Products: Abaqus/CFD Abaqus/CAE
Boundary conditions:
are used to prescribe the values of all primitive variables involved in a fluid dynamics calculation (e.g., velocities, temperatures, turbulence variables, wall-normal distance, etc.);
can be given as “history” input data (within an analysis step) to add, modify, or remove zero-valued or nonzero boundary conditions; and
can be prescribed through the use of a co-simulation region for multiphysics problems.
Combinations of boundary conditions that represent a physical type (for example, an inflow, outflow, or wall behavior) are grouped collectively for ease of use. For more information on Abaqus/CAE groupings, see “Using the boundary condition editors,” Section 16.10 of the Abaqus/CAE User's Guide.
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. You specify a boundary condition type and physical type for a fluid boundary condition. Boundary conditions and the analysis procedure and additional options required for activation, if any, are listed in Table 34.3.2–1.
Table 34.3.2–1 Surface-based fluid boundary conditions and activation options.
| Boundary condition type | Description | Incompressible flow | Physical type |
|---|---|---|---|
| TEMP | Fluid temperature | Energy equation | Velocity inlet, pressure outlet, slip wall, no-slip/no-penetration wall |
| TURBEPS | Turbulent energy dissipation rate ( ) |  - RNG and realizable models | Velocity inlet, pressure outlet, slip wall |
| TURBKE | Turbulent kinetic energy () | - SST and - RNG and realizable models | Velocity inlet, pressure outlet, slip wall |
| TURBOMEGA | Specific energy dissipation rate () | - SST model | Velocity inlet, pressure outlet, slip wall |
| TURBNU | Turbulent kinematic eddy viscosity | Spalart-Allmaras model | Velocity inlet, pressure outlet, slip wall |
| TURBINTENSITY | Turbulence intensity | Spalart-Allmaras, - SST, and - RNG and realizable models | Velocity inlet, pressure outlet, slip wall |
| TURBLENGTHSCALE | Turbulent length scale | Spalart-Allmaras, - SST, and - RNG and realizable models | Velocity inlet, pressure outlet, slip wall |
| TURBVISCOSITYRATIO | Eddy to molecular viscosity ratio | Spalart-Allmaras, - SST, and - RNG and realizable models | Velocity inlet, pressure outlet, slip wall |
| VELX | x-velocity | — | Velocity inlet, slip wall |
| VELY | y-velocity | — | Velocity inlet, slip wall |
| VELZ | z-velocity | — | Velocity inlet, slip wall |
| VELN | Normal velocity | — | Velocity inlet |
| VELXNU | x-velocity defined via user subroutine | — | Velocity inlet, slip wall |
| VELYNU | y-velocity defined via user subroutine | — | Velocity inlet, slip wall |
| VELZNU | z-velocity defined via user subroutine | — | Velocity inlet, slip wall |
| PASSIVEOUTFLOW | Passive outflow | — | Pressure outlet |
| P | Fluid pressure | — | Pressure outlet |
| PNU | Fluid pressure defined via user subroutine | — | Pressure outlet |
You can specify boundary conditions to describe the flow behavior where fluid enters the analysis domain (velocity inlet) and where the fluid leaves the analysis domain (pressure outlet).
An inflow boundary condition is used to describe the flow behavior at a surface where fluid enters the analysis domain. For incompressible flows, inflow conditions can be prescribed for velocity or pressure, temperature, and turbulence variables.
You can specify an amplitude curve (see “Amplitude curves,” Section 34.1.2) to define the time variation of changes in the inflow behavior.
| Input File Usage: | Use the following option to define inflow boundary conditions at surfaces: |
*FLUID BOUNDARY, VELOCITY INLET, SURFACE=surface name boundary condition type label, magnitude or distribution name, amplitude name where boundary condition type label is VELX, VELY, VELZ, VELN, VELXNU, VELYNU, VELZNU, TEMP, TURBKE, TURBEPS, TURBOMEGA, TURBNU, TURBINTENSITY, TURBLENGTHSCALE, or TURBVISCOSITYRATIO. |
| Abaqus/CAE Usage: | Use the following option to define the inflow boundary conditions at surfaces: |
Load module: Create Boundary Condition: Step: flow_step: Category: Fluid: Fluid inlet/outlet: select inlet regions; and specify momentum (pressure or velocity), thermal energy (temperature), and turbulence conditions at the inlet or outlet Specifying the specific energy dissipation rate, turbulence intensity, turbulent length scale, and eddy to molecular viscosity ratio is not supported in Abaqus/CAE. |
An outflow boundary corresponds to a surface where the fluid flow leaves the analysis domain. In Abaqus/CFD outflow conditions are associated with a specified pressure. However, many other flow variables can be prescribed at an outflow boundary as well.
You can specify an amplitude curve (see “Amplitude curves,” Section 34.1.2) to define the time variation of changes in the outflow behavior.
| Input File Usage: | Use the following option to define outflow pressure boundary conditions at surfaces: |
*FLUID BOUNDARY, PRESSURE OUTLET, SURFACE=surface name boundary condition type label, magnitude or distribution name, amplitude name where boundary condition type label is P, PNU, PASSIVEOUTFLOW, TEMP, TURBKE, TURBEPS, TURBOMEGA, TURBNU, TURBINTENSITY, TURBLENGTHSCALE, or TURBVISCOSITYRATIO. The values of magnitude and amplitude name are ignored for PASSIVEOUTFLOW. |
| Abaqus/CAE Usage: | Use the following option to define the outflow boundary conditions at surfaces: |
Load module: Create Boundary Condition: Step: flow_step: Category: Fluid: Fluid inlet/outlet: select outlet regions; and specify momentum (pressure or velocity), thermal energy (temperature), and turbulence conditions at the inlet or outlet Specifying the specific energy dissipation rate, turbulence intensity, turbulent length scale, and eddy to molecular viscosity ratio is not supported in Abaqus/CAE. |
Wall boundary conditions are typically associated with the no-slip/no-penetration behavior at a solid surface. However, the behavior at a solid wall may also require the prescription of temperature and, optionally, turbulence variables depending on the flow conditions. In situations where a wall heat flux is required, a heat flux loading must be prescribed in addition to the wall boundary conditions.
Depending on the physical properties of the wall, the wall boundary conditions can be modified to achieve a variety of physical behaviors that include slip, no-slip, infiltration, symmetry, etc.
A no-slip (and no-penetration) wall is a surface where the fluid adheres to the wall without penetrating it. The velocity components at the wall are all set to zero, unless the wall is moving. The boundary conditions for the different turbulence variables are implemented automatically by the solver.
You can specify an amplitude curve (see “Amplitude curves,” Section 34.1.2) to define the time variation of changes in the wall boundary conditions.
| Input File Usage: | Use the following option to define no-slip/no-penetration wall boundary conditions at surfaces: |
*FLUID BOUNDARY, WALL, SURFACE=surface name, SLIP=NO (default) boundary condition type label, magnitude or distribution name, amplitude name where boundary condition type label is TEMP. |
| Abaqus/CAE Usage: | Use the following option to define no-slip/no-penetration wall boundary conditions at surfaces: |
Load module: Create Boundary Condition: Step: flow_step: Category: Fluid: Fluid wall condition: select regions; select Condition: No slip; and specify thermal energy (temperature) and turbulence conditions at the wall |
A slip wall is a surface where the fluid does not adhere to the wall and cannot penetrate it. This wall condition is modeled by specifying the wall-normal fluid velocity equal to the wall velocity (zero if the wall is not moving). In cases where a moving boundary is being considered, an associated set of mesh displacement boundary conditions must be prescribed in conjunction with the surface fluid velocity to achieve the proper behavior.
| Input File Usage: | Use the following option to define slip wall boundary conditions at surfaces: |
*FLUID BOUNDARY, WALL, SURFACE=surface name, SLIP=YES boundary condition type label, magnitude or distribution name, amplitude name where boundary condition type label is VELX, VELY, VELZ, VELXNU, VELYNU, VELZNU, TEMP, TURBKE, TURBEPS, or TURBOMEGA. For example, use the following settings for a slip wall that is not moving and with the Spalart-Allmaras turbulence model active (wall-normal distance boundary condition and turbulent eddy viscosity set to zero at the wall): *FLUID BOUNDARY, WALL, SURFACE=Surface-1, SLIP=YES VELX, 1.0 VELY, 0.0 VELZ, 0.0 |
| Abaqus/CAE Usage: | Use the following option to define slip wall boundary conditions at surfaces: |
Load module: Create Boundary Condition: Step: flow_step: Category: Fluid: Fluid wall condition: select regions; select Condition: Shear; and specify velocity, thermal energy (temperature), and turbulence conditions at the wall Specifying the specific energy dissipation rate is not supported in Abaqus/CAE. |
A symmetry boundary condition specifies that the same flow conditions exist on both sides of the surface.
| Input File Usage: | Use the following option to define symmetry boundary conditions at surface: |
*FLUID BOUNDARY, SYMMETRIC, SURFACE=surface name |
| Abaqus/CAE Usage: | Defining symmetry boundary conditions based on a physical type is not supported in Abaqus/CAE. |
Abaqus/CFD provides the capability to perform both deforming-mesh and fluid-structure interaction (FSI) simulations using an arbitrary Lagrangian-Eulerian (ALE) methodology for the fluid flow. For FSI and deforming-mesh problems, typically some portion of the fluid domain is deformed consistent with a boundary motion. To manage the mesh motion, you must prescribe displacement boundary conditions on the mesh. For FSI problems, displacement boundary conditions are not permitted at the co-simulation region because these conditions are prescribed automatically.
| Input File Usage: | *BOUNDARY node or node set, first degree of freedom, last degree of freedom, magnitude |
where first degree of freedom is 1 for the x-displacement, 2 for the y-displacement, or 3 for the z-displacement. |
| Abaqus/CAE Usage: | Load module: Create Boundary Condition: Step: flow_step: Category: Mechanical: Displacement/Rotation: select regions and toggle on the degree or degrees of freedom |
By default, all boundary conditions defined in the previous general analysis step remain unchanged in the subsequent general step. You define the boundary conditions in effect for a given step relative to the preexisting boundary conditions. At each new step the existing boundary conditions can be modified and additional boundary conditions can be specified. Alternatively, you can release all previously applied boundary conditions in a step and specify new ones. In this case any boundary conditions that are to be retained must be respecified.
When you modify an existing boundary condition, the node or node set must be specified in exactly the same way as previously. For example, if a boundary condition is specified for a node set in one step and for an individual node contained in the set in another step, Abaqus issues an error. You must remove the boundary condition and respecify it to change the way the node or node set is specified.
| Input File Usage: | Use one of the following options to modify an existing boundary condition or to specify an additional boundary condition: |
*BOUNDARY *BOUNDARY, OP=MOD *FLUID BOUNDARY *FLUID BOUNDARY, OP=MOD |
| Abaqus/CAE Usage: | Load module: Create Boundary Condition or Boundary Condition Manager: Edit |
If you choose to remove any boundary condition in a step, no boundary conditions will be propagated from the previous general step. In that case, all boundary conditions that are in effect during the step must be respecified.
Setting a boundary condition to zero is not the same as removing it.
| Input File Usage: | Use one of the following options to release all previously applied boundary conditions and to specify new boundary conditions: |
*BOUNDARY, OP=NEW If the OP=NEW parameter is used on any *BOUNDARY option within a step, it must be used on all *BOUNDARY options in the step. *FLUID BOUNDARY, OP=NEW If the OP=NEW parameter is used on any *FLUID BOUNDARY option within a step, it must be used on all *FLUID BOUNDARY options in the step. |
| Abaqus/CAE Usage: | Use the following option to remove a boundary condition within a step: |
Load module: Boundary Condition Manager: Deactivate Abaqus/CAE automatically respecifies any boundary conditions that should remain in effect during this step. |