# 6.6 Fluid dynamic analysis • “Fluid dynamic analysis procedures: overview,” Section 6.6.1 • “Incompressible fluid dynamic analysis,” Section 6.6.2 # 6.6.1 FLUID DYNAMIC ANALYSIS PROCEDURES: OVERVIEW # Overview Abaqus/CFD provides advanced computational fluid dynamics capabilities with extensive support for preprocessing and postprocessing provided in Abaqus/CAE. These scalable parallel CFD simulation capabilities address a broad range of nonlinear coupled fluid-thermal and fluid-structural problems. Abaqus/CFD can solve the following types of incompressible flow problems: • Laminar and turbulent: Internal or external flows that are steady-state or transient, span a broad Reynolds number range, and involve complex geometry may be simulated with Abaqus/CFD. This includes flow problems induced by spatially varying distributed body forces. • Thermal convective: Problems that involve heat transfer and require an energy equation and that may involve buoyancy-driven flows (i.e., natural convection) can also be solved with Abaqus/CFD. This type of problem includes turbulent heat transfer for a broad range of Prandtl numbers. • Deforming-mesh ALE: Abaqus/CFD includes the ability to perform deforming-mesh analyses using an arbitrary Lagrangian-Eulerian (ALE) description of the equations of motion, heat transfer, and turbulent transport. Deforming-mesh problems may include prescribed boundary motion that induces fluid flow or FSI problems where the boundary motion is relatively independent of the fluid flow. For more details, see “Incompressible fluid dynamic analysis,” Section 6.6.2. # Activation of fields in Abaqus/CFD In Abaqus/CFD the active fields (degrees of freedom) are determined by the analysis procedure and the options specified, such as turbulence models and auxiliary transport equations. For example, using the energy equation in conjunction with the incompressible flow procedure activates the velocity, pressure, and temperature degrees of freedom. For a complete listing of the available degrees of freedom, see “Active degrees of freedom” in “Boundary conditions in Abaqus/CFD,” Section 34.3.2. # 6.6.2 INCOMPRESSIBLE FLUID DYNAMIC ANALYSIS Products: Abaqus/CFD Abaqus/CAE # References • “Defining an analysis,” Section 6.1.2 • “Fluid dynamic analysis procedures: overview,” Section 6.6.1 # Overview An incompressible fluid dynamics analysis: • is one where the velocity field is divergence-free and the pressure does not contain a thermodynamic component; • is one where the energy contained in acoustic waves is small relative to the energy transported by advection (i.e., when the Mach number is in the range $0 \leq M \leq 0 . 1 - 0 . 3 )$ ; • can be either laminar or turbulent, steady or time-dependent; • can be used to study either internal or external flows; • can include energy transport and buoyancy forces; • can be used with a deforming mesh for ALE calculations; and • can be performed with conjugate heat transfer or fluid-structure interaction. # Incompressible fluid dynamic analysis 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. You can perform a transient or steady-state incompressible flow analysis. Input File Usage: Use the following option for a transient incompressible flow analysis: \*CFD, INCOMPRESSIBLE NAVIER STOKES Use the following option for a steady-state incompressible flow analysis: \*CFD, INCOMPRESSIBLE NAVIER STOKES, STEADY STATE Abaqus/CAE Usage: In Abaqus/CAE you can only define a transient incompressible flow analysis. Step module: Create Step: General: Flow; Flow type: Incompressible # Governing equations The unsteady momentum equations in integral form for an arbitrary control volume can be written as $$ \frac {d}{d t} \int_ {V} \rho \mathbf {v} d V + \int_ {S} \rho \mathbf {v} \otimes (\mathbf {v} - \mathbf {v} _ {m}) \cdot \mathbf {n} d S = - \int_ {V} \nabla p d V + \int_ {S} \pmb {\tau} \cdot \mathbf {n} d S + \int_ {V} \mathbf {f} d V. $$ For steady state the integral form of the momentum conservation equation becomes $$ \int_ {S} \rho \mathbf {v} \otimes \mathbf {v} \cdot \mathbf {n} d S = - \int_ {V} \nabla p d V + \int_ {S} \pmb {\tau} \cdot \mathbf {n} d S + \int_ {V} \mathbf {f} d V, $$ where $V$ is an arbitrary control volume with surface area $S$ , $\mathbf{n}$ is the outward normal to $S$ , $\rho$ is the fluid density, $p$ is the pressure, $\mathbf{v}$ is the velocity vector, $\mathbf{v}_m$ is the velocity of the moving mesh, $\mathbf{f}$ is the body force, and $\tau$ is the viscous shear stress. The viscous shear stress, $\tau ,$ is also referred to as the deviatoric stress, $\mathbf { S } ,$ where ${ \bf S } = \eta \dot { \gamma }$ . For more information, see “Viscosity,” Section 26.1.4. Incompressibility requires a solenoidal velocity field expressed by $$ \nabla \cdot \mathbf {v} = \mathbf {0}. $$ # Numerical implementation 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 the integral form of the conservation equations. For time-dependent problems, an advanced second-order projection method is used for an arbitrary deforming domain. For steady state the solution approach is based on a SIMPLE algorithm on a fixed mesh. For both the projection and SIMPLE algorithms, a node-centered finite-element discretization for the pressure and a cell-centered finite volume discretization of all the other transported variables (such as velocity, temperature, turbulence, etc.) are adopted. This hybrid approach guarantees accurate solutions and eliminates the possibility of spurious pressure modes (without the need for any artificial dissipation) 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. # Projection method (for transient analysis) The basic concept for projection methods is the legitimate segregation of pressure and velocity fields for efficient solution of the incompressible Navier-Stokes equations. Over the past two decades, projection methods have found broad application for problems involving laminar and turbulent fluid dynamics, large density variations, chemical reactions, free surfaces, mold filling, and non-Newtonian behavior. In practice, the projection is used to remove the part of the velocity field that is not divergencefree (“div-free”). The projection is achieved by splitting the velocity field into div-free and curl-free components using a Helmholtz decomposition. The projection operators are constructed so that they satisfy prescribed boundary conditions and are norm-reducing, resulting in a robust solution algorithm for incompressible flows. # SIMPLE method (for steady-state analysis) The SIMPLE (Semi-Implicit Method for Pressure Linked Equations) method is a pressure-based method developed to efficiently simulate steady-state flows. The primary idea behind the SIMPLE method is to create a discrete pressure correction equation by enforcing mass continuity over each cell. The divergence-free velocity field is then obtained by relating the discrete pressure correction (and, hence, the discrete pressure) field with the discrete form of the momentum equations. # Least-squares gradient estimation The solution methods in Abaqus/CFD use a linearly complete second-order accurate least-squares gradient estimation. This permits accurate evaluation of dual-edge fluxes for both advective and diffusive processes. All transport equations in Abaqus/CFD make use of the second-order least-squares operators. # Advection methods The advection treatment in Abaqus/CFD is edge-based, monotonicity-preserving, and preserves smooth variations to second order in space. The advection algorithm relies on a least-squares gradient estimation with unstructured-grid slope limiters that are topology independent. Sharp gradients are captured within approximately 2–3 elements; i.e., , and the use of slope limiting in conjunction with a local diffusive limiter precludes over-/under-shoots in advected fields. For the transient solver, the advection terms in the momentum and transport equations can be treated either explicitly or implicitly (see the discussion in “Time incrementation” below). # Energy equation 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 transient form of the energy equation, in temperature form, can be obtained from the first law of thermodynamics and is given by $$ \frac {d}{d t} \int_ {V} \rho C _ {p} \theta d V + \int_ {S} \rho C _ {p} \theta (\mathbf {v} - \mathbf {v} _ {m}) \cdot \mathbf {n} d S = \int_ {V} r d V - \int_ {S} \mathbf {q} \cdot \mathbf {n} d S. $$ For steady state it is given by $$ \int_ {S} \rho C _ {p} \theta \mathbf {v} \cdot \mathbf {n} d S = \int_ {V} r d V - \int_ {S} \mathbf {q} \cdot \mathbf {n} d S, $$ where $C _ { p }$ is the constant pressure specific heat, is the temperature, is heat flux due to conduction defined by Fourier’s law, and is the heat supplied externally into the body per unit volume. The energy equation is solved in terms of temperature in Abaqus/CFD. Input File Usage: Use the following option to specify an isothermal flow problem (default): \*CFD, ENERGY EQUATION=NO ENERGY Use the following option to specify a thermal (heat) transport problem with temperature as the primary transport scalar variable: \*CFD, ENERGY EQUATION=TEMPERATURE Abaqus/CAE Usage: Use the following option to specify an isothermal flow problem: Step module: Create Step: General: Flow; Basic tabbed page: Energy equation: None Use the following option to specify a thermal (heat) transport problem with temperature as the primary transport scalar variable: Step module: Create Step: General: Flow; Basic tabbed page: Energy equation: Temperature # Turbulence models 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 in Abaqus/CFD: Spalart-Allmaras (SA), k– RNG, k– realizable, and $\pmb { k } \mathrm { - } \omega$ SST. These models span a relatively broad set of flow problems that include steady-state and 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 can 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 transient form of the turbulent viscosity transport equation for the Spalart-Allmaras model is given by $$ \begin{array}{l} \frac {d}{d t} \int_ {V} \rho \widetilde {\nu} d V + \int_ {S} \rho \widetilde {\nu} (\mathbf {v} - \mathbf {v} _ {m}) \cdot \mathbf {n} d S = \int_ {V} \rho c _ {b 1} \widetilde {S} \widetilde {\nu} d V - \int_ {V} \rho c _ {w 1} f _ {w} \left(\frac {\widetilde {\nu}}{d}\right) ^ {2} d V \\ + \int_ {V} \frac {\rho (1 + c _ {b 2})}{\sigma} \nabla \cdot \{(\nu + \widetilde {\nu}) \nabla \widetilde {\nu} \} d V - \int_ {V} \frac {\rho c _ {b 2}}{\sigma} (\nu + \widetilde {\nu}) \nabla \cdot \nabla \widetilde {\nu} d V. \\ \end{array} $$ The steady-state form of the equation is given by $$ \begin{array}{l} \int_ {S} \rho \widetilde {\nu} \mathbf {v} \cdot \mathbf {n} d S = \int_ {V} \rho c _ {b 1} \widetilde {S} \widetilde {\nu} d V - \int_ {V} \rho c _ {w 1} f _ {w} \left(\frac {\widetilde {\nu}}{d}\right) ^ {2} d V \\ + \int_ {V} \frac {\rho (1 + c _ {b 2})}{\sigma} \nabla \cdot \{(\nu + \widetilde {\nu}) \nabla \widetilde {\nu} \} d V - \int_ {V} \frac {\rho c _ {b 2}}{\sigma} (\nu + \widetilde {\nu}) \nabla \cdot \nabla \widetilde {\nu} d V. \\ \end{array} $$ The damping functions and model coefficients used in the above two equations are defined as: $$ f _ {w} = g \left(\frac {1 + c _ {w 3} ^ {6}}{g ^ {6} + c _ {w 3} ^ {6}}\right) ^ {\frac {1}{6}}, $$ $$ f _ {v 1} = \frac {\chi^ {3}}{\chi^ {3} + c _ {v 1} ^ {3}}, $$ $$ f _ {v 2} = 1 - \frac {\chi}{1 + \chi f _ {v 1}}, $$ $$ \chi = \frac {\widetilde {\nu}}{\nu}, $$ $$ g = r + c _ {w 2} (r ^ {6} - r), $$ $$ r = \frac {\widetilde {\nu}}{\widetilde {S} \kappa^ {2} d ^ {2}}, $$ $$ \widetilde {S} = S + \frac {\widetilde {\nu}}{\kappa^ {2} d ^ {2}} f _ {v 2}, $$ $$ S = \sqrt {2 R _ {i j} R _ {i j}}, $$ $$ R _ {i j} = \frac {1}{2} \left(\frac {\partial u _ {i}}{\partial x _ {j}} - \frac {\partial u _ {j}}{\partial x _ {i}}\right), $$ where is the normal distance from the wall, and the effective turbulent viscosity is defined as $$ \nu_ {t} = \widetilde {\nu} f _ {v 1}. $$ The Spalart-Allmaras model coefficients are shown in Table 6.6.2–1. In addition, a turbulent Prandtl number, $P r _ { t }$ , can be specified. Table 6.6.2–1 Spalart-Allmaras model coefficients.

$c_{b1}$	$c_{b2}$	$c_{v1}$	$\sigma$	$c_{w1}$	$c_{w2}$	$c_{w3}$	$\kappa$	$c_{v2}$
0.1355	0.622	7.1	0.6667	$\frac{c_{b1}}{\kappa^{2}}+\frac{1+c_{b2}}{\sigma}$	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: Use both of the following options: \*CFD \*TURBULENCE MODEL, TYPE=SPALART ALLMARAS Abaqus/CAE Usage: Step module: Create Step: General: Flow; Turbulence tabbed page: Spalart-Allmaras