Computational Fluid Dynamics

Introduction and Context

Computational Fluid Dynamics (CFD) is the numerical study of fluid motion, heat transfer, mass transfer, and related transport phenomena. It converts the governing conservation laws of fluid mechanics into algebraic equations that can be solved on a computer. CFD is therefore not a replacement for fluid mechanics; it is a methodology that combines physical modelling, mathematical discretisation, numerical algorithms, programming, and engineering interpretation.

CFD is especially important when analytical solutions are unavailable or experiments are expensive, hazardous, or incapable of resolving the required details. It is used in turbomachinery, internal combustion engines, aerospace vehicles, process equipment, biomedical flows, environmental engineering, microfluidics, and renewable-energy systems. At postgraduate level, the central question is not merely how to operate a solver, but whether a computed solution is physically meaningful, numerically converged, and sufficiently verified and validated for its intended use.

Learning Objectives

After studying this chapter, the reader should be able to:

1. formulate the governing equations for computational fluid-flow problems;
2. distinguish modelling, discretisation, iterative convergence, verification, and validation;
3. explain finite-difference, finite-volume, and finite-element approaches;
4. analyse stability, consistency, conservation, boundedness, and numerical diffusion;
5. select appropriate pressure–velocity coupling and turbulence models;
6. construct a defensible CFD workflow and assess uncertainty;
7. interpret CFD results critically in engineering design and research.

1. Mathematical Foundation

1.1 Conservation laws

For a continuum fluid, the local conservation of mass is

where ρ is density (kg m⁻³), t is time (s), and u is the velocity vector (m s⁻¹). For an incompressible fluid of constant density, this reduces to

The Cauchy momentum equation is

where p is pressure (Pa), τ is the viscous stress tensor (Pa), and f is body force per unit mass (m s⁻²). For a Newtonian fluid,

where μ is dynamic viscosity (Pa s), I is the identity tensor, and the final term accounts for volumetric deformation under the Stokes hypothesis. In an incompressible flow with constant μ, the momentum equation becomes

The substantial derivative, D/Dt = ∂/∂t + u·∇, separates local temporal change from convection.

A general scalar transport equation is

where φ is a transported scalar, Γ is its diffusion coefficient, and Sφ is a volumetric source. Temperature, species concentration, and turbulence variables can often be represented in this form. The equation is valid when the relevant transport mechanisms can be represented by convection, diffusion, and source terms.

1.2 Energy and species equations

For a calorically perfect fluid, a commonly used total-energy equation is

where E is total specific energy (J kg⁻¹), k is thermal conductivity (W m⁻¹ K⁻¹), T is temperature (K), and S_E represents additional energy sources. The exact form depends on whether viscous work, pressure work, radiation, chemical reaction, and compressibility are included.

For a species mass fraction Yᵢ,

where Dᵢ is the mass-diffusion coefficient (m² s⁻¹) and Rᵢ is the net production rate (kg m⁻³ s⁻¹). The mass fractions must satisfy ∑ᵢYᵢ = 1.

1.3 Dimensionless parameters

Dimensional analysis identifies dominant physical mechanisms and supports model selection. Important dimensionless groups include

the Reynolds number, comparing inertia with viscous effects; Ma = U/a, the Mach number, comparing flow speed U with speed of sound a; and

the Prandtl number, comparing momentum and thermal diffusion. Here L is a characteristic length, ν is kinematic viscosity (m² s⁻¹), and cₚ is specific heat at constant pressure (J kg⁻¹ K⁻¹). For buoyancy flows, the Grashof and Rayleigh numbers may determine whether natural convection is laminar or turbulent. These groups guide mesh requirements, time-step selection, and turbulence or compressibility modelling.

2. From a Continuous Problem to a Discrete Problem

A CFD problem consists of a domain, governing equations, initial conditions, boundary conditions, material properties, and often a constitutive or turbulence model. The continuous equations have infinitely many degrees of freedom; a computer requires a finite set of unknowns.

2.1 Meshes and control volumes

The computational domain is divided into cells or elements. A mesh may be structured, unstructured, block-structured, or hybrid. Structured meshes provide regular neighbour relationships and can be efficient, whereas unstructured meshes accommodate complex geometry more readily. Mesh quality is described by skewness, non-orthogonality, aspect ratio, smoothness, and cell volume. Poor quality can increase truncation error and impair convergence even when the nominal cell count is large.

A finite-volume method integrates the transport equation over a control volume V:

where A is the control-volume boundary, n is the outward unit normal, and dA is an area element. Applying the divergence theorem converts volume fluxes into surface fluxes. This formulation is attractive because conservation is enforced over each cell and, when internal face fluxes cancel pairwise, over the entire domain.

2.2 Finite differences

Finite-difference methods approximate derivatives at grid points. For a uniform one-dimensional grid with spacing ∆x,

is a second-order central approximation, while

is a first-order backward approximation. Finite differences are conceptually simple and effective on regular grids, but complex geometries and strict conservation can be more difficult to handle.

2.3 Finite elements

Finite-element methods approximate a field using basis functions, φ ≈ ∑ⱼNⱼφⱼ, and derive a weighted-residual or weak form. They are powerful for irregular domains, coupled multiphysics, and higher-order approximation. Stabilisation is often required for advection-dominated flows, because a straightforward Galerkin formulation may produce oscillatory solutions.

2.4 Discrete algebraic system

After spatial discretisation, a steady problem usually has the form

where A is the coefficient matrix, Φ is the vector of unknowns, and b contains source and boundary contributions. For nonlinear flow equations, A depends on Φ, so the system is solved iteratively. A transient discretisation produces a system at each time level, for example

where V is cell volume, Ff is mass flux through face f, Df represents diffusive conductance, and superscripts denote time levels. The precise coefficients depend on interpolation and time-integration schemes.

3. Numerical Properties and Discretisation Choices

3.1 Consistency, stability, convergence, and conservation

A discretisation is consistent if its truncation error approaches zero as grid spacing and time step approach zero. It is stable if errors do not grow without bound under the specified algorithm and time-step restrictions. A convergent method approaches the solution of the continuous problem as the discretisation is refined. For linear well-posed problems, the Lax equivalence theorem relates consistency and stability to convergence, but nonlinear CFD systems and practical boundary treatments require broader analysis.

Conservation means that the discrete change in a conserved quantity equals the net boundary flux plus sources. Boundedness requires that numerical values do not generate unphysical overshoots or undershoots. A scheme can be formally high-order yet produce unacceptable oscillations near shocks or steep scalar gradients if boundedness is not controlled.

3.2 Convection schemes

First-order upwind interpolation uses the upstream value at a face. It is robust and bounded in many circumstances but introduces numerical diffusion, which smooths shear layers and suppresses resolved fluctuations. Central differencing is second-order on uniform grids and has low numerical diffusion, but it may oscillate when convection dominates diffusion. Higher-order upwind, QUICK, flux-limited, and total-variation-diminishing schemes seek a compromise between accuracy and boundedness.

For a one-dimensional steady convection–diffusion equation with constant velocity U and diffusivity Γ, the cell Peclet number is

where ∆x is the cell size. Large |Pe₍c₎| indicates convection dominance and increases sensitivity to the convection scheme. This local numerical quantity should not be confused with a domain-scale physical Peclet number.

3.3 Time integration

The explicit Euler update is

where R is the semi-discrete right-hand side. It is simple but conditionally stable. Implicit Euler evaluates the residual at the new time level and is more stable for stiff diffusion problems, though it is only first-order accurate in time. The second-order backward differentiation formula is more accurate for smooth transient flows but can be less forgiving during abrupt start-up. Stability does not guarantee accuracy: an excessively large time step can yield a converged but temporally under-resolved solution.

The Courant number is

for a one-dimensional characteristic velocity U. Explicit advection schemes commonly require a scheme-dependent upper bound on Co. Implicit schemes may tolerate larger values, but temporal and convective accuracy still impose practical limits.

4. Pressure–Velocity Coupling

In incompressible flow, pressure has no independent evolution equation. It acts as a Lagrange multiplier enforcing ∇·u = 0. A velocity field predicted from the momentum equations generally has non-zero mass imbalance; a pressure-correction equation is therefore derived from continuity and the discretised momentum equations.

The SIMPLE family of algorithms performs a guessed-pressure velocity solution, estimates face fluxes, solves a pressure-correction equation, and updates pressure, velocity, and mass fluxes. Under-relaxation improves robustness but slows convergence if chosen too conservatively. PISO performs multiple corrections within a time step and is often effective for transient problems. Coupled algorithms solve pressure and momentum more simultaneously, increasing memory requirements but sometimes improving convergence for strongly coupled flows.

A collocated arrangement stores pressure and velocity at cell centres. Without special treatment, pressure–velocity decoupling can produce a checkerboard pressure field. Rhie–Chow-type momentum interpolation or an equivalent face-flux formulation prevents this nonphysical mode. Staggered grids place velocity components on faces and naturally couple pressure and velocity, but they can complicate irregular geometries.

5. Turbulence and Multiphysics Modelling

5.1 Reynolds averaging

For turbulent flow, a variable is decomposed as φ = φ̄ + φ′, where the overbar denotes a time or ensemble average and the prime denotes a fluctuation. Averaging the Navier–Stokes equations introduces Reynolds stresses:

These six apparent stresses create the closure problem. A common eddy-viscosity hypothesis models them as

where μt is turbulent viscosity, S̄ᵢⱼ is mean strain rate, k is turbulent kinetic energy, and δᵢⱼ is the Kronecker delta. Two-equation models such as k–ε and k–ω provide transport equations for turbulence scales. The standard k–ε model is economical and often effective for free shear flows, while k–ω and SST variants generally offer better near-wall behaviour and adverse-pressure-gradient performance.

RANS models solve mean quantities and are comparatively inexpensive. Large-eddy simulation (LES) resolves large turbulent structures and models smaller scales; it requires substantially finer meshes and smaller time steps, particularly near walls. Direct numerical simulation resolves all relevant scales and is generally restricted to low or moderate Reynolds numbers and canonical research problems.

5.2 Wall treatment

The non-dimensional wall coordinate is

where y is the distance from the wall and uτ = √(τw/ρ) is friction velocity. Wall functions typically require a logarithmic-layer placement, often y⁺ of order 30 or greater, whereas low-Reynolds-number or wall-resolved approaches seek y⁺ near unity. Mixing incompatible wall functions and mesh resolution can create large errors in wall shear and heat transfer.

5.3 Compressibility, combustion, and multiphase flow

Compressible solvers must account for density variation, acoustic waves, and an equation of state, such as p = ρRT for an ideal gas, where R is the specific gas constant. Shock-capturing methods require numerical dissipation and careful boundary conditions. Combustion adds chemical kinetics, turbulent mixing, radiation, and stiffness. Multiphase calculations require a choice among Eulerian–Eulerian, Eulerian–Lagrangian, volume-of-fluid, level-set, or mixture descriptions. No method is universally superior; the appropriate model depends on interface topology, phase loading, density ratio, and required outputs.

6. Boundary Conditions and Solver Setup

Boundary conditions must correspond to the physics and mathematical character of the equations. Typical conditions include:

• no-slip wall: u = 0;
• prescribed velocity or mass flow at an inlet;
• prescribed static or total pressure at an outlet, when physically justified;
• symmetry: zero normal velocity and zero normal normal-gradient of appropriate variables;
• periodicity for repeating geometries;
• specified temperature, heat flux, or convective thermal condition.

Over-specification can make a problem ill-posed, while an outlet placed too close to recirculation can contaminate the solution. Backflow treatment at pressure outlets must be physically plausible. For external aerodynamics, far-field boundaries should be sufficiently distant or use suitable non-reflecting conditions.

Material properties may be constant, temperature-dependent, pressure-dependent, or composition-dependent. Property correlations should be documented, with valid temperature and pressure ranges. Units must be consistent throughout; a common failure is mixing gauge pressure with absolute pressure in compressible calculations.

7. Verification, Validation, and Uncertainty

Verification asks, “Is the numerical model solved correctly?” Validation asks, “Does the model represent the real physical system adequately?” They are distinct. A solution can be numerically converged but physically inaccurate because of an inappropriate turbulence model or missing physics.

7.1 Iterative convergence

A typical residual for equation i is a norm of the algebraic imbalance, for example

Residual reduction is useful but insufficient. Engineering monitors such as drag, pressure drop, mass imbalance, heat-transfer rate, and integral forces should also become stable. In a steady calculation, convergence should be assessed against changes in the solution and output quantities, not a universal residual threshold.

7.2 Grid and time-step studies

A grid study compares a quantity of interest Q on systematically refined meshes. If three solutions are available and the refinement ratio is r, an estimated observed order may be obtained from

provided the solutions are in the asymptotic range and the ordering is consistent. Here Q₁, Q₂, and Q₃ correspond to successively refined meshes in a clearly stated order. Richardson extrapolation can estimate a zero-grid-spacing value, but it should not be treated as reliable outside the asymptotic range.

For a transient calculation, repeat the simulation with a smaller ∆t and compare phase, amplitude, mean values, and spectra where relevant. A time-step study is essential for unsteady separation, vortex shedding, acoustics, and reacting flows.

7.3 Validation and uncertainty

Validation compares predictions with experimental measurements or trusted benchmark solutions using matched definitions, boundary conditions, and uncertainty estimates. A useful normalised error is

where Q_CFD is the computed quantity and Q_ref is the reference value. This is not a universal acceptance criterion; tolerable error depends on the engineering decision and measurement uncertainty.

Verification and validation should report mesh topology, cell count, y⁺ distribution, discretisation schemes, convergence criteria, physical models, boundary conditions, and sensitivity studies. Model-form uncertainty, input uncertainty, discretisation uncertainty, and experimental uncertainty should be distinguished rather than hidden in a single unexplained error percentage.

8. A Defensible CFD Workflow

A professional workflow is iterative rather than purely sequential:

1. Define the question. Identify the output quantity, accuracy requirement, relevant time scales, and decision to be supported.
2. Select the physical model. Decide whether the flow is incompressible or compressible, laminar or turbulent, single-phase or multiphase, steady or transient, and whether heat transfer or reaction matters.
3. Prepare geometry and domain. Remove irrelevant details, retain flow-critical features, and place boundaries far enough away.
4. Generate and inspect the mesh. Resolve boundary layers, wakes, jets, shocks, interfaces, and geometric curvature. Check quality metrics and local refinement.
5. Specify physics and boundary conditions. Use dimensional consistency and documented property data.
6. Choose numerical schemes and initialise. Start robustly if necessary, then use higher-order schemes after the flow field is reasonably developed.
7. Solve and monitor. Track residuals, mass conservation, forces, fluxes, and physically meaningful probes.
8. Verify. Perform grid, time-step, iterative, and model-sensitivity studies.
9. Validate. Compare with experiments, analytical solutions, or benchmark data.
10. Report uncertainty and interpret. Present contours together with quantitative values, scales, averages, and limitations.

Post-processing must avoid misleading visualisation. A contour plot can conceal poor scales, clipped extrema, or non-converged regions. Streamlines show paths of a steady vector field, not necessarily trajectories in an unsteady flow. Vorticity magnitude is not automatically a measure of turbulence or coherent structure. Integral quantities and uncertainty bounds are usually more useful for design decisions than attractive images.

9. Worked Example: Laminar Flow in a Circular Tube

Consider water at 20 °C flowing steadily through a smooth circular tube of diameter D = 0.020 m. Let the mean velocity be U = 0.10 m s⁻¹, density ρ = 998 kg m⁻³, and dynamic viscosity μ = 1.00 × 10⁻³ Pa s. Determine the Reynolds number and assess whether a laminar analytical benchmark is appropriate.

The Reynolds number is

Substitution gives

This value is below the commonly used transition range for fully developed pipe flow, so a laminar model is appropriate as an initial benchmark. For a fully developed Newtonian laminar flow, the axial velocity profile is

where R = D/2 and r is radial distance from the centreline. The centreline velocity is therefore 2U = 0.20 m s⁻¹, and the no-slip wall condition gives u(R) = 0.

The pressure gradient for a tube of length L is

This relation assumes steady, incompressible, fully developed laminar flow in a circular tube with constant properties. Numerically,

A CFD solution should reproduce the parabolic profile and pressure gradient as the mesh is refined and the solver is converged. It is poor practice to claim validation from one matching centreline velocity alone; the pressure gradient, wall shear, mass flow, and profile should also be compared. Near the wall, the mesh should adequately represent the velocity gradient, even though no turbulence wall function is required.

10. Applied Case: CFD Assessment of an Automotive Exhaust Manifold

The following is an illustrative engineering case. An automotive manufacturer is redesigning a four-cylinder exhaust manifold to reduce cylinder-to-cylinder back pressure while maintaining acceptable wall temperature and avoiding excessive thermal stress.

Background and problem

The manifold contains merging branches, strong curvature, pulsating compressible flow, heat transfer to the solid, and possible flow separation. A steady incompressible simulation could predict a visually smooth flow field but would omit pressure-wave interactions and temperature-dependent density. The engineering objective is therefore to compare candidate geometries using pressure loss, branch mass-flow balance, wall temperature, and transient peak pressure.

Analysis and approach

The design team constructs a conjugate heat-transfer model comprising the gas domain and solid manifold. The gas is treated as compressible with temperature-dependent properties. Time-dependent inlet mass-flow histories are obtained from an engine-cycle model. A transient RANS model is selected for initial design screening, with local mesh refinement at branch junctions and near walls. The mesh is checked for skewness and boundary-layer resolution; time-step sensitivity is tested against the dominant pulse frequency.

At each operating condition, the team monitors mass conservation, pressure at each runner, total pressure loss, wall heat flux, and outlet temperature. Candidate designs are not ranked by a single contour. Instead, a weighted engineering assessment considers back pressure, thermal limits, manufacturing constraints, and robustness over the engine-speed range.

Verification and validation

The manifold calculation is first verified using a simplified geometry with a measured pressure-loss benchmark. Grid refinement is performed until the predicted pressure loss changes by less than the design tolerance. The transient time step is reduced until peak pressure and cycle-averaged loss are insensitive within the same tolerance. Thermocouple measurements and pressure transducers are then compared with CFD at selected operating points. Differences are examined for possible causes: sensor location, surface emissivity, turbulence model, inlet waveform, and uncertainty in material properties.

Outcome

Suppose the revised manifold reduces the computed cycle-averaged pressure loss by 8% but increases a local wall temperature by 25 K. The redesign cannot be accepted solely on the pressure benefit. The team may add a heat shield, alter wall thickness, or reshape the junction to reduce recirculation. The final recommendation should report predicted benefits, validated ranges, uncertainty, and conditions under which the design may fail.

Learning points

The case demonstrates that CFD is a decision-support method, not an image generator. Physical fidelity, numerical quality, validation data, and multidisciplinary constraints must be considered together. Model complexity should be increased only when it changes the decision or reduces uncertainty in a defensible way.

11. Challenges, Limitations, and Governance

CFD limitations arise from three sources. First, the mathematical model may omit physics such as transition, unresolved turbulence, radiation, surface roughness, or chemical non-equilibrium. Second, discretisation and mesh limitations create numerical error. Third, input data and boundary conditions may be uncertain. Increasing mesh density does not correct an incorrect physical model.

Computational cost can restrict design exploration, uncertainty quantification, and high-fidelity LES. Reduced-order models and surrogate models can accelerate optimisation, but their training range and extrapolation risk must be documented. Automatic mesh adaptation and machine-learning turbulence closures are promising, yet they require rigorous benchmark testing, physical constraints, and out-of-sample validation.

Engineering governance requires reproducibility. A simulation record should preserve solver version, input files, geometry revision, mesh-generation settings, numerical schemes, convergence history, material data, and post-processing scripts. Safety-critical decisions should not depend on an unverifiable proprietary setting or an undocumented manual adjustment. AI-assisted meshing, surrogate prediction, and automated design must remain subject to human review, traceable data provenance, and independent verification.

12. Contemporary Developments and Best Practice

Current research directions include high-order methods, adaptive mesh refinement, immersed-boundary methods, GPU acceleration, exascale computing, uncertainty quantification, hybrid RANS–LES, data assimilation, physics-informed machine learning, and digital twins. These developments expand capability but do not remove the need for conservation, verification, validation, and physical judgement.

Best practice can be summarised as follows:

• define outputs and acceptance criteria before running the model;
• choose the simplest physical model capable of answering the question;
• use mesh and time-step studies rather than relying on default settings;
• monitor conservation and engineering quantities, not residuals alone;
• match wall treatment to near-wall mesh resolution;
• distinguish numerical convergence from physical validation;
• document assumptions, uncertainty, and model limitations;
• compare simulations with analytical solutions and benchmark experiments whenever possible;
• preserve computational provenance and enable independent reproduction.

Chapter Summary

Computational Fluid Dynamics transforms conservation laws into a finite algebraic system through mesh generation, spatial discretisation, time integration, and iterative solution. The continuity, momentum, energy, and species equations provide the physical foundation, while constitutive and turbulence models close the system. Finite-volume methods are widely used because their control-volume formulation supports discrete conservation; finite-difference and finite-element methods offer important alternatives for regular and complex domains.

Numerical accuracy depends on consistency, stability, convergence, conservation, boundedness, mesh quality, and suitable treatment of convection and time. In incompressible flow, pressure–velocity coupling enforces continuity. Turbulence, compressibility, multiphase flow, combustion, and wall processes introduce model-form uncertainty that cannot be eliminated by simply refining the mesh.

A credible CFD study defines its engineering question, selects defensible physics, generates an appropriate mesh, solves with monitored convergence, verifies grid and time-step sensitivity, validates against reference evidence, and reports uncertainty. CFD results become professionally useful only when their limitations and range of validity are explicit.

Key Terms

Continuity equation: Conservation equation for fluid mass.

Control volume: Finite region over which conservation laws are integrated.

Convergence: Approach of a numerical solution or output to a stable value under iteration or refinement.

Discretisation: Conversion of continuous differential equations into algebraic equations.

Finite difference: Method that approximates derivatives at discrete points.

Finite element: Method based on basis functions and a weighted-residual formulation.

Finite volume: Method that integrates governing equations over control volumes.

Grid independence: Condition in which further mesh refinement negligibly changes the quantity of interest.

Mesh: Spatial partition of the computational domain.

Numerical diffusion: Artificial smoothing introduced by a discretisation scheme.

Peclet number: Ratio of convective to diffusive transport.

Pressure–velocity coupling: Numerical treatment that enforces compatibility between pressure and velocity.

RANS: Reynolds-averaged Navier–Stokes modelling approach.

Residual: Algebraic imbalance remaining in a discretised equation.

Reynolds number: Ratio of inertial to viscous effects.

Stability: Property that numerical errors remain controlled.

Turbulence closure: Model used to represent unresolved turbulent correlations.

Validation: Assessment of agreement between a model prediction and physical or benchmark evidence.

Verification: Assessment of whether equations have been solved correctly.

Wall function: Near-wall model that represents unresolved boundary-layer behaviour.

Review Questions

Short Answer Questions

1. What is the distinction between CFD verification and validation?
2. Why does an incompressible flow require pressure–velocity coupling?
3. Define numerical diffusion and state one consequence of excessive numerical diffusion.
4. What information is conveyed by the Reynolds number?
5. Why must wall treatment be consistent with near-wall mesh resolution?

Long Answer Questions

1. Derive the integral finite-volume form of a general scalar transport equation and explain the role of face fluxes.
2. Compare finite-difference, finite-volume, and finite-element methods for complex engineering flows.
3. Explain consistency, stability, convergence, conservation, and boundedness, and discuss why they are not interchangeable.
4. Compare RANS, LES, and DNS in terms of resolved physics, computational cost, and engineering applicability.
5. Develop a complete verification and validation plan for a transient heat-transfer CFD study.

Analytical / Application Questions

1. A liquid flows through a tube with ρ = 1000 kg m⁻³, U = 0.25 m s⁻¹, D = 0.01 m, and μ = 1.0 × 10⁻³ Pa s. Calculate the Reynolds number and recommend an initial flow model, stating the limitations of the recommendation.
2. A steady CFD solution has very low residuals, but the predicted drag changes by 6% when the mesh is refined. Diagnose the result and propose a technically defensible next step.
3. An unsteady simulation predicts periodic vortex shedding, but halving the time step changes the shedding frequency by 12%. Explain what this indicates and design a time-step verification study.

Multiple Choice Questions with Answers

Question 1

Which equation enforces mass conservation in a general compressible flow?

A. ∂ρ/∂t + ∇·(ρu) = 0

B. ∇·u = 0 in all flows

C. ρu·∇u = −∇p

D. q = −k∇T

Correct Answer: A. ∂ρ/∂t + ∇·(ρu) = 0

Question 2

What is the principal advantage of the finite-volume method?

A. It never requires a mesh

B. It enforces conservation over control volumes

C. It eliminates turbulence modelling

D. It is restricted to rectangular domains

Correct Answer: B. It enforces conservation over control volumes

Question 3

For water with ρ = 998 kg m⁻³, U = 0.10 m s⁻¹, D = 0.020 m, and μ = 1.00 × 10⁻³ Pa s, the Reynolds number is approximately:

A. 20

B. 200

C. 2,000

D. 20,000

Correct Answer: C. 2,000

Question 4

What is the main purpose of pressure correction in incompressible CFD?

A. To enforce mass conservation

B. To increase fluid density

C. To remove viscosity

D. To prescribe temperature

Correct Answer: A. To enforce mass conservation

Question 5

Which scheme generally introduces the greatest numerical diffusion for convection-dominated flow?

A. First-order upwind

B. Second-order central differencing

C. Spectral differentiation

D. Exact analytical integration

Correct Answer: A. First-order upwind

Question 6

The wall coordinate y⁺ primarily characterises:

A. Compressibility of the far field

B. Near-wall mesh placement relative to viscous scales

C. The global Mach number

D. The number of solver iterations

Correct Answer: B. Near-wall mesh placement relative to viscous scales

Question 7

What does validation primarily assess?

A. Whether the code compiled

B. Whether algebraic residuals are zero

C. Whether predictions agree adequately with physical or benchmark evidence

D. Whether the mesh contains only hexahedral cells

Correct Answer: C. Whether predictions agree adequately with physical or benchmark evidence

Question 8

For a fully developed laminar pipe flow, the centreline velocity is, in terms of mean velocity U:

A. U/2

B. U

C. √2U

D. 2U

Correct Answer: D. 2U

Question 9

A large cell Peclet number indicates that:

A. Diffusion dominates convection

B. Convection dominates diffusion locally

C. The fluid must be incompressible

D. The mesh is necessarily orthogonal

Correct Answer: B. Convection dominates diffusion locally

Question 10

Which statement about residuals is most accurate?

A. Low residuals alone guarantee physical validity

B. Residuals are irrelevant in CFD

C. Residuals should be considered together with conservation and engineering monitors

D. Residuals measure experimental uncertainty directly

Correct Answer: C. Residuals should be considered together with conservation and engineering monitors