fixed at one end carrying a uniform axial load q = 2 N/mm along L = 1,000 mm (like friction along a rock bolt), A = 100 mm². Report the root stress from linear elements, n = 2, 4, 8, 16, 32; stop at < 2% change
  1. Exact root stress qL/A = 20 MPa
  2. FE (consistent nodal loads, solved for each n): the first element's stress n = 2: 15.0000, n = 4: 17.5000, n = 8: 18.7500, n = 16: 19.3750, n = 32: 19.6875 MPa
  3. Change from the previous mesh: 14.3%, 6.7%, 3.2%, 1.6%
  4. The < 2% rule stops at n = 32, still 1.6% low: element stress is the average over the element, error ∝ h
  5. Richardson with error ∝ h: 2 × 19.6875 − 19.3750 = 20.000 MPa

Answer: Converged by the 2% rule at n = 32 (19.69 MPa); extrapolation recovers 20.0 MPa. A small change between meshes is not a small error

Warpage of a shell quad on a curved panel · 20 × 20 mm shell quad; nodes 1, 2, 4 in a plane, node 3 lifted 0.8 mm (case A) or 2.0 mm (case B)
  1. Split along diagonal 1-3: normals of triangles (1, 2, 3) and (1, 3, 4) are (0, −16, 400) and (−16, 0, 400) for case A
  2. cos θ = 1,60,000/1,60,256 → θ = 3.24°; the other diagonal gives 3.24°
  3. Case A warpage = 3.24° (passes 5°); case B = 8.07° (fails)

Answer: 3.2° and 8.1°: a 2 mm lift on a 20 mm element breaks the 5° guidance, so mesh the curved panel finer

Chapter 17

Heat transfer by FEM: composite walls and fins

Which syllabus covers thisAU not in syllabusVTU BME701 Module 5SPPU not in syllabusMU MEC504 Module 3KTU MET433 Module 5

How does a bar element become a heat conduction element?

Steady 1D conduction, d/dx(kA dT/dx) = 0, has the same form as an axial bar, d/dx(EA du/dx) = 0. Swap displacement for temperature, EA for kA and force for heat flow, and the element matrix is the bar's, (kA/L)[1 −1; −1 1], now called a conductance matrix. Assembly, boundary conditions and solution do not change. A prescribed temperature is an essential condition, like a fixed support; a prescribed heat flux or a convecting surface is natural and enters the load vector. The 'reaction' at a node held at a fixed temperature is the heat flowing in there.

How is a composite wall with convection on both faces modelled?

One element per layer is enough: with no heat generated inside, the temperature in each layer is exactly linear, so the nodal temperatures come out exact. Convection from a fluid at T∞ through a film coefficient h acts like a spring to ground: add hA to the diagonal of the surface node and hA T∞ to its load. In a cold-store wall of plaster, dense brick and polyurethane foam (worked below), the 75 mm of foam carries 87% of the total resistance, and the FE heat flow equals the resistance-network answer, 12.5 W/m².

What does a fin element add?

A fin also loses heat from its sides. Over an element of perimeter P and length L, the convection term hP(T − T∞) adds (hPL/6)[2 1; 1 2] to the conductance matrix and hPLT∞/2 to each node's load, the same weighting as a consistent mass matrix. A convective tip adds hA at the last node. Fix the base temperature, solve, and the base reaction is the heat the fin sheds. Inside the FE solution energy balances exactly: that reaction equals the convection summed over the elements and the tip. Try one to ten elements against the exact fin.

Pin fin by FEM: temperatures and heat loss from 1 to 10 elements against the exact fin solution: interactive loads as you scroll

How accurate is a coarse fin mesh, and which way is it wrong?

For a 6 mm carbon-steel pin 60 mm long in air at h = 20 W/m²K (mL = 0.94), one element over-predicts the heat loss by 6.1%, two by 1.5%, four by 0.37%: the error falls about four times each time the elements halve, the h² rate of linear elements. It is always high here: with the base temperature fixed, a restricted temperature shape behaves like a stiffer path and carries more heat. The exact cosh fin solution, built in the Heat and Mass Transfer book, exists only for uniform fins; FE handles tapered fins, varying h and 3D heat sinks the same way.

Predict, then check

A pin fin is modelled with one linear element. Compared with the exact fin, the FE heat loss is:

Worked examples

Cold-store wall, three layers, convection on both faces · Per m² of wall: sand plaster 15 mm (k = 0.71 W/mK), dense brick 230 mm (1.31), polyurethane foam 75 mm (0.03); outside air 38 °C with h = 15 W/m²K, store air 2 °C with h = 8 W/m²K (h values and temperatures illustrative). One element per layer, nodes 1-4 from outside in
  1. Conductances k/L: 47.33, 5.696, 0.400 W/K
  2. [K] = [62.33 −47.33 0 0; −47.33 53.03 −5.696 0; 0 −5.696 6.096 −0.400; 0 0 −0.400 8.400] W/K (h added at nodes 1 and 4)
  3. {F} = [15 × 38, 0, 0, 8 × 2] = [570, 0, 0, 16] W
  4. Solve: T = 37.17, 36.91, 34.72, 3.56 °C
  5. Heat flow: 15 × (38 − 37.17) = 12.46 W; check: R = 1/15 + 0.015/0.71 + 0.23/1.31 + 0.075/0.03 + 1/8 = 2.888 m²K/W and 36/2.888 = 12.46 W/m²

Answer: 12.5 W/m² into the store; the foam takes 31.2 °C of the 36 °C drop and the inner face sits at 3.6 °C

Steel pin fin with two elements · Carbon-steel pin (k = 54 W/mK), D = 6 mm, L = 60 mm, h = 20 W/m²K, base 100 °C, air 30 °C (illustrative), tip insulated; two elements of 30 mm
  1. A = 28.27 mm², P = 18.85 mm; kA/Le = 0.05089 W/K, hPLe = 0.01131 W/K
  2. Element matrix kA/Le [1 −1; −1 1] + hPLe/6 [2 1; 1 2] = [0.05466 −0.04901; −0.04901 0.05466] W/K; load hPLe × 30/2 = 0.1696 W per node
  3. With T1 = 100 °C: 0.10933 T2 − 0.04901 T3 = 0.3393 + 4.901; −0.04901 T2 + 0.05466 T3 = 0.1696
  4. T2 = 82.47 °C, T3 = 77.04 °C
  5. Heat loss = base reaction = 0.05466 × 100 − 0.04901 × 82.47 − 0.1696 = 1.2552 W
  6. Exact: m = √(hP/kA) = 15.71 1/m, Q = √(hPkA) × 70 × tanh 0.943 = 1.2369 W, tip 77.35 °C

Answer: FE 1.255 W against 1.237 W exact (+1.5%); tip 77.04 °C against 77.35 °C

Energy balance and convergence of the same fin · The fin above, solved with 1, 2, 4 and 8 elements
  1. Energy check for two elements: Σ hPLe (θi + θj)/2 = 0.01131/2 × (70 + 52.47) + 0.01131/2 × (52.47 + 47.04) = 1.2552 W, equal to the base reaction
  2. Heat-loss error: n = 1: +6.07%, n = 2: +1.48%, n = 4: +0.37%, n = 8: +0.092%
  3. Ratios 4.10, 4.02, 4.01: halving the element size divides the error by about 4

Answer: The error goes as h² and is always on the high side; two elements already land within 1.5%

Chapter 18

Dynamic analysis: lumped and consistent mass, natural frequencies and mode shapes

Which syllabus covers thisAU CME367 Unit IVVTU BME701 Module 5SPPU 302050 Unit 5MU MEC504 Module 6KTU MET433 Module 5

Where do natural frequencies come from in FEM?

Drop the loads and keep inertia: M ü + K u = 0. Try a motion in which every node moves in step, u = φ sin ωt, and the equation becomes (K − ω²M)φ = 0. A non-zero φ needs det(K − ω²M) = 0, an eigenvalue problem with one root per free degree of freedom. Each ω is a natural frequency (f = ω/2π in Hz) and each φ its mode shape: a pattern of relative motion, not an amplitude. Apply the supports first; an unsupported body has zero frequencies, one per rigid-body motion.

Lumped or consistent mass?

Lumped mass puts half of each element's mass ρAL on each node: a diagonal matrix, cheap, and what explicit codes use. Consistent mass uses the same shape functions as the stiffness, giving (ρAL/6)[2 1; 1 2]. Consistent mass is a Rayleigh-Ritz model, so its frequencies are upper bounds; for a uniform bar of linear elements, lumped mass lands below. A 1 m steel bar fixed at one end has f1 = 1,262 Hz; one element gives 1,391 Hz consistent (+10.3%) and 1,136 Hz lumped (−10.0%). With ten elements both are within 0.1%.

Natural frequencies of a bar: lumped against consistent mass and the exact modes: interactive loads as you scroll

What is a mode shape, and how is it scaled?

A mode shape fixes only the ratios between nodal motions, so it has to be scaled. Scaling the largest value to 1 suits plots. Mass normalisation, φᵀMφ = 1, suits analysis: then φᵢᵀKφᵢ = ωᵢ², and different modes are orthogonal through both M and K, which modal superposition relies on. The k-th mode of a bar has k − 1 still points between the supports. Shape matters as well as length: a 1 m steel bar whose outer half has half the area has f1 = 1,535 Hz, 22% above the uniform bar, because mass is removed where the motion is largest.

How many modes can you trust, and what about beams?

With n elements you get n frequencies, but only the lower ones are accurate. For a fixed-free bar of ten consistent-mass elements the error is 0.1% in mode 1, 2.6% in mode 3, 8.4% in mode 5 and above 12% from mode 6 on. A common rule of thumb is to trust about the lower half of the spectrum and refine until the modes you need stop changing. Beam elements use a 4×4 consistent mass built from the Hermite shape functions, (ρAL/420)[156 22L 54 −13L; …]. Check beam modes for five support types with Skill-Lync's free beam natural frequency calculator (linked under Related at the end of this book).

Predict, then check

A uniform bar is meshed with consistent mass. The FE fundamental frequency will be:

Worked examples

Fixed-free steel bar with one and two elements · Steel bar, L = 1 m, fixed at x = 0, free at x = L; E = 200 GPa, ρ = 7,850 kg/m³ (SI units: m, kg, N). The area cancels
  1. c = √(E/ρ) = 5,048 m/s; exact f1 = c/4L = 1,262 Hz, f2 = 3c/4L = 3,786 Hz
  2. One element: K = EA/L; consistent M = ρAL/3 (free node), so ω² = 3c²/L² and f1 = 1,391 Hz; lumped M = ρAL/2, ω² = 2c²/L², f1 = 1,136 Hz
  3. Two elements (Le = 0.5 m): K = (EA/Le)[2 −1; −1 1], consistent M = (ρALe/6)[4 1; 1 2], lumped M = (ρALe/2)[2 0; 0 1]
  4. det(K − ω²M) = 0: consistent f = 1,295, 4,522 Hz; lumped f = 1,230, 2,969 Hz

Answer: f1 errors: one element +10.3% / −10.0%, two elements +2.6% / −2.6% (consistent / lumped); f2 with two elements is still +19% / −22% out

Stepped steel bar, two consistent elements · Steel bar fixed at the left: 0.5 m of 400 mm² then 0.5 m of 200 mm² to a free end (illustrative sizes); E = 200 GPa, ρ = 7,850 kg/m³; one element per step
  1. k1 = EA1/0.5 = 1.6 × 10⁸ N/m, k2 = 0.8 × 10⁸ N/m; K = 10⁸ × [2.4 −0.8; −0.8 0.8] N/m
  2. m1 = ρA1Le = 1.570 kg, m2 = 0.785 kg; M = [(m1 + m2)/3 m2/6; m2/6 m2/3] = [0.785 0.1308; 0.1308 0.2617] kg
  3. det(K − ω²M) = 0: f1 = 1,594 Hz, f2 = 4,144 Hz
  4. Exact: displacement and force continuous at the step give A1 cot z = A2 tan z with z = βL/2, so tan² z = 2, z = 0.9553, 2.1863; f = 2zc/(2πL) = 1,535, 3,513 Hz

Answer: FE f1 = 1,594 Hz (+3.8%), f2 = 4,144 Hz (+18%): the second mode needs more elements

Fixed-fixed aluminium bar, lumped mass, mass-normalised modes · Aluminium bar 0.6 m long, A = 100 mm², fixed at both ends; E = 69 GPa, ρ = 2,712 kg/m³; three equal elements, lumped mass
  1. k = EA/Le = 3.45 × 10⁷ N/m; each interior node carries ρALe = 0.05424 kg
  2. K = 3.45 × 10⁷ [2 −1; −1 2] N/m, M = 0.05424 [1 0; 0 1] kg; ω² = (k/m)(2 ∓ 1)
  3. ω1 = √(k/m) = 25,220 rad/s, f1 = 4,014 Hz, mode [1, 1]; f2 = √3 f1 = 6,952 Hz, mode [1, −1]
  4. Mass-normalise mode 1: φ = [1, 1]/√(2 × 0.05424) = [3.036, 3.036]; φᵀKφ = 636.1 × 10⁶ = ω1²
  5. Exact: c = 5,044 m/s, f1 = c/2L = 4,203 Hz, f2 = c/L = 8,407 Hz

Answer: Lumped FE 4,014 and 6,952 Hz against 4,203 and 8,407 Hz exact (−4.5% and −17%): both below, as lumped mass on a uniform bar of linear elements always is

Chapter 19

Transient analysis: explicit and implicit time integration, Newmark and crash

Which syllabus covers thisAU CME367 Unit IVVTU not in syllabusSPPU 302050 Units 5, 6MU MEC504 Module 6KTU not in syllabus

When is a transient analysis needed, and which kind?

When the load changes in a time comparable with the structure's natural periods: an impact, a drop test, a crash, a shaker table. If the load rises slowly compared with the first period, a static analysis is enough. Linear problems can use modal superposition: find the first few modes, solve one single-DOF equation per mode and add the responses. Nonlinear problems (contact, plasticity, large deformation) need direct integration of M ü + C u̇ + K u = F, step by step, by an explicit or an implicit method.

Why do explicit crash codes take microsecond time steps?

Central difference finds the next displacement from the current and previous ones using only the mass matrix; with lumped mass that needs no equation solving, so each step is cheap. But it is conditionally stable: Δt must stay below 2/ω_max, and the highest frequency belongs to the smallest element. For bars and shells this is the Courant limit Le/c, the time a stress wave takes to cross the element. Steel with 5 mm elements gives 0.99 μs, so a 100 ms crash needs about 1 lakh steps. Mass scaling adds artificial density to the smallest elements to lift Δt.

Explicit against implicit time integration: the critical time step and when the solution blows up: interactive loads as you scroll

What does Newmark's implicit method buy?

Newmark's average acceleration scheme (β = 1/4, γ = 1/2) takes the acceleration over a step as the mean of its start and end values. For linear problems it is unconditionally stable, so Δt is chosen for accuracy, but every step solves a stiffness-like system. It adds no numerical damping and lengthens the period: by 0.8% at Δt = T/20 and by 40% at Δt = 0.4 T. A common rule of thumb is 20 or more steps per period of the highest mode that matters. Implicit suits vibration and seismic response; explicit suits short, violent events.

How is transient heat conduction stepped in time?

Transient conduction gives C Ṫ + K T = F, first order in time, with a capacitance matrix C built like the mass matrix (ρc in place of ρ). The θ-method blends the two ends of a step: forward Euler (θ = 0) is explicit and, with lumped capacitance, stable only for Δt ≤ Δx²/(2α), α = k/ρc; Crank-Nicolson (θ = 1/2) and backward Euler (θ = 1) are unconditionally stable. The limit scales with Δx², not Δx: refine a steel mesh from 5 to 2.5 mm and the explicit step falls from 0.89 s to 0.22 s, a quarter.

Predict, then check

An explicit crash model's smallest steel element shrinks from 5 mm to 2.5 mm. The stable time step:

Worked examples

Time step for a hatchback crash box · Steel crash box meshed with 5 mm shell elements (illustrative), E = 200 GPa, ρ = 7,850 kg/m³; impact event 100 ms (illustrative); the Courant limit taken as Le/c without a safety factor
  1. c = √(E/ρ) = √(200 × 10⁹/7,850) = 5,048 m/s
  2. Δt_cr = 0.005/5,048 = 0.991 μs; steps for 100 ms = 0.1/Δt = 1,00,951
  3. One badly meshed 2 mm element sets the step for the whole model: Δt = 0.396 μs, 2,52,377 steps (2.5 times the run time)
  4. Mass scaling that element back to 0.99 μs: Δt ∝ √ρ, so its density × (5/2)² = 6.25
  5. An aluminium box would barely change it: c = 5,044 m/s, Δt = 0.991 μs

Answer: About 0.99 μs and 1.01 lakh steps; fix small elements in the mesh before reaching for mass scaling

Central difference against Newmark on a 100 Hz mode · A mode with T = 10 ms (ω = 628.3 rad/s), no damping (illustrative); time steps 4 ms and 0.5 ms
  1. Central difference limit: Δt_cr = 2/ω = T/π = 3.18 ms, so 4 ms is unstable
  2. Ω = ωΔt = 2.513; the recurrence u(n+1) = (2 − Ω²) u(n) − u(n−1) has roots of z² + 4.317 z + 1 = 0, the larger in size z = −4.071: the error multiplies by 4.07 every step
  3. Newmark at 4 ms: stable (|z| = 1), period lengthened by Ω/(2 atan(Ω/2)) = 1.398, +40%
  4. At 0.5 ms (T/20): central difference period × Ω/(2 asin(Ω/2)) = 0.9959 (−0.41%), Newmark × 1.0082 (+0.82%)

Answer: At 4 ms the explicit run blows up and Newmark runs but with a 40% wrong period; at T/20 both are within 1%

Explicit time step for transient conduction in steel · 1D transient conduction in steel: k = 54 W/mK, ρ = 7,850 kg/m³, c = 490 J/kgK; linear elements with lumped capacitance, forward Euler
  1. α = k/(ρc) = 54/(7,850 × 490) = 1.404 × 10⁻⁵ m²/s
  2. Δx = 5 mm: Δt ≤ Δx²/(2α) = 0.890 s
  3. Δx = 2.5 mm: Δt ≤ 0.223 s, a quarter
  4. With consistent capacitance the limit is Δx²/(6α) = 0.297 s at 5 mm, a third of the lumped value

Answer: 0.89 s at 5 mm and 0.22 s at 2.5 mm: in diffusion, refining the mesh costs steps as the square of the refinement

Chapter 20

Nonlinear analysis: types of nonlinearity and the Newton-Raphson method

Which syllabus covers thisAU CME367 Unit IIIVTU not in syllabusSPPU 302050 Unit 5MU not in syllabusKTU not in syllabus

When does an FE problem stop being linear?

A linear analysis assumes [K] does not change as the part deforms, so doubling the load doubles every answer and load cases can be added. That fails in three ways. Geometric nonlinearity: large rotations or deflections change the load paths, as in a fishing rod, a buckling column or a panel that snaps through. Material nonlinearity: the stress-strain curve bends, as in yielding steel, rubber mounts (hyperelastic) or creep. Boundary nonlinearity: contact opens and closes, and friction sticks or slips. In each case the internal force is a nonlinear function F(u), so the solver has to iterate.

How does Newton-Raphson find the equilibrium point?

Equilibrium means the residual R = P − F(u) is zero. Newton-Raphson linearises at the current guess: solve the tangent stiffness K_T Δu = R, update u, recompute F and K_T, repeat. For the hardening spring f = 20u + 4u³ N at 60 N, the first guess 3 mm overshoots to 168 N, then 2.156, 1.850, 1.812 and 1.811 mm follow: five iterations, and near the answer the number of correct digits roughly doubles each time. That is quadratic convergence. Pick the springs below, raise the load and watch the tangents zig-zag onto the curve.

Newton-Raphson for a nonlinear spring: load steps, tangent iterations and convergence: interactive loads as you scroll

Why apply the load in steps, and what is modified Newton-Raphson?

Iterations converge only from a starting point close enough to the answer, so the load is split into increments and each converged state starts the next. Path-dependent materials such as plasticity need small steps anyway, because the answer depends on the history. Modified NR factorises K_T once per step and reuses it: each iteration is far cheaper on a big model, but convergence becomes linear. On the softening spring at 20 N, full NR needs 4 iterations and modified NR 14, each one leaving about 0.40 of the previous error. With a stiffening response the stale tangent can even diverge.

When does the solver decide it has converged?

It compares norms with tolerances: the out-of-balance force against the applied load, and the displacement correction against the total displacement. Ansys Mechanical APDL, for example, uses an L2 norm with default tolerances of 0.5% for force and 5% for displacement. A force check alone can pass a soft structure with a big error, and a displacement check alone can pass a stiff one, so codes use both. If a step will not converge, the usual fixes are smaller load steps (automatic bisection), a line search, or checking the model for unstable rigid-body motion.

What is a limit point, and why does NR fail there?

At a limit point the load-displacement curve peaks: K_T = 0, so Newton's step Δu = R/K_T blows up, and beyond it no nearby equilibrium exists at a higher load. A shallow two-bar steel truss of 1,000 mm half-span and 50 mm rise (100 mm² bars, illustrative) peaks at about 960 N; ask for 1 kN in load control and the apex has to snap through to a far branch. Arc-length methods (Riks, Crisfield) fix this by controlling a combined load-displacement path length, so the load may drop and the solver can follow the curve over the peak. Buckling is the same story.

Predict, then check

A softening spring peaks at 24.3 N. You ask a load-controlled Newton-Raphson solver for 26 N. What happens?

Worked examples

Full Newton-Raphson on a hardening spring · A bump stop modelled as f = 20u + 4u³ (N, u in mm; illustrative). Load P = 60 N in one step from u = 0, stop when |R|/P ≤ 10⁻⁶. Tangent K_T = 20 + 12u²
  1. Iteration 1: K_T = 20 N/mm, Δu = 60/20, so u = 3.000 mm; f(3) = 168 N, R = −108 N (overshoot)
  2. Iteration 2: K_T = 20 + 12 × 9 = 128 N/mm, Δu = −108/128, so u = 2.1562 mm; R = −23.23 N
  3. Iteration 3: u = 1.8498 mm, R = −2.315 N; iteration 4: u = 1.8119 mm, R = −0.0317 N
  4. Iteration 5: u = 1.81137 mm, R ≈ 6 × 10⁻⁶ N: converged. Near the end the number of correct digits roughly doubles each iteration
  5. Check by bisection on f(u) = 60: u = 1.81137 mm. With three load steps of 20 N the same answer takes 11 iterations and the worst overshoot falls from 1.19 to 0.13 mm

Answer: u = 1.811 mm in 5 full-NR iterations

Full against modified Newton-Raphson · Softening spring f = 20u − 2u³ (N, mm; illustrative), P = 20 N from u = 0, tolerance |R|/P ≤ 10⁻⁶. Modified NR keeps K₀ = 20 N/mm
  1. Limit point: K_T = 20 − 6u² = 0 at u = 1.826 mm, P = 24.34 N, so 20 N is on the rising branch
  2. Full NR: u = 1, 1.1429, 1.1534, 1.15347 mm: 4 iterations
  3. Modified NR: u = 1, 1.1, 1.1331, … each step uses 20 N/mm: 14 iterations
  4. At the answer K_T = 12.02 N/mm, so each modified NR iteration multiplies the error by 1 − 12.02/20 = 0.40

Answer: u = 1.1535 mm; full NR 4 iterations, modified NR 14 (each one cheaper)

Limit load of a shallow two-bar truss · Two steel bars (E = 200 GPa, A = 100 mm²) from supports 2,000 mm apart rise 50 mm to a loaded apex (illustrative). Exact geometry, axial force from the engineering strain
  1. L₀ = √(1,000² + 50²) = 1,001.25 mm; vertical load P = 2N(h − w)/L, N = EA(L₀ − L)/L₀
  2. Limit point where dP/dw = 0: L³ = L₀a², so L = 1,000.42 mm, w = 21.14 mm
  3. P_lim = 959.9 N (shallow formula EA·(2/3√3)·(h/L₀)³ = 958.7 N)
  4. Bar force there 16,639 N, stress 166 MPa: below the 250 MPa yield of ASTM A36 steel, so still elastic
  5. At 1 kN the only equilibrium is the snapped shape at w = 108.0 mm, past 2h = 100 mm

Answer: P_lim ≈ 960 N at w ≈ 21.1 mm; beyond it load control fails and arc-length is needed

Chapter 21

Post-processing and checking results: averaged stresses, errors, singularities and contact

Which syllabus covers thisAU CME367 Unit VVTU BME701 Module 1SPPU 302050 Units 4, 6MU MEC504 Module 4KTU MET433 Module 5

Why do averaged and unaveraged stress plots differ, and which should you trust?

Displacements are continuous across elements, but stresses come from their derivatives, so each element has its own value at a shared node. Unaveraged (element) plots show these steps; averaged (nodal) plots take the mean at each node and look smooth. The size of the step is a free error indicator: a 600 m steel rod hanging under its own weight, in three elements, jumps 15.4 MPa at every interior node, and the top element reads 38.5 MPa against an exact 46.2 MPa. A big difference between the two plots means the mesh is too coarse there, not that one plot is right.

Averaged against unaveraged stresses: element stress jumps as an error indicator: interactive loads as you scroll

Where inside an element is the stress most accurate?

Not at the nodes. Displacement elements give their best derivatives at special interior points, usually the Gauss points: the midpoint of a linear bar, the 2 × 2 points of a Q4. For the hanging rod the element stress equals the exact stress at every midpoint because the stress is linear; with a load that grows towards the tip the stress is a parabola and the midpoint is off by ρgLe²/(12L), 0.43 MPa for the same rod and mesh. Solvers sample stresses at the Gauss points and extrapolate to the nodes, which is why peak nodal stresses on coarse meshes deserve suspicion.

How do you check an FE result and write it up?

Errors come from modelling (wrong geometry, supports, loads or material: the biggest and the hardest to spot), discretisation (mesh too coarse) and numerics (round-off, ill-conditioning from very stiff and very soft parts together). Before believing a contour plot: check the reactions add up to the applied loads, animate the deformed shape and ask whether it moves the way the part would, confirm units (mm, N, MPa, tonne), compare one number with a hand calculation, and run a mesh-convergence check at the critical location. A CAE report states the objective, geometry and simplifications, material, mesh and quality, loads and boundary conditions, these checks, results against the allowable, and conclusions.

Why does the stress at a sharp corner keep rising as you refine the mesh?

Elasticity predicts infinite stress at a sharp re-entrant corner, a point load or a point support. For a 270° inside corner the stress grows as r^(λ − 1) with λ = 0.5445, so every halving of the element size raises the peak by about 37% and it never converges. That number is a property of the mesh, not the part. Report the stress a small distance away, model the real fillet radius, or use a fracture or weld-assessment method built for sharp notches. Spread point loads over a realistic patch.

How do FE codes enforce contact: penalty or Lagrange multipliers?

Contact is a constraint: the gap g ≥ 0, and pressure exists only when g = 0. The penalty method places a very stiff spring kₚ between the surfaces once they touch. It adds no unknowns and keeps the matrix size, but allows a small penetration, and the contact force is short by a fraction k/(k + kₚ); too large a kₚ makes the system ill-conditioned. The Lagrange multiplier method adds the contact force as an extra unknown and enforces zero penetration exactly, at the cost of extra equations and a matrix with zeros on the diagonal. Augmented Lagrange iterates a penalty towards the exact force.

Where else is CAE used beyond static stress?

Durability: stress-life (S-N, Basquin) for long, elastic lives and strain-life (E-N, Coffin-Manson) where local yielding shortens life, with rainflow counting and Miner's rule summing the damage of a load history. NVH: modes and frequency response to keep resonances away from engine orders and road inputs. Crash: explicit dynamics with tiny time steps for crush boxes and occupant safety. Mould-flow simulation of plastic filling, packing and warpage; casting simulation of filling, solidification and shrinkage porosity; sheet-metal forming simulation for thinning, wrinkling and springback. CFD covers fluids and heat. Each is a specialised solver around the same mesh-solve-check loop.

Predict, then check

Refining the mesh at a sharp 270° inside corner from 2 mm to 1 mm to 0.5 mm elements gives peaks of 180, 247 and 338 MPa. What should you report?

Worked examples

Averaged against unaveraged stresses in a hanging rod · Steel rod 600 m long (ρ = 7,850 kg/m³, E = 200 GPa), A = 500 mm² (illustrative), hanging from the top under its own weight; three 200 m linear elements, consistent loads ρgA Le/2 per element end. mm-N-MPa units
  1. ρg = 7,850 × 9.81 = 77,008 N/m³ = 7.70 × 10⁻⁵ N/mm³; weight W = ρgAL = 23,103 N
  2. Element stresses (load below ÷ A): 38.50, 23.10, 7.70 MPa, equal to the exact ρg(L − x) at each midpoint
  3. Averaged nodal stresses: top 38.50, then 30.80, 15.40, tip 7.70 MPa; the two interior values are exact
  4. Jump at each interior node 15.40 MPa = ρg Le; exact top stress 46.21 MPa, so the top element is short by 7.70 MPa, half the jump
  5. Reaction = 23,103 N = weight; tip displacement 69.31 mm, exact at the nodes

Answer: FE peak 38.5 MPa (averaged or not) against exact 46.2 MPa; the 15.4 MPa jump flags it

Penalty against Lagrange multiplier contact · A part modelled as a spring k = 2,000 N/mm is pushed by P = 10 kN towards a rigid stop 2 mm away (illustrative)
  1. Without the stop u = 10,000/2,000 = 5 mm > 2 mm, so contact closes
  2. Lagrange multiplier: u = 2 mm exactly, contact force λ = 10,000 − 2,000 × 2 = 6,000 N
  3. Penalty kₚ = 10⁵ N/mm: (k + kₚ)u = P + kₚ·2 → u = 2.0588 mm, penetration 0.0588 mm, force 5,882 N (1.96% low)
  4. Penalty kₚ = 10⁷ N/mm: penetration 0.60 µm, force 5,998.8 N (0.020% low); the error is k/(k + kₚ)

Answer: Lagrange: 6,000 N, zero penetration; penalty: 5,882 N at 10⁵ and 5,999 N at 10⁷ N/mm

Is the peak stress converging? · An L-bracket meshed with 2, 1 and 0.5 mm elements at its inside corner (illustrative results). Sharp corner: peak 180 MPa at 2 mm. With a 2 mm fillet: 212.0, 219.0 and 220.8 MPa
  1. Sharp 270° corner: λ = 0.5445 (Williams' equation λ = sin(3πλ/2) re-solved: 0.5445); each halving multiplies the peak by 2^(1 − λ) = 1.371
  2. So the sharp corner reads 180, 247, 338 MPa: growing without limit
  3. Fillet: changes 7.0 then 1.8 MPa; observed order p = log₂(7.0/1.8) = 1.96
  4. Richardson estimate 220.8 + 1.8/(2^p − 1) = 221.4 MPa; last change 0.8% (below a typical 2-5% stopping rule)

Answer: Sharp corner: a singularity, do not report it. Fillet: converged at about 221 MPa

Keep going

Recommended reading

  • Introduction to Finite Elements in Engineering, T. R. Chandrupatla, A. D. Belegundu
  • A First Course in the Finite Element Method, D. L. Logan
  • Textbook of Finite Element Analysis, P. Seshu
  • An Introduction to the Finite Element Method, J. N. Reddy
  • Concepts and Applications of Finite Element Analysis, R. D. Cook, D. S. Malkus, M. E. Plesha, R. J. Witt
  • Finite Element Procedures, K.-J. Bathe
  • Practical Finite Element Analysis, N. S. Gokhale, S. S. Deshpande, S. V. Bedekar, A. N. Thite

How this book was made

Chapters follow the official syllabi listed above. Every interactive's formulas and every worked-example number were checked by script. Explanations, animations and examples are original to Skill-Lync. Topics informed by MIT OpenCourseWare 2.092 (Finite Element Analysis of Solids and Fluids I), CC BY-NC-SA. All explanations, animations and examples are original to Skill-Lync; MIT does not endorse this page.

From the exam to a core job

Talk to a counsellor.

Ask how CAE engineers use finite element analysis on real projects, and what the PG Program in CAE (FEA) covers.

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.

Talk to a career counsellor

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.