Couette flow (shear flow between parallel plates)

It's the steady laminar flow between parallel plates where the top plate moves with velocity $U$. The linear velocity distribution $u(y) = Uy/h$ is the exact solution. It's the simplest non-trivial solution of the Navier-Stokes equations and is used to verify the implementation of the viscous term in CFD solvers. It's an ideal starting point for the Code Verification procedure in ASME V&V 20.

Because the velocity field is spatially linear, it should be solved exactly by any discretization scheme (Finite Volume Method, Finite Element Method, Finite Difference Method). If the numerical solution doesn't match the theoretical solution, it immediately indicates a bug in the discretization or boundary condition implementation. Extending it to generalized Couette flow with a pressure gradient (Couette-Poiseuille flow) allows verification of parabolic distributions as well.

Under the assumptions of steady, incompressible, fully developed flow, the Navier-Stokes equation reduces to:

For pure Couette flow, $dp/dx = 0$, so

The shear stress $\tau$ is constant regardless of height. The theoretical wall shear stress is $\tau_w = \mu U/h$, which can be used directly to verify the wall friction coefficient output from a CFD solver.

For generalized Couette flow (Couette-Poiseuille flow):

The second term is the Poiseuille component, resulting in a parabolic distribution. The superposition pattern of forward/backward flow changes depending on the sign of $dp/dx$, which can be used to verify the accuracy of the nonlinear terms in discretization schemes.

$h = 0.01$ m, $U = 1$ m/s, $\mu = 0.001$ Pa·s (equivalent to water), $\rho = 1000$ kg/m³. Re = $\rho U h/\mu = 10000$, but we enforce the laminar solution.

Theoretical values: $u(y) = 100y$ (y in m), $\tau_w = 0.1$ Pa.

Even with a 5-cell mesh in the height direction using OpenFOAM's simpleFoam, the velocity field matches exactly. This is because FVM's linear interpolation can accurately represent a linear velocity field. If it doesn't match, there's a problem with the boundary condition implementation.

Use simpleFoam. Case structure:

• constant/transportProperties: nu 1e-06 (kinematic viscosity)
• 0/U: Top wall fixedValue uniform (1 0 0), bottom wall fixedValue uniform (0 0 0), front/back faces empty
• 0/p: Inlet/outlet fixedValue uniform 0
• system/fvSchemes: div(phi,U) Gauss linear is sufficient.

Solve with a 2D mesh (1 cell × N_y × 1 cell using blockMesh). Even with N_y = 5, the velocity distribution matches exactly.

Specify the wall velocity directly with fixedValue. There is also a boundary condition called movingWallVelocity, but that is for ALE calculations where the mesh moves. For cases where the wall is at a fixed position and only the velocity is specified, fixedValue is fine.

Enable the Moving Wall option in the wall boundary condition and set Speed = 1 m/s. Solve with a steady solver (Pressure-Based, Coupled or SIMPLE). Select Second Order discretization.

In Fluent's case, internal pressure-velocity coupling uses Rhie-Chow interpolation, but for Couette flow the pressure gradient is zero, so the accuracy of this interpolation is not an issue. Do not use wall functions; specify the Laminar model.

If a turbulence model is enabled at Re = 10000, the solution will deviate from the laminar theoretical solution. The k-ε model generates turbulent viscosity near the wall, making the velocity profile nonlinear. This is the behavior of the turbulence model, not a code bug. For Code Verification, always run with the Laminar model and confirm agreement with the theoretical solution.

Because it's a linear velocity field, theoretically the exact solution can be obtained with a single cell using discretization schemes of linear order or higher. In practice, it depends on the order of the FVM face interpolation (linear, upwind, etc.).

All schemes match exactly. This is a special characteristic of Couette flow; differences appear for nonlinear velocity fields (Poiseuille flow).

No, bugs can be detected when "it should match exactly but doesn't." Mistakes can lurk in the details of implementation, such as internal interpolation of boundary conditions, handling of wall velocity, zero-gradient conditions for the pressure equation, etc. It can also be used for accuracy verification on non-uniform (biased) meshes.