Wall boundary conditions are used to bound fluid and solid regions. In viscous flows, the no-slip boundary condition is enforced at walls by default, but you can specify a tangential velocity component in terms of the translational or rotational motion of the wall boundary, or model a "slip'' wall by specifying shear. (You can also model a slip wall with zero shear using the symmetry boundary type, but using a symmetry boundary will apply symmetry conditions for all equations. See Section 7.3.15 for details.)
The shear stress and heat transfer between the fluid and wall are computed based on the flow details in the local flow field.
Inputs at Wall Boundaries
You will enter the following information for a wall boundary:
Wall boundaries can be either stationary or moving. The stationary boundary condition specifies a fixed wall, whereas the moving boundary condition can be used to specify the translational or rotational velocity of the wall, or the velocity components.
Wall motion conditions are entered in the Momentum tab of the Wall dialog box (Figure 7.3.15), which is opened from the Boundary Conditions task page (as described in Section 7.1.4). To view the wall motion conditions, click the Momentum tab.
Defining a Stationary Wall
For a stationary wall, choose the Stationary Wall option under Wall Motion.
Velocity Conditions for Moving Walls
If you wish to include tangential motion of the wall in your calculation, you need to define the translational or rotational velocity, or the velocity components. Select the Moving Wall option under Wall Motion. The Wall dialog box will expand, as shown in Figure 7.3.15, to show the wall velocity conditions.
Note that you cannot use the moving wall condition to model problems where the wall has a motion normal to itself. ANSYS FLUENT will neglect any normal component of wall motion that you specify using the methods below.
Specifying Relative or Absolute Velocity
If the cell zone adjacent to the wall is moving (e.g., if you are using a moving reference frame or a sliding mesh), you can choose to specify velocities relative to the zone motion by enabling the Relative to Adjacent Cell Zone option. If you choose to specify relative velocities, a velocity of zero means that the wall is stationary in the relative frame, and therefore moving at the speed of the adjacent cell zone in the absolute frame. If you choose to specify absolute velocities (by enabling the Absolute option), a velocity of zero means that the wall is stationary in the absolute frame, and therefore moving at the speed of the adjacent cell zone--but in the opposite direction--in the relative reference frame.
| If you are using one or more moving reference frames, sliding meshes, or mixing planes, and you want the wall to be fixed in the moving frame, it is recommended that you specify relative velocities (the default) rather than absolute velocities. Then, if you modify the speed of the adjacent cell zone, you will not need to make any changes to the wall velocities, as you would if you specified absolute velocities.
Note that if the adjacent cell zone is not moving, the absolute and relative options are equivalent.
Translational Wall Motion
For problems that include linear translational motion of the wall boundary (e.g., a rectangular duct with a moving belt as one wall) you can enable the Translational option and specify the wall's Speed and Direction ( X,Y,Z vector). By default, wall motion is "disabled'' by the specification of Translational velocity with a Speed of zero.
If you need to define non-linear translational motion, you will need to use the Components option, described below.
Rotational Wall Motion
For problems that include rotational wall motion you can enable the Rotational option and define the rotational Speed about a specified axis. To define the axis, set the Rotation-Axis Direction and Rotation-Axis Origin. This axis is independent of the axis of rotation used by the adjacent cell zone, and independent of any other wall rotation axis. For 3D problems, the axis of rotation is the vector passing through the specified Rotation-Axis Origin and parallel to the vector from (0,0,0) to the ( X,Y,Z) point specified under Rotation-Axis Direction. For 2D problems, you will specify only the Rotation-Axis Origin; the axis of rotation is the -direction vector passing through the specified point. For 2D axisymmetric problems, you will not define the axis: the rotation will always be about the axis, with the origin at (0,0).
Note that the modeling of tangential rotational motion will be correct only if the wall bounds a surface of revolution about the prescribed axis of rotation (e.g., a circle or cylinder). Note also that rotational motion can be specified for a wall in a stationary reference frame.
Wall Motion Based on Velocity Components
For problems that include linear or non-linear translational motion of the wall boundary you can enable the Components option and specify the X-Velocity, Y-Velocity, and Z-Velocity of the wall. You can define non-linear translational motion using a profile or a user-defined function for the X-Velocity, Y-Velocity, and/or Z-Velocity of the wall.
Wall Motion for Two-Sided Walls
As discussed earlier in this section, when you read a mesh with a two-sided wall zone (which forms the interface between fluid/solid regions) into ANSYS FLUENT, a "shadow'' zone will automatically be created so that each side of the wall is a distinct wall zone. For two-sided walls, it is possible to specify different motions for the wall and shadow zones, whether or not they are coupled. Note, however, that you cannot specify motion for a wall (or shadow) that is adjacent to a solid zone.
Shear Conditions at Walls
Four types of shear conditions are available:
The no-slip condition is the default, and it indicates that the fluid sticks to the wall and moves with the same velocity as the wall, if it is moving. The specified shear and Marangoni stress boundary conditions are useful in modeling situations in which the shear stress (rather than the motion of the fluid) is known. Examples of such situations are applied shear stress, slip wall (zero shear stress), and free surface conditions (zero shear stress or shear stress dependent on surface tension gradient). The specified shear boundary condition allows you to specify the , , and components of the shear stress as constant values or profiles. The Marangoni stress boundary condition allows you to specify the gradient of the surface tension with respect to the temperature at this surface. The shear stress is calculated based on the surface gradient of the temperature and the specified surface tension gradient. The Marangoni stress option is available only for calculations in which the energy equation is being solved.
The specularity coefficient shear condition is specifically used in multiphase with granular flows. The specularity coefficient is a measure of the fraction of collisions which transfer momentum to the wall and its value ranges between zero and unity. This implementation is based on the Johnson and Jackson [ 36] boundary conditions for granular flows.
Shear conditions are entered in the Momentum tab of the Wall dialog box, which is opened from the Boundary Conditions task page (as described in Section 7.1.4).
You can model a no-slip wall by selecting the No Slip option under Shear Condition. This is the default for all walls in viscous flows.
In addition to the no-slip wall that is the default for viscous flows, you can model a slip wall by specifying zero or non-zero shear. For non-zero shear, the shear to be specified is the shear at the wall by the fluid. To specify the shear, select the Specified Shear option under Shear Condition (see Figure 7.3.16). You can then enter , , and components of shear under Shear Stress. Wall functions for turbulence are not used with the Specified Shear option.
For multiphase granular flow, you can specify the specularity coefficient such that when the value is zero, this condition is equivalent to zero shear at the wall, but when the value is near unity, there is a significant amount of lateral momentum transfer. To specify the specularity coefficient, select the Specularity Coefficient option under Shear Condition (see Figure 7.3.17) and enter the desired value in the text-entry box under Specularity Coefficient.
ANSYS FLUENT can also model shear stresses caused by the variation of surface tension due to temperature. The shear stress applied at the wall is given by
where is the surface tension gradient with respect to temperature, and is the surface gradient. This shear stress is then applied to the momentum equation.
To model Marangoni stress for the wall, select the Marangoni Stress option under Shear Condition (see Figure 7.3.18). This option is available only for calculations in which the energy equation is being solved. You can then enter the surface tension gradient ( in Equation 7.3-40) in the Surface Tension Gradient field. Wall functions for turbulence are not used with the Marangoni Stress option.
Wall Roughness Effects in Turbulent Wall-Bounded Flows
Fluid flows over rough surfaces are encountered in diverse situations. Examples are, among many others, flows over the surfaces of airplanes, ships, turbomachinery, heat exchangers, and piping systems, and atmospheric boundary layers over terrain of varying roughness. Wall roughness affects drag (resistance) and heat and mass transfer on the walls.
If you are modeling a turbulent wall-bounded flow in which the wall roughness effects are considered to be significant, you can include the wall roughness effects through the law-of-the-wall modified for roughness.
Law-of-the-Wall Modified for Roughness
Experiments in roughened pipes and channels indicate that the mean velocity distribution near rough walls, when plotted in the usual semi-logarithmic scale, has the same slope ( ) but a different intercept (additive constant in the log-law). Thus, the law-of-the-wall for mean velocity modified for roughness has the form
where is a roughness function that quantifies the shift of the intercept due to roughness effects.
depends, in general, on the type (uniform sand, rivets, threads, ribs, mesh-wire, etc.) and size of the roughness. There is no universal roughness function valid for all types of roughness. For a sand-grain roughness and similar types of uniform roughness elements, however, has been found to be well-correlated with the nondimensional roughness height, , where is the physical roughness height and . Analyses of experimental data show that the roughness function is not a single function of , but takes different forms depending on the value. It has been observed that there are three distinct regimes:
According to the data, roughness effects are negligible in the hydrodynamically smooth regime, but become increasingly important in the transitional regime, and take full effect in the fully rough regime.
In ANSYS FLUENT, the whole roughness regime is subdivided into the three regimes, and the formulas proposed by Cebeci and Bradshaw based on Nikuradse's data [ 14] are adopted to compute for each regime.
For the hydrodynamically smooth regime (
For the transitional regime ( ):
where is a roughness constant, and depends on the type of the roughness.
In the fully rough regime (
In the solver, given the roughness parameters, is evaluated using the corresponding formula (Equation 7.3-43, 7.3-44, or 7.3-45). The modified law-of-the-wall in Equation 7.3-41 is then used to evaluate the shear stress at the wall and other wall functions for the mean temperature and turbulent quantities.
Setting the Roughness Parameters
The roughness parameters are in the Momentum tab of the Wall dialog box (see Figure 7.3.18), which is opened from the Boundary Conditions task page (as described in Section 7.1.4).
To model the wall roughness effects, you must specify two roughness parameters: the Roughness Height, , and the Roughness Constant, . The default roughness height ( ) is zero, which corresponds to smooth walls. For the roughness to take effect, you must specify a non-zero value for . For a uniform sand-grain roughness, the height of the sand-grain can simply be taken for . For a non-uniform sand-grain, however, the mean diameter ( ) would be a more meaningful roughness height. For other types of roughness, an "equivalent'' sand-grain roughness height could be used for . The above approaches are only relevant if the height is considered constant per surface. However, if the roughness constant or roughness height is not constant (i.e., flow over a nonuniform surface), then you can specify a profile (Section 7.6). Similarly, user-defined functions may be used to define a wall roughness height that is not constant. For details on the format of user-defined functions, refer to the separate UDF Manual.
Choosing a proper roughness constant ( ) is dictated mainly by the type of the given roughness. The default roughness constant ( ) was determined so that, when used with - turbulence models, it reproduces Nikuradse's resistance data for pipes roughened with tightly-packed, uniform sand-grain roughness. You may need to adjust the roughness constant when the roughness you want to model departs much from uniform sand-grain. For instance, there is some experimental evidence that, for non-uniform sand-grains, ribs, and wire-mesh roughness, a higher value ( ) is more appropriate. Unfortunately, a clear guideline for choosing for arbitrary types of roughness is not available.
Note that it is not physically meaningful to have a mesh size such that the wall-adjacent cell is smaller than the roughness height. For best results, make sure that the distance from the wall to the centroid of the wall-adjacent cell is greater than .
Thermal Boundary Conditions at Walls
When you are solving the energy equation, you need to define thermal boundary conditions at wall boundaries. Five types of thermal conditions are available:
If the wall zone is a "two-sided wall'' (a wall that forms the interface between two regions, such as the fluid/solid interface for a conjugate heat transfer problem) a subset of these thermal conditions will be available, but you will also be able to choose whether or not the two sides of the wall are "coupled''. See below for details.
The inputs for each type of thermal condition are described below. If the wall has a non-zero thickness, you should also set parameters for calculating thin-wall thermal resistance and heat generation in the wall, as described below.
You can model conduction within boundary walls and internal (i.e., two-sided) walls of your model. This type of conduction, called shell conduction, allows you to more conveniently model heat conduction on walls where the wall thickness is small with respect to the overall geometry (e.g., finned heat exchangers or sheet metal in automobile underhoods). Meshing these walls with solid cells would lead to high-aspect-ratio meshes and a significant increase in the total number of cells. See below for details about shell conduction.
Thermal conditions are entered in the Thermal tab of the Wall dialog box (Figure 7.3.19), which is opened from the Boundary Conditions (as described in Section 7.1.4).
Heat Flux Boundary Conditions
For a fixed heat flux condition, choose the Heat Flux option under Thermal Conditions. You will then need to set the appropriate value for the heat flux at the wall surface in the Heat Flux field. You can define an adiabatic wall by setting a zero heat flux condition. This is the default condition for all walls.
Temperature Boundary Conditions
To select the fixed temperature condition, choose the Temperature option under Thermal Conditions in the Wall dialog box. You will need to specify the temperature at the wall surface ( Temperature). The heat transfer to the wall is computed using Equation 7.3-47 or Equation 7.3-48.
Convective Heat Transfer Boundary Conditions
For a convective heat transfer wall boundary, select Convection under Thermal Conditions. Your inputs of Heat Transfer Coefficient and Free Stream Temperature will allow ANSYS FLUENT to compute the heat transfer to the wall using Equation 7.3-51.
External Radiation Boundary Conditions
If radiation heat transfer from the exterior of your model is of interest, you can enable the Radiation option in the Wall dialog box and set the External Emissivity and External Radiation Temperature.
Combined Convection and External Radiation Boundary Conditions
You can choose a thermal condition that combines the convection and radiation boundary conditions by selecting the Mixed option. With this thermal condition, you will need to set the Heat Transfer Coefficient, Free Stream Temperature, External Emissivity, and External Radiation Temperature.
Thin-Wall Thermal Resistance Parameters
By default, a wall will have a thickness of zero. You can, however, in conjunction with any of the thermal conditions, model a thin layer of material on the wall. For example, you can model the effect of a piece of sheet metal between two fluid zones, a coating on a solid zone, or contact resistance between two solid regions. ANSYS FLUENT will solve a 1D steady heat conduction equation to compute the thermal resistance offered by the wall and the heat generation in the wall.
To include these effects in the heat transfer calculation you will need to specify the type of material, the thickness of the wall, and the heat generation rate in the wall. Select the material type in the Material Name drop-down list, and specify the thickness in the Wall Thickness field. If you want to check or modify the properties of the selected material, you can click Edit... to open the Edit Material dialog box; this dialog box contains just the properties of the selected material, not the full contents of the standard Create/Edit Materials dialog box.
The thermal resistance of the wall is , where is the conductivity of the wall material and is the wall thickness. The thermal wall boundary condition you set will be specified on the outside of the fluid/solid domain, which is called the inner surface of the thin wall, as shown in Figure 7.3.20. This is the side of the wall surface away from the adjacent fluid or solid cell zone. The temperature specified at this side of the wall is .
| The convention used in
ANSYS FLUENT is that for any wall, "outer" refers to the surface of the wall facing the fluid/solid cell zone and "inner" refers to the surface of the wall facing away from the adjacent fluid/solid cell zone. If shell conduction is enabled (Section
7.3.14), the shell cell temperature will be stored in the "inner" surface. If there is no shell conduction, then the "outer" surface stores the face temperature of the wall while the "inner" surface stores the evaluated value of the boundary condition specified by the user.
| Note that for thin walls, you can only specify a constant thermal conductivity. If you want to use a non-constant thermal conductivity for a wall with non-zero thickness, you should use the shell conduction model (see below for details).
Specify the heat generation rate inside the wall in the Heat Generation Rate field. This option is useful if, for example, you are modeling printed circuit boards where you know the electrical power dissipated in the circuits.
Thermal Conditions for Two-Sided Walls
If the wall zone has a fluid or solid region on each side, it is called a "two-sided wall''. When you read a mesh with this type of wall zone into ANSYS FLUENT, a "shadow'' zone will automatically be created so that each side of the wall is a distinct wall zone. In the Wall dialog box, the shadow zone's name will be shown in the Shadow Face Zone field. You can choose to specify different thermal conditions on each zone, or to couple the two zones:
Shell Conduction in Thin-Walls
To enable shell conduction for a wall, turn on the Shell Conduction option in the Wall boundary condition dialog box. When this option is enabled, ANSYS FLUENT will compute heat conduction within the wall, in addition to conduction across the wall (which is always computed when the energy equation is solved). The Shell Conduction option will appear in the Wall dialog box for all walls when solution of the energy equation is active. For a wall with shell conduction enabled, the thermal conditions are applied as described above for thin walls.
ANSYS FLUENT cases with shell conduction can be read in serial or parallel. Either a partitioned or an unpartitioned case file can be read in parallel (see Section 32.5 for more information on partitioning). After reading a case file in parallel, shell zones can be created on any wall with a positive thickness.
To delete existing shell conduction zones all at once, the TUI command define/boundary-conditions/modify-zones/delete-all-shells is used. This capability is available in both serial and parallel mode.
| You must specify a non-zero
Wall Thickness in the
Wall dialog box, because the shell conduction model is relevant only for walls with non-zero thickness.
| Note that the shell conduction model has several limitations:
Species Boundary Conditions for Walls
By default, a zero-gradient condition for all species is assumed at walls (except for species that participate in surface reactions), but it is also possible to specify species mass fractions at walls. That is, Dirichlet boundary conditions such as those that are specified at inlets can be used at walls as well.
If you wish to retain the default zero-gradient condition for a species, no inputs are required. If you want to specify the mass fraction for a species at the wall, the steps are as follows:
The boundary condition type for each species is specified separately, so you can choose to use different methods for different species.
If you are modeling species transport with reactions, you can, alternatively, enable a reaction mechanism at a wall by turning on the Reaction option and selecting an available mechanism from the Reaction Mechanisms drop-down list. See Section 15.1.3 more information about defining reaction mechanisms.
Reaction Boundary Conditions for Walls
If you have enabled the modeling of wall surface reactions in the Species Model dialog box, you can indicate whether or not surface reactions should be activated for the wall. In the Species tab of the Wall dialog box (Figure 7.3.22), turn the Surface Reactions option on or off.
Note that a zero-gradient condition is assumed at the wall for species that do not participate in any surface reactions.
Radiation Boundary Conditions for Walls
If you are using the P-1 radiation model, the DTRM, the DO gray model, or the surface-to-surface model, you will need to set the emissivity of the wall ( Internal Emissivity) in the Thermal tab of the Wall dialog box. If you are using the Rosseland model you do not need to set the emissivity, because ANSYS FLUENT assumes the emissivity is 1. If you are using the DO non-gray model, you will also need to define the wall as opaque or semi-transparent in the Radiation tab. See Section 13.3.6 for details.
Discrete Phase Model (DPM) Boundary Conditions for Walls
If you are modeling a discrete phase of particles, you can set the fate of particle trajectories at the wall in the DPM section of the Wall dialog box. See Section 23.4 for details.
Wall Adhesion Contact Angle for VOF Model
If you are using the VOF model and you are modeling wall adhesion, you can specify the contact angle for each pair of phases at the wall in the Momentum tab of the Wall dialog box. See Section 24.2.9 for details.
User-Defined Scalar (UDS) Boundary Conditions for Walls
If you have defined UDS transport equations in your model, you can specify boundary conditions for each equation in the UDS section of the Wall dialog box. See Section 9.1.3 for details.
Default Settings at Wall Boundaries
The default thermal boundary condition is a fixed heat flux of zero. Walls are, by default, not moving.
Shear-Stress Calculation Procedure at Wall Boundaries
For no-slip wall conditions, ANSYS FLUENT uses the properties of the flow adjacent to the wall/fluid boundary to predict the shear stress on the fluid at the wall. In laminar flows this calculation simply depends on the velocity gradient at the wall, while in turbulent flows one of the approaches described in this section in the separate Theory Guide is used.
For specified-shear walls, ANSYS FLUENT will compute the tangential velocity at the boundary.
If you are modeling inviscid flow with ANSYS FLUENT, all walls use a slip condition, so they are frictionless and exert no shear stress on the adjacent fluid.
Shear-Stress Calculation in Laminar Flow
In a laminar flow , the wall shear stress is defined by the normal velocity gradient at the wall as
When there is a steep velocity gradient at the wall, you must be sure that the mesh is sufficiently fine to accurately resolve the boundary layer. Guidelines for the appropriate placement of the near-wall node in laminar flows are provided in Section 6.2.2.
Shear-Stress Calculation in Turbulent Flows
Wall treatments for turbulent flows are described in this section in the separate Theory Guide.
Heat Transfer Calculations at Wall Boundaries
Temperature Boundary Conditions
When a fixed temperature condition is applied at the wall, the heat flux to the wall from a fluid cell is computed as
|=||fluid-side local heat transfer coefficient|
|=||wall surface temperature|
|=||local fluid temperature|
|=||radiative heat flux|
Note that the fluid-side heat transfer coefficient is computed based on the local flow-field conditions (e.g., turbulence level, temperature, and velocity profiles), as described by Equation 7.3-54 and this equation in the separate Theory Guide.
Heat transfer to the wall boundary from a solid cell is computed as
|=||thermal conductivity of the solid|
|=||local solid temperature|
|=||distance between wall surface and the solid cell center|
Heat Flux Boundary Conditions
When you define a heat flux boundary condition at a wall, you specify the heat flux at the wall surface. ANSYS FLUENT uses Equation 7.3-47 and your input of heat flux to determine the wall surface temperature adjacent to a fluid cell as
where, as noted above, the fluid-side heat transfer coefficient is computed based on the local flow-field conditions. When the wall borders a solid region, the wall surface temperature is computed as
Convective Heat Transfer Boundary Conditions
When you specify a convective heat transfer coefficient boundary condition at a wall, ANSYS FLUENT uses your inputs of the external heat transfer coefficient and external heat sink temperature to compute the heat flux to the wall as
|=||external heat transfer coefficient defined by you|
|=||external heat-sink temperature defined by you|
|=||radiative heat flux|
Equation 7.3-51 assumes a wall of zero thickness.
External Radiation Boundary Conditions
When the external radiation boundary condition is used in ANSYS FLUENT, the heat flux to the wall is computed as
|=||emissivity of the external wall surface defined by you|
|=||surface temperature of the wall|
|=||temperature of the radiation source or sink on the exterior|
|of the domain, defined by you|
|=||radiative heat flux to the wall from within the domain|
Equation 7.3-52 assumes a wall of zero thickness.
Combined External Convection and Radiation Boundary Conditions
When you choose the combined external heat transfer condition , the heat flux to the wall is computed as
where the variables are as defined above. Equation 7.3-53 assumes a wall of zero thickness.
Calculation of the Fluid-Side Heat Transfer Coefficient
In laminar flows, the fluid side heat transfer at walls is computed using Fourier's law applied at the walls. ANSYS FLUENT uses its discrete form:
where is the local coordinate normal to the wall.
For turbulent flows, ANSYS FLUENT uses the law-of-the-wall for temperature derived using the analogy between heat and momentum transfer [ 41]. See this section in the separate Theory Guide for details.