CFD Fundamentals — Governing Equations, Numerical Methods & Key Parameters

CFD numerically solves three coupled conservation laws that govern every fluid flow. Think of a river: mass can't appear or disappear (continuity), momentum changes only when forces act on the water (Navier-Stokes), and if the water warms near a hot rock, energy has to balance too (energy equation). These three laws together describe everything from the airflow over a racing car wing to coolant flow through a data center.

The governing equations in compact form:

Continuity (mass conservation): $\dfrac{\partial \rho}{\partial t} + \nabla \cdot (\rho \mathbf{u}) = 0$

Momentum (Navier-Stokes): $\rho\dfrac{D\mathbf{u}}{Dt} = -\nabla p + \nabla \cdot \boldsymbol{\tau} + \rho \mathbf{g}$

Energy: $\rho c_p \dfrac{DT}{Dt} = \nabla \cdot (k \nabla T) + \Phi$

where $\boldsymbol{\tau}$ is the viscous stress tensor and $\Phi$ is viscous dissipation. These are nonlinear partial differential equations — no closed-form solution exists for general geometries and flow conditions. That's why numerical methods are essential.

Analytical solutions exist only for highly idealized cases — Poiseuille pipe flow, Stokes flow around a sphere, Couette flow between parallel plates. The moment you have a real geometry — a centrifugal pump impeller, a car door mirror, an aircraft engine inlet — boundary conditions become impossible to express analytically. A modern CFD mesh discretizes the domain into millions of small control volumes and solves a system of algebraic equations at every cell, iterating until convergence. That's essentially what OpenFOAM, Fluent, and Star-CCM+ do under the hood.

The vast majority of industrial CFD codes — OpenFOAM, Fluent, Star-CCM+ — use the Finite Volume Method (FVM). Here's why: FVM integrates the conservation equations over each control volume, so mass, momentum, and energy are conserved exactly at the cell level regardless of mesh quality. FDM approximates derivatives at grid points — simple to implement but requires structured meshes. FEM uses weighted residuals over elements and is dominant in structural mechanics, but less natural for convection-dominated flows. FVM hits the sweet spot: conservative, flexible on unstructured meshes, and well-proven over 40 years of industrial use.

Three completely different quantities, but each is diagnostic for a different aspect of the flow or the numerics:

Reynolds number — ratio of inertial to viscous forces:

$$Re = \frac{\rho U L}{\mu} = \frac{UL}{\nu}$$

Low Re (say, Re < 2000 for a pipe): laminar, smooth flow. High Re (Re > 4000 for pipe): turbulent, chaotic. Re tells you whether you need a turbulence model. A 1 mm micro-channel at Re = 0.01 needs no turbulence model; a wind turbine blade at Re = 10⁷ definitely does.

Mach number — ratio of flow speed to local speed of sound:

$$Ma = \frac{U}{a}, \qquad a = \sqrt{\gamma R T}$$

Ma < 0.3: incompressible assumption valid (density changes < 5%). Ma > 0.3: compressible effects become important; use density-based solvers. Ma > 1: supersonic — shocks appear. This number decides whether you solve incompressible Navier-Stokes or the full compressible Euler/N-S equations.

Courant number (CFL) — governs time-step stability in transient simulations:

$$Co = \frac{U \Delta t}{\Delta x}$$

For explicit time integration, Co < 1 is required for stability — it means a fluid parcel moves less than one cell per time step. Implicit schemes tolerate Co > 1, but accuracy degrades. In OpenFOAM's controlDict, setting maxCo 0.5 keeps transient simulations stable with auto time-stepping.

Start with three diagnostic questions: Is the flow incompressible or compressible (Ma)? Is it steady or transient? Is it single-phase or multiphase? Those three answers narrow it down fast. For most industrial problems — subsonic aerodynamics, HVAC, pipe flow — simpleFoam (steady, incompressible RANS) is the workhorse. Add a heat equation and you need buoyantSimpleFoam. If you have free surfaces, interFoam (VOF method). If Ma > 0.3, switch to rhoCentralFoam or sonicFoam.

Each tool has a distinct character. OpenFOAM is free but text-based — you learn a lot by configuring case files manually, and it's highly customizable. Fluent has a polished GUI and excellent documentation — good for teams that need validated workflows fast. Star-CCM+ has the best integrated mesher (polyhedral auto-meshing) and is very strong in automotive and turbomachinery. SU2 is open-source and focused on aerospace shape optimization. The "free vs. paid" question in a company context is really "engineer time vs. license cost" — a $50,000/year Fluent license pays for itself if it saves a senior engineer two weeks per project.