Products: Abaqus/CFD Abaqus/CAE
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 
);
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 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.
| Input File Usage: | *CFD, INCOMPRESSIBLE NAVIER STOKES |
| Abaqus/CAE Usage: | Step module: Create Step: General: Flow; Flow type: Incompressible |
The momentum equations in integral form for an arbitrary control volume can be written as
is an arbitrary control volume with surface area 
,
is the outward normal to ,
is the fluid density,
is the pressure,
is the velocity vector,
is the velocity of the moving mesh,
is the body force, and
is the viscous shear stress.
, is also referred to as the deviatoric stress, 
, where 
. For more information, see “Viscosity,” Section 25.1.4.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 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 divergence-free (“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.
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.
The implementation of advection in Abaqus/CFD is edge-based, monotonicity-preserving, and preserves smooth variations to second order in space. The advection 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. The advection is treated explicitly (see the stability discussion in “Time incrementation” below).
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
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.| 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 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).
Large-eddy simulation relies on a segregation of length and time scales in turbulent flows and a modeling approach that permits the direct simulation of grid-resolved flow structures and the modeling of unresolved subgrid features. Implicit LES is a methodology for modeling high Reynolds number flows that combines computational efficiency and ease of implementation with predictive calculations and flexible application. In Abaqus/CFD ILES relies on the discrete monotonicity-preserving form of the advective operator to implicitly define the subgrid-scale model. This model is inherently time-dependent requiring time-accurate solutions to the incompressible Navier-Stokes equations where the time scale is approximately that of an eddy-turnover time for resolve-scale flow features. In addition, this model must be run in full three dimensions, which typically imposes larger grid densities and stringent grid resolution criteria relative to more traditional steady-state RANS simulations. However, this approach is extremely flexible and can be applied to a broad range of flows and FSI problems. There are no user settings required for ILES.
| Input File Usage: | Use the *CFD option without the *TURBULENCE MODEL option. |
| Abaqus/CAE Usage: | Step module: Create Step: General: Flow; Turbulence tabbed page: None |
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
is the normal distance from the wall, and the effective turbulent viscosity is defined as
) can be specified.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 |
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
is
transport equations above represent the production and dissipation of k and , respectively. The RNG k– model coefficients are shown in Table 6.6.2–2. In addition, a turbulent Prandtl number () can be specified.
| Input File Usage: | Use both of the following options: |
*CFD *TURBULENCE MODEL, TYPE=RNG KEPSILON |
| Abaqus/CAE Usage: | Step module: Create Step: General: Flow; Turbulence tabbed page: k-epsilon renormalization group (RNG) |
It is well known that the k– model has limitations, especially on wall-bounded flows where high values of eddy viscosity in the near-wall region are usually reproduced. For high Reynolds number flows often encountered in many industrial applications, a full resolution of the thin viscous sub-layer that occurs near a wall using a fine mesh may not be economical. Consequently, for meshes that cannot resolve the viscous sub-layer, wall functions are used to represent the effects of the viscous sub-layer on the transport processes. In Abaqus/CFD wall functions are used to avoid the need for highly resolved boundary layer meshes. This approach relies on the law of the wall to obtain the wall shear stress.
The law of the wall is a universal velocity profile that wall-bounded flows develop in the absence of pressure gradients. The law of the wall is
is the wall tangent velocity, 
is the kinematic viscosity, is the density, 
is the shear stress at the wall, and 
and 
are constants. The standard law of the wall profile is limited in its usage. For example, in recirculating flows the turbulent kinetic energy k becomes zero at separation and reattachment points, where, by definition, 
is zero. This singular behavior causes the predicted results to be erroneous. To overcome this, the standard law of the wall is modified based on a new scale for the friction velocity following the method proposed by Launder and Spalding (1974). The modified friction velocity is given by
The modified law of the wall reduces to the standard law of the wall under the conditions of uniform wall shear stress, and when the generation and dissipation of turbulent kinetic energy are in balance (i.e., when the turbulence structure is in equilibrium). Under such conditions, 
and thus, 
.
The wall shear stress for the modified law of the wall can be evaluated as (Albets-Chico, et al., 2008)
for the wall layer of elements. Specifically, the production and dissipation terms in the governing transport equation for the turbulent kinetic energy k are modified to account for the presence of the wall. Following the procedure outlined in (Craft et al., 2002), an average value of the production of k as given below is used in the transport equation. Such an average is obtained based on a two-layer model of the wall element (i.e., the wall element is divided into a partly viscous sub-layer region and a partly turbulent log-layer or inertial layer region).
is the maximum of the wall normal distances of all the vertices of a given wall element, and 
is the wall normal distance of the edge of the viscous sub-layer, where
Similarly, an average value of the dissipation rate for k is also prescribed for the wall elements based on a two-layer integration and is given by
The transport equation for is not solved for the wall layer elements. Instead, the value of is directly prescribed at the point p as follows:
transport equations is performed with a zero-flux (i.e., homogeneous Neumann boundary conditions) at the walls.The main advantage of wall functions is the relaxed requirement on mesh resolution at walls. However, the main disadvantage of using wall functions is the dependence on the near-wall mesh resolution. Wall functions based on the law of the wall approach usually work best for wall elements whose centers lie in the fully turbulent layer (inertial or log layer) for which such functions are designed. This effectively imposes a lower limit on the value of the scaled wall coordinate, 
. For complex geometries, ensuring that all the near wall cells are outside the viscous sublayer is difficult. The precise location of the logarithmic region is solution dependent and may vary with time. To accommodate a more flexible mesh, a resolution-insensitive wall function (Durbin, 2009) has been implemented. Briefly, this wall function is based on limiting the minimum value of such that the value of the velocity gradient at the first wall-attached element is the same as if it was located on the edge of the viscous sub-layer. A best practice for wall-bounded flows is to have at least 8–10 points in the boundary layer region where 
(see Casey and Wintergerste, 2000).
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. Abaqus/CFD offers distortion control to prevent elements from inverting or distorting excessively in fluid mesh movement (see “Controlling the solution accuracy in an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation” in “Commonly used control parameters,” Section 7.2.2).
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.
| Input File Usage: | Use the following option to specify parameters for solving the momentum transport equations: |
*MOMENTUM EQUATION SOLVER Use the following option to specify parameters for solving other transport equations, such as the energy or turbulence transport equations: *TRANSPORT EQUATION SOLVER Use the following option to specify parameters for solving the pressure equation: *PRESSURE EQUATION SOLVER |
Iterative solvers compute an approximate solution to a given set of equations; therefore, convergence criteria are required to determine if the solution is acceptable. While default settings should be adequate for most problems, you can modify the convergence criteria. In addition to the option of setting convergence criteria, convergence history output is available that may be useful for some advanced users to tune the solvers for performance or robustness. For the algebraic multigrid preconditioner, diagnostic information such as the number of grids, grid sparsity, and largest eigenvalue and condition number estimates are available upon request. The diagnostic information for the algebraic multigrid preconditioner is printed every time the preconditioner is computed.
The linear convergence limit (also commonly referred to as the convergence tolerance), the frequency of convergence checking, and the maximum number of iterations can be set. The iterative solver will stop when the relative residual norm of the system of equations and the relative correction of the solution norm fall below the convergence limit.
| Input File Usage: | Use the following options to specify convergence criteria for the momentum and auxiliary transport equations: |
*MOMENTUM EQUATION SOLVER max iterations, frequency check, convergence limit *TRANSPORT EQUATION SOLVER max iterations, frequency check, convergence limit *PRESSURE EQUATION SOLVER max iterations, frequency check, convergence limit |
| Abaqus/CAE Usage: | Step module: Create Step: General: Flow; Solvers tabbed page: Momentum Equation, Pressure Equation, or Transport Equation tabbed page; enter values for Iteration limit, Convergence checking frequency, and Linear convergence limit |
You can monitor the convergence of the iterative solver by accessing convergence output. When you activate the convergence output, the current relative residual norm and the relative solution correction norm are output each time the convergence is checked.
| Input File Usage: | Use the following options to write convergence output to the log file for the linear equation solvers: |
*MOMENTUM EQUATION SOLVER, CONVERGENCE=ON *TRANSPORT EQUATION SOLVER, CONVERGENCE=ON *PRESSURE EQUATION SOLVER, CONVERGENCE=ON |
| Abaqus/CAE Usage: | Step module: Create Step: General: Flow; Solvers tabbed page: Momentum Equation, Pressure Equation, or Transport Equation tabbed page; toggle on Include convergence output |
Diagnostic output is useful only for the algebraic multigrid preconditioner. For other preconditioners, only a solver initialization message is printed for diagnostic output. For the algebraic multigrid preconditioner, the number of grids, grid sparsity, and largest eigenvalue and condition number estimates are output each time the preconditioner is computed.
| Input File Usage: | Use the following option to write diagnostic output to the log file for the pressure equation solver using the algebraic multigrid preconditioner: |
*PRESSURE EQUATION SOLVER, TYPE=AMG, DIAGNOSTICS=ON |
| Abaqus/CAE Usage: | Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page; toggle on Include diagnostic output |
Three solver types are available for the solving the pressure equation. The default AMG solver uses an algebraic multigrid preconditioner and offers the choice of three Krylov solvers: conjugate gradient, bi-conjugate gradient stabilized, and flexible generalized minimal residual. The SSORCG solver uses a symmetric successive over-relaxation preconditioner and conjugate gradient Krylov solver. The DSCG solver uses a diagonally scaled preconditioner and conjugate gradient Krylov solver. The AMG solver provides many additional options that are intended for advanced usage and in cases where convergence difficulties are encountered.
| Input File Usage: | Use one of the following options to specify the solver type: |
*PRESSURE EQUATION SOLVER, TYPE=AMG (default) *PRESSURE EQUATION SOLVER, TYPE=SSORCG *PRESSURE EQUATION SOLVER, TYPE=DSCG |
| Abaqus/CAE Usage: | Use the following option to specify the AMG solver: |
Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Use analysis defaults Use the following option to specify the SSORCG solver: Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Specify, Preconditioner Type: Symmetric successive over-relaxation The DSCG solver is not supported in Abaqus/CAE. |
For the AMG solver, you can choose from three preset levels or you can specify the Krylov solver and smoother settings directly. The presets are provided for convenience. Preset level 1 is primarily intended for use with meshes with good element aspect ratios and in some cases may provide a performance benefit over the default preset level 2. Preset level 3 is intended for problems that encounter convergence difficulties, which typically have elements with high aspect ratios or highly distorted elements.
| Input File Usage: | Preset level 1 corresponds to the following: |
*PRESSURE EQUATION SOLVER, TYPE=AMG 250, 2, 10–5 CHEBYCHEV, 2, 2, CG V Preset level 2 (default) corresponds to the following: *PRESSURE EQUATION SOLVER, TYPE=AMG 250, 2, 10–5 ICC, 1, 1, CG V Preset level 3 corresponds to the following: *PRESSURE EQUATION SOLVER, TYPE=AMG 250, 2, 10–5 ICC, 2, 2, BCGS V |
| Abaqus/CAE Usage: | Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Specify, Preconditioner Type: Algebraic multi-grid |
Use one of the following options to choose a preset complexity level: Complexity Level: Preset: 1, 2, or 3 Use the following option to specify the Krylov solver and smoother settings directly: Complexity Level: User defined |
Three Krylov solver options are provided for the AMG solver. The default conjugate gradient solver is the fastest; however, in some cases where convergence difficulties are observed, the bi-conjugate gradient stabilized or flexible generalized minimal residual solvers are recommended. These two solvers are more robust but computationally more expensive than the conjugate gradient solver.
| Input File Usage: | Use the following option to specify the Krylov solver type: |
*PRESSURE EQUATION SOLVER, TYPE=AMG first data line , , , solver type where solver type is CG for the conjugate gradient solver (default), BCGS for the bi-conjugate gradient squared solver, and FGMRES for the flexible generalized minimum residual solver. |
| Abaqus/CAE Usage: | Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Specify, Preconditioner Type: Algebraic multi-grid |
Use one of the following options to specify the Krylov solver: Solver Type: Conjugate gradient, Bi-conjugate gradient, stabilized, or Flexible generalized minimal residual |
You can choose between incomplete factorization and polynomial residual smoothers that are used within the AMG preconditioner. While incomplete factorization is computationally more expensive than polynomial smoothing, in many cases this cost is amortized by fast convergence and robustness. Polynomial smoothing is recommended for problems with a very good mesh quality (i.e., no skewed or large aspect ratio elements). The number of pre- and post-smoothing sweeps can also be specified. It is recommended that you apply the same number of pre- and post-sweeps. For the polynomial smoother, a minimum of two pre- and post-sweeps are recommended.
| Input File Usage: | Use the following option to specify the residual smoother settings: |
*PRESSURE EQUATION SOLVER, TYPE=AMG first data line smoother, pre-smoothing sweeps, post-smoothing sweeps |
| Abaqus/CAE Usage: | Step module: Create Step: General: Flow; Solvers tabbed page: Pressure Equation tabbed page: Solver options: Specify, Preconditioner Type: Algebraic multi-grid, Residual Smoother: Incomplete factorization or Polynomial, Pre-sweeps: select number, Post-sweeps: select number |
Abaqus/CFD relies on a second-order semi-implicit projection method for time-dependent problems. By default, all viscous/diffusive terms and boundary conditions are treated with a second-order accurate trapezoid rule (Crank-Nicolson method), while the advective terms are currently treated explicitly. Alternatively, the use of a Galerkin or backward-Euler integrator can be selected for the viscous/diffusive terms and boundary conditions. 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.
| Input File Usage: | Use the following option to specify automatic time incrementation (default): |
*CFD, INCREMENTATION=FIXED CFL time increment, time period, scale factor, suggested CFL, check increment divergence tolerance, Use the following option to specify fixed time step incrementation: *CFD, INCREMENTATION=FIXED STEP SIZE time increment, time period divergence tolerance, For both options above, |
| Abaqus/CAE Usage: | Use the following options to specify automatic time incrementation: |
Step module: Create Step: General: Flow; Basic tabbed page: enter a value for Time period; Incrementation tabbed page: Type: Automatic (Fixed CFL); enter values for Initial time increment, Maximum CFL number, Increment adjustment frequency, Time step growth scale factor, Divergence tolerance Use the following option to specify fixed time step incrementation: Step module: Create Step: General: Flow; Basic tabbed page: enter a value for Time period; Incrementation tabbed page: Type: Fixed, enter values for Time increment and Divergence tolerance Use the following options to specify the time integration method for viscous/diffusive terms and boundary conditions: Viscous or Load/Boundary condition: Trapezoid (1/2), Galerkin (2/3), or Backward-Euler (1) |
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 written to the status (.sta) file and can be examined as the analysis job is executing. The RMS divergence output variable is useful for determining if a calculation is proceeding normally. Values of the RMS divergence output variable that are O(1) can 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; i.e., when the kinetic energy asymptotically approaches a constant value, the flow is typically achieving a steady-state condition where the velocities and pressure do not vary in time. Alternatively, the global kinetic energy can indicate a steady-periodic or chaotic flow situation as well.
Initial conditions for the density, velocity, temperature, turbulent eddy viscosity, turbulent kinetic energy, and dissipation rate can be specified (see “Initial conditions in Abaqus/CFD,” Section 32.2.2). If the density is omitted, the specified material density is used for incompressible flow simulations.
For a well-posed incompressible flow problem, the initial velocity must satisfy the boundary conditions and also the imposed divergence-free condition; i.e., the solvability conditions. Abaqus/CFD automatically uses the user-defined boundary conditions and tests the specified velocity initial conditions to be sure the solvability conditions are satisfied. If they are not, the initial velocity is projected onto a divergence-free subspace, yielding initial conditions that define a well-posed incompressible Navier-Stokes problem. Therefore, in some circumstances, user-specified velocity initial conditions may be overridden with velocity conditions that satisfy solvability.
Boundary conditions for velocity, temperature, pressure, and eddy viscosity can be defined (see “Boundary conditions in Abaqus/CFD,” Section 32.3.2). During the analysis prescribed boundary conditions can be varied using an amplitude definition (see “Amplitude curves,” Section 32.1.2). All amplitude definitions except smooth step and solution-dependent amplitudes are available. By default, all boundary conditions are applied instantaneously.
Displacement and velocity boundary conditions at FSI interfaces are prescribed automatically by the definition of a co-simulation region; therefore, you should not prescribe these conditions at an FSI interface. Similarly, you should not define the temperature at a CHT interface; the temperature is automatically prescribed by the definition of a co-simulation region. For more information, see “Preparing an Abaqus analysis for co-simulation,” Section 16.1.2.
The specification of no-slip/no-penetration boundary conditions at walls requires the specification of the turbulent eddy viscosity and normal-distance function, which is handled automatically by Abaqus/CFD.
In incompressible flows, the pressure is only known within an arbitrary additive constant value or the hydrostatic pressure. In many practical situations, the pressure at an outflow boundary may be prescribed, which, in effect, sets the hydrostatic pressure level. In cases where there is no pressure prescribed, it is necessary to set the hydrostatic pressure level at a minimum of one node in the mesh.
The fluid reference pressure can be used to specify the hydrostatic pressure level. When there are no prescribed pressure boundary conditions, the fluid reference pressure establishes the hydrostatic pressure level and makes the pressure-increment equation non-singular. If pressure boundary conditions are prescribed in addition to the reference pressure level, the reference pressure simply adjusts the output pressures according to the specified pressure level. For more information, see “Specifying a fluid reference pressure” in “Concentrated loads,” Section 32.4.2.
The loading types for Abaqus/CFD include applied heat flux, volumetric heat-generation sources, general body forces, and gravity loading. Gravity loading defines the gravity vector used with a Boussinesq-type body force in buoyancy driven flow (see “Specifying gravity loading” in “Distributed loads,” Section 32.4.3). Gravity loading can be used only in conjunction with the energy equation and will be ignored if used without the energy equation. During the analysis prescribed loads can be varied using an amplitude definition (see “Amplitude curves,” Section 32.1.2). All amplitude definitions except smooth step and solution-dependent amplitudes are available.
Material definitions in Abaqus/CFD follow the Abaqus conventions but also present several material properties specific to fluid dynamics. In Abaqus/CFD the typical material properties include viscosity, constant-pressure specific heat, density, and coefficient of thermal expansion. The thermal expansion is used with a Boussinesq-type body force in buoyancy driven flow.
In contrast to Abaqus/Standard and Abaqus/Explicit, which use the constant-volume specific heat, the constant-pressure specific heat is required when the energy equation is used for thermal-flow problems. For problems involving an ideal gas, the user may optionally specify constant-volume specific heat and the ideal gas constant.
Abaqus/CFD supports three element types: the 8-node hexahedral element, FC3D8; the 6-node triangular prism element, FC3D6; and the 4-node tetrahedral element, FC3D4 (see “Fluid (continuum) elements,” Section 27.2.1). These elements cannot be mixed in a single connected fluid domain. However, a single flow model can contain multiple domains, each with a different element type.
The output available from Abaqus/CFD for an incompressible fluid dynamic analysis includes both nodal and surface field data and element and surface time-history data. For the nodal and element output, the preselected field and history data include velocity (V), temperature (TEMP), pressure (PRESSURE), and turbulent eddy viscosity (TURBNU). In addition, preselected field data include displacement (U). Preselected data are not available for surface output.
In addition to the preselected output, you can request several derived and auxiliary variables. All of the output variable identifiers are outlined in “Abaqus/CFD output variable identifiers,” Section 4.2.3.
*HEADING … *NODE … *ELEMENT, TYPE=FC3D4 … *MATERIAL, NAME=matname *CONDUCTIVITY Data lines to define the thermal conductivity *DENSITY Data lines to define the fluid density *SPECIFIC HEAT, TYPE=CONSTANT PRESSURE Data lines to define the specific heat *VISCOSITY Data lines to define the fluid viscosity *INITIAL CONDITIONS, TYPE=TEMPERATURE, ELEMENT AVERAGE Data lines to prescribe initial temperatures at the elements *INITIAL CONDITIONS, TYPE=VELX, ELEMENT AVERAGE Data lines to prescribe initial x-velocity at the elements *INITIAL CONDITIONS, TYPE=VELY, ELEMENT AVERAGE Data lines to prescribe initial y-velocity at the elements *INITIAL CONDITIONS, TYPE=VELY, ELEMENT AVERAGE Data lines to prescribe initial y-velocity at the elements … *AMPLITUDE, NAME=velxamp, DEFINITION=TABULAR Data lines to define amplitude curve to be used for inlet x-velocity ** *STEP ** Incompressible flow example *CFD, INCOMPRESSIBLE NAVIER STOKES, INCREMENTATION=FIXED CFL Data lines to define incrementation ** ** Boundary conditions ** *FLUID BOUNDARY, TYPE=SURFACE inlet_surface, VELX, value for x-velocity inlet_surface, VELY, value for y-velocity inlet_surface, VELZ, value for z-velocity ** *FLUID BOUNDARY, TYPE=SURFACE temperature_surface, TEMP, value for temperature ** *FLUID BOUNDARY, TYPE=SURFACE outlet_surface, P, value for pressure ** ** Field output ** *OUTPUT, FIELD, TIME INTERVAL=interval for field output *ELEMENT OUTPUT PRESSURE, TEMP, TURBNU, V *NODE OUTPUT PRESSURE, TEMP, TURBNU, V ** ** History output ** *OUTPUT, HISTORY, FREQUENCY=interval for history output *ELEMENT OUTPUT, ELSET=element set for history output, FREQUENCY=SURFACE … *END STEP
Albets-Chico, X., C. D. Perez-Segarra, A. Olivia, and J. Bredberg, “Analysis of Wall-Function Approaches using Two-Equation Turbulence Models,” International Journal of Heat and Mass Transfer, vol. 51 4940–4957, 2008.
Casey, M., and T. Wintergerste, ERCOFTAC Special Interest Group on “Quality and Trust in Industrial CFD”, European Research Community on Flow, Turbulence and Combustion (ERCOFTAC), 2000.
Craft, T. J., A. V. Gerasimov, H. Iacovides, and B. E. Launder, “Progress in the Generalization of Wall-Function Treatments,” International Journal of Heat and Fluid Flow, vol. 23 148–160, 2002.
Durbin, P. A., “Limiters and wall treatments in applied turbulence modeling,” Fluid Dynamics research, vol. 41 1–17, 2009.
Launder, B. E., and D. B. Spalding, “The Numerical Computation of Turbulent Flows,” Computer Methods in Applied Mechanics and Engineering, vol. 3 269–289, 1974.
Yakhot, V., S. A. Orszag, S. Thangam, T. B. Gatski, and C. G. Speziale, “Development of Turbulence Models for Shear Flows by a Double Expansion Technique,” Physics of Fluids A, vol. 4, no.7 1510–1520, 1992.
