10. Computational Fluid Dynamics

Introduction and Context

Computational Fluid Dynamics (CFD) is the numerical study of fluid motion, heat transfer, mass transport, and related physical phenomena. It converts the governing conservation laws of fluid mechanics into algebraic equations that can be solved on a computer. CFD has become an essential engineering tool because many flows are difficult, expensive, or dangerous to investigate exclusively through experiments. It is used in turbomachinery, internal combustion engines, aerospace systems, process equipment, automobiles, biomedical devices, environmental engineering, and energy systems.

CFD does not replace fluid mechanics or experimentation. A numerical solution is meaningful only when the physical model, boundary conditions, mesh, numerical scheme, and convergence assessment are appropriate. The central professional skill is therefore not merely operating a solver, but judging whether the computed result is physically and numerically credible.

The governing equations are usually the conservation equations for mass, momentum, and energy, supplemented by constitutive relations and turbulence or multiphase models when required. In this chapter, emphasis is placed on conservation-based finite-volume methods, pressure–velocity coupling, convection discretization, turbulence modeling, mesh quality, and transient simulations. These topics form the practical foundation for reliable incompressible and compressible CFD.

Learning Objectives

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

1. Explain the physical and mathematical basis of CFD.

2. Formulate conservation equations for incompressible and compressible flows.

3. Describe the finite-volume method and its treatment of fluxes and source terms.

4. Distinguish between pressure-based and density-based solution strategies.

5. Explain pressure–velocity coupling methods such as SIMPLE, PISO, and coupled algorithms.

6. Select suitable convection schemes while recognizing their accuracy and boundedness characteristics.

7. Evaluate mesh quality and conduct mesh-independence studies.

8. Select and assess turbulence models for engineering applications.

9. Design reliable transient CFD simulations.

10. Interpret CFD results critically and recognize common sources of error.

From Conservation Laws to a Computable Model

A fluid problem is described by conservation laws together with initial and boundary conditions. For a general transported scalar quantity \(\phi\), the integral conservation equation may be written as

\[

\frac{\partial}{\partial t}\int_V \rho\phi\,dV + \oint_A \rho\phi\mathbf{u}\cdot\mathbf{n}\,dA

= \oint_A \Gamma_\phi\nabla\phi\cdot\mathbf{n}\,dA + \int_V S_\phi\,dV.

\]

The terms represent accumulation, convection, diffusion, and sources, respectively. The finite-volume method applies this equation over small control volumes. Conservation is enforced locally: the flux leaving one control volume enters the neighboring volume with equal magnitude and opposite sign.

For mass conservation, \(\phi=1\), and the continuity equation is

\[

\frac{\partial \rho}{\partial t}+\nabla\cdot(\rho\mathbf{u})=0.

\]

For a Newtonian fluid, the momentum equation is

\[

\frac{\partial(\rho\mathbf{u})}{\partial t}+\nabla\cdot(\rho\mathbf{u}\mathbf{u})

=-\nabla p+\nabla\cdot\boldsymbol{\tau}+\rho\mathbf{g}+\mathbf{S}_m,

\]

where \(p\) is pressure, \(\boldsymbol{\tau}\) is the viscous stress tensor, \(\mathbf{g}\) is gravitational acceleration, and \(\mathbf{S}_m\) represents additional momentum sources.

For constant-viscosity incompressible flow, the viscous term becomes \(\mu\nabla^2\mathbf{u}\), and continuity reduces to

\[

\nabla\cdot\mathbf{u}=0.

\]

For compressible flow, density, pressure, temperature, and internal energy are coupled. The energy equation must normally be solved, and an equation of state, such as \(p=\rho RT\) for an ideal gas, closes the system. Compressibility effects become especially important when density changes are appreciable, often associated with high Mach number, strong heating, or pressure variations.

A CFD model also requires material properties, wall conditions, inlet and outlet specifications, symmetry or periodic conditions, and initial fields. Poorly selected boundary conditions can produce a numerically converged but physically meaningless solution.

The Finite-Volume Method

The finite-volume method divides the computational domain into control volumes surrounding cell centers or vertices. Each control volume has faces through which convective and diffusive fluxes are evaluated. Integrating the governing equation over a control volume and applying Gauss's divergence theorem gives an algebraic balance:

\[

a_P\phi_P=\sum_N a_N\phi_N+b.

\]

Here, \(P\) denotes the current cell, \(N\) its neighboring cells, and \(b\) includes source contributions and known boundary terms. The coefficients depend on mass fluxes, diffusion conductances, time-step size, and the selected discretization scheme.

At a face, the mass flow rate is

\[

\dot m_f=\rho_f\mathbf{u}_f\cdot\mathbf{A}_f.

\]

The convective flux is \(\dot m_f\phi_f\), while the diffusive flux is approximated using the face-normal gradient. Face values must be reconstructed from cell values. The simplest reconstruction is upwind: the face value is taken from the upstream cell. Central differencing uses an interpolation between neighboring cells and is formally second-order on suitable meshes, but may generate oscillations when convection dominates.

The finite-volume formulation is attractive because it preserves conservation at the discrete level. Nevertheless, conservation alone does not guarantee accuracy. A conservative calculation may still contain excessive numerical diffusion, inadequate resolution, or errors caused by an unsuitable turbulence model.

Boundary and Source Treatment

Boundary faces do not have a neighboring fluid cell, so their fluxes are obtained from specified conditions. A no-slip wall sets velocity to the wall velocity, while an adiabatic wall imposes zero normal heat flux. A prescribed pressure outlet should be used only when the flow direction and physical situation support it; an outlet placed too close to recirculation can cause instability or distortion.

Source terms require special care. Linearization in the form \(S_\phi=S_C+S_P\phi_P\), with a suitably non-positive \(S_P\), can improve stability. Strongly discontinuous or improperly scaled sources may produce poor conditioning and slow convergence.

Pressure–Velocity Coupling in Incompressible Flow

In incompressible flow, pressure is not determined by a separate thermodynamic equation. It acts as a constraint that enforces continuity. Since pressure and velocity are coupled, a momentum solution based on an estimated pressure generally does not satisfy mass conservation. Pressure–velocity coupling algorithms correct this inconsistency.

The SIMPLE algorithm begins with guessed pressure and face fluxes. The momentum equations are solved to obtain provisional velocities. A pressure-correction equation is then derived from the requirement that corrected face fluxes satisfy continuity. Pressure, velocity, and fluxes are corrected, and the process is repeated. Under-relaxation is commonly applied to pressure and momentum variables to control oscillations.

PISO performs multiple correction steps within a time step or outer iteration. It is particularly effective for transient calculations because additional corrections reduce the need for repeated outer iterations. SIMPLE is often robust for steady problems, whereas PISO can be advantageous when temporal accuracy and rapid pressure correction are important.

Coupled algorithms solve pressure and momentum equations together, often providing strong convergence for highly coupled or compressible flows. Their larger linear systems require more memory and computational effort. The choice depends on the physics, mesh, time scale, and solver implementation.

Residual reduction is useful but insufficient as the sole convergence criterion. A solution should also be monitored through mass imbalance, forces, pressure drop, heat-transfer rate, or another engineering quantity. A residual plateau may indicate mesh inadequacy, poor boundary conditions, insufficient under-relaxation, or an intrinsically unsteady flow rather than simple solver failure.

Convection Schemes and Numerical Behavior

Convection discretization strongly influences accuracy. First-order upwind schemes are bounded and robust but introduce numerical diffusion, which smears shear layers, wakes, and scalar gradients. They are often useful during initial iterations or for difficult flows, but final engineering predictions should not automatically rely on them.

Second-order upwind schemes reconstruct gradients to improve accuracy. They usually reduce numerical diffusion but may be less robust on poor meshes or in strongly separated flows. Central differencing has low numerical diffusion and is attractive for well-resolved, low-diffusion flows, but it can produce nonphysical oscillations in convection-dominated problems unless stabilization is provided.

Bounded high-resolution schemes limit reconstructed values to prevent new extrema. They offer a compromise between accuracy and stability. The appropriate scheme depends on mesh quality, Peclet number, flow regime, and the quantity being transported. A scheme that performs well for velocity may not be ideal for turbulence quantities or discontinuous compressible flow.

For compressible flows containing shocks, schemes must capture discontinuities without producing spurious oscillations. Flux-limited, upwind-biased, and approximate Riemann-solver approaches are commonly used. Shock-capturing methods introduce some numerical dissipation, which is necessary for stability but must be controlled to preserve physically important gradients.

Mesh Generation and Quality Assessment

The mesh is the geometric framework on which the equations are approximated. Structured meshes offer ordered connectivity and can provide high accuracy with relatively low numerical diffusion. Unstructured meshes accommodate complex geometry and local refinement more easily, but may require greater care in gradient reconstruction and quality control. Hybrid meshes combine approaches, often using hexahedral or prismatic layers near walls and tetrahedral or polyhedral cells elsewhere.

Important quality measures include skewness, non-orthogonality, aspect ratio, smoothness of cell-size transition, and alignment with dominant flow features. Excessive skewness makes the line connecting neighboring cell centers poorly aligned with the face normal, increasing interpolation error. High non-orthogonality requires correction terms that may reduce stability. Abrupt changes in cell size can reflect waves and generate artificial gradients.

Boundary layers demand special attention. If wall functions are used, the first-cell distance should be consistent with the model's wall-resolution assumptions, commonly expressed through the dimensionless wall distance \(y^+\). Low-Reynolds-number approaches resolve the near-wall region with small \(y^+\), whereas wall-function approaches place the first cell in an appropriate logarithmic-layer range. Using a turbulence model and wall treatment inconsistently can invalidate wall shear and heat-transfer predictions.

A mesh-independence study should use at least three systematically refined meshes where practical. The comparison should focus on quantities of interest, such as pressure drop, lift, drag, peak temperature, or average heat-transfer coefficient. Grid convergence is not established merely because contour plots appear similar. A formal refinement assessment may use the Grid Convergence Index or related extrapolation methods, provided the meshes are sufficiently systematic and the solution is in the asymptotic range.

Turbulence Modeling

Most engineering flows have Reynolds numbers high enough for direct resolution of all turbulent scales to be computationally impractical. Reynolds-averaged Navier–Stokes (RANS) methods decompose instantaneous variables into mean and fluctuating parts. Averaging introduces Reynolds stresses, creating a closure problem.

The standard \(k-\varepsilon\) family solves transport equations for turbulent kinetic energy \(k\) and its dissipation rate \(\varepsilon\). It is robust and widely used for free shear flows and many industrial applications, but may be less reliable for strong separation, rotation, curvature, or near-wall effects.

The \(k-\omega\) family uses specific dissipation rate \(\omega\). It often performs well near walls, while the shear-stress-transport formulation blends near-wall behavior with outer-flow characteristics and is frequently selected for adverse-pressure-gradient and separated flows.

Reynolds stress models solve additional transport equations for individual Reynolds stresses and can represent anisotropy more directly. Their cost and convergence difficulty are greater. Large-eddy simulation resolves large turbulent structures and models smaller scales, offering richer unsteady information but requiring substantially finer meshes and smaller time steps. Direct numerical simulation resolves all scales and is generally restricted to low-Reynolds-number research problems.

No turbulence model is universally superior. Model selection should be based on flow physics, available resolution, required output, validation evidence, and computational resources. Turbulence-model sensitivity should be examined when predictions are important or the flow lies outside a model's established range.

Compressible Flow and Energy Coupling

In compressible CFD, density variations couple continuity, momentum, energy, and the equation of state. Mach number, pressure-based versus density-based formulation, and thermal boundary conditions influence solver selection. Pressure-based methods can handle a broad range of flow speeds with suitable compressibility treatment, whereas density-based methods are naturally suited to strongly compressible, shock-dominated regimes.

The energy equation includes convection, heat conduction, viscous dissipation, pressure work, and possible volumetric sources. Thermal properties may depend strongly on temperature. At high temperature, constant-property assumptions can lead to significant errors in density, viscosity, acoustic speed, and heat transfer.

Shock waves require adequate resolution and appropriate numerical dissipation. Boundary conditions must distinguish between subsonic and supersonic regions. At a subsonic inlet, multiple flow variables may be specified because information enters the domain in several characteristic directions. At a supersonic inlet, all characteristics enter and the required state can generally be prescribed. At a supersonic outlet, imposing an additional pressure condition may overconstrain the problem.

Transient CFD Simulations

A transient simulation advances the solution through discrete time steps. The time-step size should resolve both physical time scales and numerical stability requirements. A useful indicator is the Courant number,

\[

Co=\frac{u\Delta t}{\Delta x},

\]

or its multidimensional generalization. The acceptable value depends on the discretization scheme and solver, but a small Courant number does not by itself guarantee temporal accuracy.

First-order implicit time integration is robust but numerically diffusive. Second-order implicit methods improve temporal accuracy but may require better initial fields and tighter convergence within each time step. Explicit methods impose restrictive stability limits but can be efficient for suitable wave-resolving calculations.

The number of iterations per time step should be sufficient to reduce algebraic error below the scale of the physical change being computed. If the solution is not adequately converged at each step, temporal errors become mixed with iterative errors. Periodic flows should be advanced until statistically stationary behavior is reached, after which mean values and fluctuations can be sampled over an appropriate interval.

A Reliable CFD Workflow

A professional CFD study begins with a clear engineering question. The analyst should identify the required outputs, relevant physical effects, acceptable uncertainty, and validation data. Geometry is then simplified deliberately: small features may be removed if they do not influence the target quantities, while flow restrictions, sharp corners, and heat-transfer surfaces may need to be retained.

The next stages are physical-model selection, domain definition, boundary-condition specification, mesh generation, solver initialization, and solution monitoring. A robust workflow often begins with conservative schemes and relaxed settings, then progresses to higher-order discretization after the flow field becomes stable. Mesh and model sensitivity studies should be planned rather than performed only after an unexpected result.

Post-processing must be quantitative. Conservation balances, residual histories, surface integrals, line profiles, force coefficients, pressure losses, and uncertainty estimates are more informative than visually attractive contours. Results should be compared with analytical solutions, benchmark cases, experiments, or trusted correlations whenever possible.

Illustrative Case Study: CFD Analysis of a Heated Air Channel

Background

Consider an illustrative engineering case involving air flowing through a rectangular channel containing a uniformly heated lower wall. The objective is to predict pressure drop and average heat-transfer coefficient for use in a compact thermal-management system.

Situation and Problem

A preliminary simulation using a coarse mesh and first-order upwind discretization predicts a low pressure drop and nearly uniform wall temperature. However, an independent energy balance indicates that the heat removed by the air is inconsistent with the supplied wall heat flux. The engineering team must determine whether the discrepancy results from mesh resolution, boundary conditions, turbulence modeling, or inadequate convergence.

Analysis

The flow is internal and forced, with a temperature rise along the channel. The inlet mass flow rate and temperature are known, while the outlet pressure is specified. Because the target includes heat transfer, the energy equation is required. A mesh-refinement study is designed with local refinement near the heated wall and sufficient streamwise resolution. The near-wall treatment is selected consistently with the first-cell height.

The initial calculation uses a stable first-order scheme to obtain a developed flow field. It is then continued with a second-order scheme. Mass-flow imbalance, total enthalpy balance, pressure drop, wall heat flux, and area-averaged wall temperature are monitored. Two turbulence models are tested because the flow may contain developing boundary layers and mild separation near the channel entrance.

Approach and Solution

The refined meshes reduce the discrepancy in wall heat transfer. The energy equation is solved with temperature-dependent air properties, and the outlet is moved sufficiently far downstream to avoid imposing a condition inside a developing recirculation region. The second-order solution is accepted only after the heat balance closes within the engineering tolerance and the monitored quantities become insensitive to further iteration.

The study reports not only the final heat-transfer coefficient but also mesh sizes, wall treatment, time or iteration convergence, property assumptions, and sensitivity to turbulence model. This documentation allows another engineer to reproduce and assess the result.

Outcome

The case demonstrates that the first converged solution was not necessarily the first reliable solution. The apparent agreement of temperature contours had hidden an energy imbalance and excessive numerical diffusion. Refinement, consistent boundary conditions, improved discretization, and conservation monitoring produced a defensible result.

Learning Points

The principal lesson is that CFD credibility is established through verification and validation, not through solver convergence alone. Engineering quantities must be monitored directly, and numerical choices must be connected to the physics of the problem.

Challenges, Errors, and Professional Judgment

Common mistakes include using an outlet boundary too close to separation, specifying incompatible pressure and velocity conditions, neglecting compressibility in a high-speed flow, and applying wall functions without checking near-wall resolution. Another frequent error is interpreting residual reduction as proof of accuracy. Residuals can fall while an incorrect boundary condition or insufficient mesh continues to dominate the result.

Under-relaxation can stabilize a calculation, but excessive under-relaxation may conceal modeling problems and make convergence unnecessarily slow. Conversely, aggressive relaxation can produce oscillations or divergence. Poor initialization, abrupt property changes, highly skewed cells, and inconsistent units are practical sources of failure.

CFD also involves uncertainty. Discretization error, iterative error, modeling error, input uncertainty, and geometric uncertainty contribute differently. A refined mesh reduces one category but does not correct an inappropriate turbulence model or uncertain inlet profile. Validation against experimental data is therefore essential when decisions involve safety, certification, major capital expenditure, or public risk.

Professional, Ethical, and Digital Considerations

CFD results may influence aircraft safety, pressure-vessel design, thermal protection, emissions, and medical-device performance. Analysts have a professional obligation to document assumptions, numerical settings, validation evidence, and limitations. Selective presentation of favorable contours while omitting sensitivity studies is technically misleading.

Modern CFD platforms increasingly include automated meshing, adaptive refinement, cloud computing, reduced-order models, and machine-learning-assisted surrogate models. Automation can improve productivity, but it does not eliminate the need for physical judgment. Artificial intelligence may help identify flow features, optimize designs, or accelerate parameter studies; however, training-data bias, extrapolation failure, and lack of physical constraints must be considered. Automated optimization should include conservation checks, manufacturability constraints, and independent verification.

Current Developments and Best Practices

Current research and industrial practice are moving toward hybrid RANS–LES methods, adaptive mesh refinement, high-order discretization, immersed-boundary methods, GPU acceleration, uncertainty quantification, and tightly coupled multiphysics simulation. Digital engineering workflows increasingly connect CAD, meshing, solvers, optimization, and experimental databases.

The following practices provide a dependable foundation:

• Define the engineering question and output quantities before meshing.
• Use conservation laws and dimensional analysis to check the model.
• Choose boundary conditions based on the physical experiment, not convenience.
• Inspect mesh quality and resolve regions controlling the target output.
• Start robustly, then increase spatial and temporal order when appropriate.
• Monitor engineering quantities as well as residuals.
• Perform mesh, time-step, and model-sensitivity studies.
• Validate against analytical, experimental, or benchmark evidence.
• Report assumptions, uncertainty, and limitations transparently.

Chapter Summary

Computational Fluid Dynamics transforms conservation equations into numerical solutions over a discretized flow domain. The finite-volume method is especially valuable because it enforces local conservation through control-volume flux balances. Reliable CFD requires appropriate treatment of pressure–velocity coupling, convection, diffusion, source terms, turbulence, compressibility, and time advancement.

Mesh quality and near-wall resolution strongly influence accuracy. SIMPLE, PISO, and coupled algorithms provide different strategies for enforcing continuity and coupling pressure with velocity. Convection schemes involve a trade-off between robustness, boundedness, and numerical diffusion. Turbulence models are approximations whose suitability depends on flow physics and required outputs. Transient simulations require time-step and inner-convergence control. Ultimately, CFD quality is established through verification, validation, sensitivity analysis, and professional reporting rather than by attractive plots or residual reduction alone.

Key Terms

Finite-volume method: A discretization method that applies conservation laws over finite control volumes.

Control volume: A small computational region over which integral conservation is enforced.

Continuity equation: Conservation equation for mass.

Pressure–velocity coupling: Numerical treatment linking pressure corrections to velocity and mass conservation.

SIMPLE: An iterative pressure-correction algorithm widely used for steady incompressible flow.

PISO: A multiple-correction pressure–velocity algorithm suited especially to transient calculations.

Convection: Transport of a quantity by bulk fluid motion.

Diffusion: Transport caused by molecular or turbulent gradients.

Numerical diffusion: Artificial smearing introduced by a discretization scheme.

Skewness: A measure of deviation of a cell geometry from an ideal computational shape.

Non-orthogonality: Misalignment between the face normal and the line joining neighboring cell centers.

Wall function: A near-wall modeling treatment that avoids resolving the entire viscous sublayer.

Turbulent kinetic energy: Mean kinetic energy per unit mass associated with velocity fluctuations.

RANS: Reynolds-averaged Navier–Stokes approach using modeled turbulence stresses.

LES: Large-eddy simulation that resolves large turbulent structures and models smaller ones.

Courant number: A nondimensional ratio relating fluid travel during a time step to cell size.

Mesh independence: Condition in which further mesh refinement has negligible effect on target outputs.

Verification: Assessment of whether the equations are solved correctly.

Validation: Assessment of whether the model represents the physical system adequately.

Compressible flow: Flow in which density changes are significant or must be included in the model.

Review Questions

Short Answer Questions

1. Why is pressure treated as a constraint variable in incompressible CFD?

2. What is the principal conservation advantage of the finite-volume method?

3. Define numerical diffusion and state one undesirable consequence.

4. What does the Courant number indicate in a transient simulation?

5. Distinguish verification from validation.

Long Answer Questions

1. Derive the general finite-volume algebraic balance for a transported scalar and explain the role of face fluxes.

2. Explain the working principles of SIMPLE and PISO and compare their typical applications.

3. Discuss how mesh skewness, non-orthogonality, aspect ratio, and near-wall resolution affect CFD accuracy.

4. Compare RANS, LES, and DNS in terms of physical resolution, computational cost, and engineering use.

5. Explain the major steps required to conduct a credible CFD study of a compressible heated flow.

Analytical / Application Questions

1. A steady incompressible calculation has low residuals but a significant mass imbalance at the outlet. Diagnose possible causes and propose a systematic corrective procedure.

2. A first-order calculation predicts a much lower pressure drop than a second-order calculation on a refined mesh. Explain the numerical and physical reasons for this difference and identify checks needed before accepting either result.

3. Design a verification plan for an unsteady turbulent flow through a duct, including mesh refinement, time-step selection, turbulence-model sensitivity, monitored quantities, and validation evidence.

22. Multiple Choice Questions with Answers

Question 1

Which feature most directly explains why the finite-volume method is widely used in engineering CFD?

A. It eliminates the need for boundary conditions

B. It enforces conservation through control-volume flux balances

C. It always produces second-order accuracy

D. It does not require a computational mesh

Correct Answer: B. It enforces conservation through control-volume flux balances

Question 2

In incompressible flow, the primary numerical role of pressure is to:

A. Specify fluid viscosity

B. Control temperature diffusion

C. Enforce continuity by correcting velocity fluxes

D. Replace the momentum equation

Correct Answer: C. Enforce continuity by correcting velocity fluxes

Question 3

A first-order upwind scheme is generally robust because it:

A. Introduces controlled numerical diffusion

B. Eliminates all discretization error

C. Always resolves shocks exactly

D. Uses no information about flow direction

Correct Answer: A. Introduces controlled numerical diffusion

Question 4

Which algorithm is particularly associated with multiple pressure corrections within a time step?

A. SIMPLE

B. PISO

C. DNS

D. RANS

Correct Answer: B. PISO

Question 5

If the line joining two neighboring cell centers is strongly misaligned with a face normal, the mesh has excessive:

A. Aspect ratio

B. Orthogonality

C. Non-orthogonality

D. Temporal resolution

Correct Answer: C. Non-orthogonality

Question 6

What is the principal purpose of a mesh-independence study?

A. To prove that residuals are unnecessary

B. To determine whether target outputs change significantly with refinement

C. To select the largest possible time step

D. To remove the need for experimental validation

Correct Answer: B. To determine whether target outputs change significantly with refinement

Question 7

Which turbulence approach resolves large eddies while modeling smaller scales?

A. DNS

B. LES

C. Laminar modeling

D. Steady potential flow

Correct Answer: B. LES

Question 8

A CFD solution has converged residuals but an incorrect heat balance. The most appropriate conclusion is that:

A. The solution is automatically valid

B. The mesh must be discarded immediately

C. Algebraic convergence has not guaranteed physical credibility

D. The energy equation should always be removed

Correct Answer: C. Algebraic convergence has not guaranteed physical credibility

Question 9

For a transient simulation, reducing the time step primarily improves:

A. Temporal resolution, provided each step is adequately converged

B. The thermodynamic equation of state

C. The physical accuracy of an unsuitable turbulence model

D. The geometry definition

Correct Answer: A. Temporal resolution, provided each step is adequately converged

Question 10

Which statement best distinguishes validation from verification?

A. Verification compares with experiments; validation checks algebraic equations

B. Verification checks correct solution of the mathematical model; validation compares the model with physical reality

C. Both terms refer only to residual reduction

D. Validation concerns mesh quality only

Correct Answer: B. Verification checks correct solution of the mathematical model; validation compares the model with physical reality