Incompressible flow is one of the most frequently encountered flow regimes encompassing a diverse set of problems that include: atmospheric dispersal, food processing, aerodynamic design of automobiles, biomedical flows, electronics cooling, and manufacturing processes such as chemical vapor deposition, mold filling, and casting.

The momentum equations in integral form for an arbitrary control volume can be written as

Incompressibility requires a solenoidal velocity field expressed by

The solution of the incompressible Navier-Stokes equations poses a number of algorithmic issues due to the divergence-free velocity condition and the concomitant spatial and temporal resolution required to achieve solutions in complex geometries for engineering applications. The Abaqus/CFD incompressible solver uses a hybrid discretization built on the integral conservation statements for an arbitrary deforming domain. For time-dependent problems, an advanced second-order projection method is used with a node-centered finite-element discretization for the pressure. This hybrid approach guarantees accurate solutions and eliminates the possibility of spurious pressure modes while retaining the local conservation properties associated with traditional finite volume methods. An edge-based implementation is used for all transport equations permitting a single implementation that spans a broad variety of element topologies ranging from simple tetrahedral and hexahedral elements to arbitrary polyhedral. In Abaqus/CFD tetrahedral, wedge, and hexahedral elements are supported.

The energy transport equation is optionally activated in Abaqus/CFD for non-isothermal flows. For small density variations, the Boussinesq approximation provides the coupling between momentum and energy equations. In turbulent flows, the energy transport includes a turbulent heat flux based on the turbulent eddy viscosity and turbulent Prandtl number. Abaqus/CFD provides a temperature-based energy equation.

The energy equation, in temperature form, can be obtained from the first law of thermodynamics and is given by

Turbulence modeling is a pacing technology for computational fluid dynamics. There is no single universal turbulence model that can adequately handle all possible flow conditions and geometrical configurations. This is complicated by the plethora of turbulence models and modeling approaches that are currently available; e.g., Reynolds Averaged Navier-Stokes (RANS), Unsteady Reynolds Averaged Navier-Stokes (URANS), Large-Eddy Simulation (LES), Implicit Large-Eddy Simulation (ILES), and hybrid RANS/LES (HRLES). Ultimately, you must ensure that the approximations made in a given turbulence model are consistent with the physical problem being modeled.

The following turbulent flow models are available: ILES, Spalart-Allmaras (SA), and RNG k–. These models span a relatively broad set of flow problems that include time-dependent flows, fluid-structure interaction (FSI), and conjugate heat transfer (CHT).

Spalart-Allmaras (SA) turbulence model

The Spalart-Allmaras (SA) model is a one-equation turbulence model that uses an eddy-viscosity variable with a nonlinear transport equation. The model was developed based on empiricism, dimensional analysis, and a requirement for Galilean invariance. The model has found broad use and has been calibrated for two-dimensional mixing layers, wakes, and flat-plate boundary layers. The model produces reasonably accurate predictions of turbulent flows in the presence of adverse pressure gradients and may be used for flows where separation occurs. This model is spatially local and requires only moderate resolution in boundary layers. Although initially designed for external and free-shear flows, the Spalart-Allmaras model can also be used for internal flows.

The basic form of the one-equation Spalart-Allmaras model consists of one transport equation for the turbulent eddy viscosity, . The model requires the normal distance from the wall used in the damping functions needed to control the turbulent viscosity in the near-wall region. Abaqus/CFD automatically computes the normal distance function, permitting simple specification of the model boundary conditions. The turbulent viscosity transport equation for the Spalart-Allmaras model is given by

where the damping functions and model coefficients are defined as:

where is the normal distance from the wall, and the effective turbulent viscosity is defined as

The Spalart-Allmaras model coefficients are shown in Table 6.6.2–1.

Table 6.6.2–1 Spalart-Allmaras model coefficients.

0.1355	0.622	7.1	2/3		0.3	2	0.41	5

The Spalart-Allmaras model can provide very accurate boundary layer results if the near-wall region is resolved (near-wall resolution such that the nondimensional wall distance is approximately 3). However, the implementation of boundary conditions for the Spalart-Allmaras model in Abaqus/CFD permits the use of coarser meshes as well.

Input File Usage:

You can generate the input file using Abaqus/CAE.

Abaqus/CAE Usage:

Step module: Create Step: General: Flow; Turbulence: Spalart-Allmaras

RNG k–epsilon turbulence model

The RNG k– model is a two-equation turbulence model that evolves an equation for the turbulent kinetic energy, k, and the energy dissipation rate, . The model equations are developed from fundamental physical principles and dimensional analysis. In general, the coefficients of the model are usually calibrated using canonical flows and experimental data. However, the RNG version of the model computes the coefficients using Renormalization Group theory (Yakhot et al., 1992). The model equations are

where

The RNG k– model coefficients are shown in Table 6.6.2–2.

Table 6.6.2–2 RNG k– model coefficients.

1.42	1.68	0.085	0.72	0.72	0.012	4.38

Input File Usage:

You can generate the input file using Abaqus/CAE.

Abaqus/CAE Usage:

Step module: Create Step: General: Flow; Turbulence: k-epsilon renormalization group (RNG)

Wall function

It is well known that the k– model has limitations, especially on wall-bounded simulations where high values of eddy viscosity in the near-wall region are usually reproduced. Consequently, near-wall modeling is usually provided to improve the accuracy of the predictions. For the current implementation the “law of the wall” approach is used to provide near-wall modeling to the k– model. This approach relies on known results (law of the wall) to obtain the wall shear stress.

The law of the wall is a universal velocity profile that wall-bounded flows (in the absence of pressure gradients) develop when the proper viscous scales are used to normalize the velocity and length scales. This law can be stated as

where

is the wall tangent velocity, is the kinematic viscosity, is the density, is the shear stress at the wall, and and are constants. An alternative set of units can be defined as

In equilibrium conditions (i.e., in the absence of pressure gradients, ), the law of the wall can be written in the following alternative form:

where the wall shear stress can be computed as

where the subscript p stands for evaluation at the element center of the first element away from the wall.

Many industrial CFD/FSI/CHT problems involve moving boundaries or deforming geometries. This class of problem includes prescribed boundary motion that induces fluid flow or where the boundary motion is relatively independent of the fluid flow. Abaqus/CFD uses an arbitrary Lagrangian Eulerian (ALE) formulation and automated mesh deformation method that preserves element size in boundary layers. The ALE and deforming-mesh algorithms are activated automatically for problems that involve a moving boundary prescribed by the user or identified as a moving boundary in an FSI co-simulation.

To properly control the mesh motion during a simulation, it is the user’s responsibility to prescribe appropriate displacement boundary conditions on the computational mesh.

The solution methods for the momentum and auxiliary transport equations in Abaqus/CFD rely on scalable parallel preconditioned Krylov solvers. The pressure, pressure-increment, and distance function equations are solved with user-selectable Krylov solvers and a robust algebraic multigrid preconditioner. A set of preselected default convergence criteria and iteration limits are prescribed for all linear equation solvers. The default solver settings should provide computationally efficient and robust solutions across a spectrum of CFD problems. However, full access to diagnostic information, convergence criteria, and optional solvers is provided. In practice, the pressure-increment equation may be the most sensitive linear system and could require user intervention based on knowledge of the specific flow problem.

Abaqus/CFD relies on a second-order semi-implicit projection method for time-dependent problems. By default, all viscous/diffusive terms are treated with a second-order accurate trapezoid rule while the advective terms are currently treated explicitly. In addition, the use of a Galerkin or backward-Euler integrator may be selected for the viscous/diffusive terms. When attempting to reach a steady state, the use of backward-Euler time-marching with a relaxed tolerance on the divergence is recommended.

By default, Abaqus/CFD uses automatic time incrementation that guarantees the solution stability. You may select fixed time-step incrementation, but stability may not be guaranteed. The explicit advection treatment requires that the Courant-Freidrichs-Levy (CFL) stability condition be respected, which requires that . With automatic incrementation, you can select an initial time increment, but the initial time step may be recomputed.

Abaqus/CFD provides a number of output variables that are useful for monitoring the health of a calculation and are good indicators for situations where the flow has reached a steady-state condition. These variables are typically written to the status (.sta) file. The RMS divergence output variable is useful for determining if a calculation is proceeding normally. Abnormally large values of the RMS divergence output variable typically indicate that the problem is incorrectly specified or that the calculation has become unstable. The global kinetic energy (KE) provides a good indicator for when the flow has reached a steady state. Alternatively, the global kinetic energy can indicate a steady-periodic flow situation.