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 Symmetry Boundary Conditions 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.
You will enter the following information for a wall boundary:
wall motion conditions (for moving or rotating walls)
shear conditions (for slip walls, optional)
wall roughness (for turbulent flows, optional)
thermal boundary conditions (for heat transfer calculations)
species boundary conditions (for species calculations)
chemical reaction boundary conditions (for surface reactions)
radiation boundary conditions (for calculations using the P-1, DTRM, DO, surface-to-surface, or MC models)
discrete phase boundary conditions (for discrete phase calculations)
wall adhesion contact angle (for VOF calculations, optional)
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 6.35: The Wall Dialog Box for a Moving Wall), which is opened from the Boundary Conditions Task Page (as described in Setting Cell Zone and Boundary Conditions). To view the wall motion conditions, click the Momentum tab.
For a stationary wall, choose the Stationary Wall option under Wall Motion.
If you want 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 6.35: The Wall Dialog Box for a Moving Wall, to show the wall velocity conditions.
Note that you cannot use the moving wall condition to model problems where the wall motion with respect to the adjacent cell zone has a component that is normal to the wall itself. For such problems, consider using a Sliding or Dynamic Mesh approach as discussed in Modeling Flows Using Sliding and Dynamic Meshes. 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 (for example, 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.
Important: 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 (for example, 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. You can define time-varying translational speed using a transient profile (Standard Transient Profiles) or user-defined function for the speed of the wall.
If you need to define nonlinear 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).
You can define time-varying rotational speed using a transient profile
(Standard Transient Profiles) profile or a user-defined function
for the speed of the wall.
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 (for example, 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 nonlinear 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 nonlinear 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.
Four types of shear conditions are available:
no-slip
specified shear
specularity coefficient
Marangoni stress
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 that transfer momentum to the wall and its value ranges between zero and unity. This implementation is based on the Johnson and Jackson [48] 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 Setting Cell Zone and Boundary Conditions).
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 nonzero shear.
For nonzero 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 6.36: The Wall Dialog Box for Specified Shear). 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 6.37: The Wall Dialog Box for the Specularity Coefficient) and enter the desired value in the text-entry box under Specularity Coefficient.
Note: The specularity coefficient is not available for moving walls.
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
(6–100) |
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 6.38: The Wall Dialog Box for Marangoni Stress). 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 6–100) in the Surface
Tension Gradient field. Wall functions for turbulence are
not used with the Marangoni Stress option.
Fluid flows over rough surfaces are encountered in diverse situations. Examples are, among many others, flows over the surfaces of airplanes (especially due to ice accretion), 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 Standard Law-of-the-Wall Modified for Roughness law-of-the-wall modified for roughness or you can use one of the Additional Roughness Models for Icing Simulations.
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). Therefore, the law-of-the-wall for mean velocity
modified for roughness has the form
(6–101) |
where and
(6–102) |
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, and so on) 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:
hydrodynamically smooth ()
transitional ()
fully rough ()
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
[20] are adopted to compute for each regime.
For the hydrodynamically smooth regime ():
(6–103) |
For the transitional regime ():
(6–104) |
where is a roughness constant, and depends on the type of the
roughness.
In the fully rough regime ():
(6–105) |
In the solver, given the roughness parameters, is evaluated using the corresponding formula (Equation 6–103, Equation 6–104, or Equation 6–105). The modified law-of-the-wall in
Equation 6–101 is then used to evaluate the shear
stress at the wall and other wall functions for the mean temperature and turbulent
quantities.
represents a downward shift of the logarithmic velocity profile, as
shown in the following figure:
This downward shift leads to a singularity for large roughness heights and low
values of . Depending on the turbulence model and near wall treatment, two
different approaches are used in ANSYS Fluent in order to avoid this issue:
reducing the roughness height as decreases
The first approach consists in redefining the roughness height based on the mesh refinement:
(6–106) |
This ensures that as approaches zero, so too does
. Therefore, the mesh requirement for rough walls in this case is
, in order to maintain the full effect of the roughness on the
flow.
virtually shifting the wall
The second approach is based on the observation that the viscous sublayer is fully established only near hydraulically smooth walls. In the transitional roughness regime, the roughness elements are slightly thicker than the viscous sublayer and start to disturb it, so that in fully rough flows, the sublayer is destroyed and viscous effects become negligible. The following figure illustrates the equivalent sand-grain roughness using a wall with a layer of closely packed spheres, which have an average roughness height representing a technical roughness with peaks and valleys of different shapes and sizes (see Schlichting and Gersten [101]):
It can be assumed that the roughness has a blockage effect, which is about 50% of its height (note that the figure above shows a two-dimensional cut of a three-dimensional arrangement).
It is therefore sensible to virtually shift the wall to 50% of the height of
the roughness elements. This results in a corrected value for the first cell center:
(6–107) |
which gives about the correct displacement caused by the surface roughness. Thus the singularity issue is avoided and fine meshes can be handled correctly.
The second approach (that is, virtually shifting the wall) is the default
treatment for rough walls for all two-equation turbulence models based on the
-equation and for the following turbulence models based on the
-equation, when they are used with standard and scalable wall
functions (note that the use of scalable wall functions is recommended over the use of
standard wall functions):
standard, RNG, and realizable -
model
Reynolds stress models
All other model combinations with rough walls (for example, the Spalart-Allmaras
model) have no special calibration on fine meshes, and therefore the first approach
(reducing the roughness height as decreases) is used.
Note: Rough walls cannot be used together with the following model combinations:
an -equation model with enhanced wall treatment or the
Menter-Lechner near-wall treatment
Note that the following are the relevant -equation models:
all of the -
models (that is, standard, RNG, and realizable)
the Reynolds stress model with the Linear Pressure-Strain model selected
the detached eddy simulation (DES) model with the Realizable k-epsilon option selected
the Reynolds stress model with the Stress-Omega or Stress-BSL model selected
the transition -
-
model
the large eddy simulation (LES) model
Important: Prior to ANSYS Fluent 14, the shift described by Equation 6–107 was not applied when using turbulence
models based on the -equation. You can recover the previous code behavior by using the
following scheme
command:
(rpsetvar 'ke-rough-wall-treatment-r14? #f) (models-changed)
The roughness parameters are in the Momentum tab of the Wall Dialog Box (see Figure 6.38: The Wall Dialog Box for Marangoni Stress), which is opened from the Boundary Conditions Task Page (as described in Setting Cell Zone and Boundary Conditions).
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 nonzero 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, then you can specify a profile (see Profiles). 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 Fluent Customization 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: The advantage of the rough wall formulation using a virtual shift of the wall
(Equation 6–107) compared to reducing the
roughness height as decreases (Equation 6–106) is
that it eliminates all restrictions with respect to mesh resolution near the wall,
and can therefore be used on arbitrarily fine meshes.
Additional roughness models are available if you have selected the Spalart-Allmaras or the SST k-ω model in the Viscous Model dialog box. See the Steps in Using a Turbulence Model for more information. With one of these viscous models active, the additional roughness models will be available on the Wall boundary condition panel on the Momentum tab under Wall Roughness → Roughness Models → High Roughness (Icing). A discussion of the treatment of the turbulence models with the High Roughness (Icing) enabled is given in Treatment of the Spalart-Allmaras Model for Icing Simulations and Treatment of the SST Model for Icing Simulations. These models are primarily designed and tested for simulations of icing applications, however they may also be useful for other applications in which the boundary layer is fully resolved and there is surface roughness that is large relative to the near-wall mesh.
Note that the High Roughness (Icing) models are only valid for low-Re number turbulence, or need fine near-wall meshes (mesh should fully resolve the boundary layer).
You have the following options:
Specified Roughness
NASA Correlation
Shin-et-al
ICE3D Roughness File
The Specified Roughness option is the same as in the Standard roughness model. See Setting the Roughness Parameters for more details.
If the NASA Correlation option is selected, the surface sand-grain roughness height is computed with an empirical NASA correlation for icing in air flows [103]. The sand-grain roughness height is computed from the product of the following coefficients:
(6–108) |
(6–109) |
(6–110) |
Where is the Free Stream Velocity,
is the Free Stream Temperature, LC is the
Liquid Content (in most cases water for ice accretion), c is
the Characteristic Length, and
.
The sand-grain roughness height is then obtained from the formulation:
(6–111) |
If the Shin-et-al option is selected the empirical correlation for the surface sand-grain roughness is computed with the Shin and Bond formulation [103], which modifies the NASA correlation (see the NASA Correlation for a description of variables) with the following factor:
(6–112) |
where MVD is the droplet mean diameter (Droplet Diameter). The corresponding value of the sand-grain roughness height is obtained from:
(6–113) |
If the ICE3D Roughness File is selected, the sand-grain
roughness height is read from a node-based input file obtained from FENSAP-ICE. The
file must have the format , and be read in Fluent via File →
Read → Profile. After the
FENSAP-ICE roughness file is read into Fluent, the file name will appear in the
dropdown list.
When you are solving the energy equation, you need to define thermal boundary conditions at wall boundaries. Seven types of thermal conditions are available:
fixed heat flux
fixed temperature
convective heat transfer
external radiation heat transfer
combined external radiation and convection heat transfer
thermal data transferred between another system in Workbench using System Coupling
thermal coupling across a mapped interface
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 nonzero-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 (that is, 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 (for example, 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 6.42: The Wall Dialog Box (Thermal Tab)), which is opened from the Boundary Conditions task page (as described in Setting Cell Zone and 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.
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 6–115 or Equation 6–116.
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 6–119.
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.
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.
When modeling the heat transfer of applications that have perturbed flow and/or disturbed boundary layers, it can be necessary to augment the calculation of the diffusive heat flux with a convective augmentation factor. Such applications include the modeling of underhood and underbody heat loads, as wells as transient heat transfer in fully warmed-up exhaust systems.
The convective augmentation factor represents the ratio of the measured Nusselt number to the Nusselt number of an ideal flow. You can define it by using the following text command:
define → boundary-conditions → wall
You will be prompted to define the Convective Augmentation
Factor as either a profile or a single value. Note that
a value of 1 (the default value) represents no augmentation of the
diffusive heat flux, whereas values greater than 1 initiate augmentation.
For further details, see the equation for qid in DEFINE_HEAT_FLUX of the Fluent Customization Manual.
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 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.
When you specify a thickness, the wall is then treated as a coupled wall, where the surface that is adjacent to the fluid / solid cells is referred to as the “wall surface”. See Figure 6.43: A Thin Wall.
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 surface that
is separated from the fluid / solid cells by the wall thickness. The
temperature specified at this side of the wall is
.
Important: 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 nonzero-thickness, you should use the shell conduction model (see Shell Conduction 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.
When postprocessing a wall that has a thickness but does not have shell conduction enabled, the Temperature... category provides three options: the temperature of the adjacent fluid / solid cells are stored as Static Temperature; the temperature of the wall surface itself is stored as Wall Temperature; and the temperature of the surface that is separated from the fluid / solid cells by the wall thickness is stored as Wall Temperature (Thin). If a more detailed analysis of the solid zone and surfaces is required, then you should consider creating layers of solid cells in your meshing application.
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:
To couple the two sides of the wall, select the Coupled option under Thermal Conditions. (This option will appear in the Wall dialog box only when the wall is a two-sided wall.) No additional thermal boundary conditions are required, because the solver will calculate heat transfer directly from the solution in the adjacent cells. You can, however, specify the material type, wall thickness, and heat generation rate for thin-wall thermal resistance calculations, as described above. Note that the resistance parameters you set for one side of the wall will automatically be assigned to its shadow wall zone. Specifying the heat generation rate inside the wall is useful if, for example, you are modeling printed circuit boards where you know the electrical power dissipated in the circuits but not the heat flux or wall temperature.
To uncouple the two sides of the wall and specify
different thermal conditions on each one, choose Temperature or Heat Flux as the thermal condition type
(Convection and Radiation are not applicable for two-sided walls); note that this uncoupling
will not be effective if you have enabled shell conduction for the
wall. The relationship between the wall and its shadow will be retained,
so that you can couple them again at a later time, if desired. You
will need to set the relevant parameters for the selected thermal
condition, as described above. The two uncoupled walls can have different
thicknesses, and are effectively insulated from one another. If you
specify a nonzero wall thickness for the uncoupled walls, the thermal
boundary conditions you set will be specified for each thin wall on
the surface that is separated from the fluid / solid cells by the
wall thickness, as shown in Figure 6.44: Uncoupled Thin Walls, where is the Temperature (or
is the Heat Flux) specified
on one wall and
is the Temperature (or
is the Heat Flux) specified on the other wall.
and
are the thermal
conductivities of the uncoupled thin walls. Note that the gap between
the walls in Figure 6.44: Uncoupled Thin Walls is
not part of the model; it is included in the figure only to show where
the thermal boundary condition for each uncoupled wall is applied.
To enable shell conduction for a wall, enable the Shell Conduction option in the Wall boundary condition dialog box. You can then click the button to open the Shell Conduction Layers dialog box, where you can define the properties of the single or multiple layers of the shell. Note that you must specify a nonzero wall thickness for every layer of the shell. When shell conduction is enabled, ANSYS Fluent will compute heat conduction for the wall not only in the normal direction (which is always computed when the energy equation is solved), but also in the planar directions. The Shell Conduction option will appear in the Wall dialog box for all walls when solution of the energy equation is active (except for mapped interfaces). For information about how the thermal conditions are applied on a wall with shell conduction enabled, managing multiple shells, and postprocessing shell conduction walls, see Shell Conduction Considerations.
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 Mesh Partitioning and Load Balancing for more information on partitioning). After reading a case file in parallel, shell zones can be created on any wall.
To convert every wall with a finite thickness into a shell with
a single action, the TUI command define/boundary-conditions/modify-zones/create-all-shell-threads can be used; each converted shell will have a single layer with
the same thickness as the original thin wall (any pre-existing shells
will not be modified). To disable shell conduction in every wall with
a single action, the TUI command define/boundary-conditions/modify-zones/delete-all-shells can be used. These capabilities are available in both serial and
parallel mode.
Important: Note that the shell conduction model has several limitations:
It cannot be applied on non-conformal interfaces, including mapped interfaces.
It cannot be applied on moving wall zones.
It cannot be used with FMG initialization.
Shell conduction is not available when the wall is set up to receive thermal data via system coupling.
It is available only in 3D.
It is available only when the pressure-based solver is used.
Shells cannot be split or merged. If you need to split or merge a shell, disable the Shell Conduction option for the wall, perform the split or merge operation, and then enable Shell Conduction for the new wall zones.
The shell conduction model cannot be used on a wall zone that has undergone hanging node adaption. If you want to perform such adaption elsewhere in the computational domain, be sure to use the mask register described in Manipulating Adaption Registers.
Fluxes at the ends of a shell are not included in the heat balance reports. These fluxes are accounted for correctly in the ANSYS Fluent solution, but not in the flux report itself.
The junction of a wall with shell conduction enabled and a non-conformal coupled wall is not supported. Such a junction will not be thermally connected, that is, there will be no heat transfer between the shell and the mesh interface wall.
When running the parallel solver with the shell conduction model, note that coupled walls are encapsulated. If you encounter problems with the partitioning of the mesh, you can try changing the encapsulation method to see if that resolves the problem (see Troubleshooting for this and other troubleshooting options).
System coupling allows the input and output of thermal data from ANSYS Fluent. When Fluent is coupled with another system in Workbench using System Coupling, you can select the via System Coupling option on the desired wall boundaries to receive thermal data through System Coupling service. Note that this option does not need to be selected to provide thermal data from Fluent.
For more details about setting up a simulation with system coupling, see the Fluent in Workbench User's Guide and the System Coupling User’s Guide.
When thermal data is transferred into Fluent via System Coupling, the following variables are available:
temperature
heat flow (heat rate)
When thermal data is transferred out of Fluent via System Coupling, the following variables are available:
temperature
heat flow (heat rate)
heat transfer coefficient (also known as “convection coefficient”)
near wall temperature (also known as “bulk temperature” or “ambient temperature”)
For each data transfer, you specify the type of data transfer (the variables transferred) during the System Coupling setup.
As part of standard heat transfer boundary condition settings in ANSYS Fluent, you can also 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; if you want to check or modify the properties of the selected material, you can click to open the Edit Material dialog box (this dialog box contains just the properties of the selected material, and not the full contents of the standard Create/Edit Materials dialog box). You can specify the thickness in the Wall Thickness number-entry box and the heat generation rate in the Heat Generation Rate number-entry box.
Note: A boundary will behave in the same way as an adiabatic boundary if the via System Coupling option is enabled on this boundary, and ANSYS Fluent is not receiving data from the coupling data transfer. Fluent is not receiving coupling data if it is either not involved with a System Coupling simulation, or if the coupling is a one-way transfer with the Fluent analysis only providing data to the second solver.
Mapped interfaces provide a robust approach for modeling coupled walls between zones when the interface zones penetrate each other or have gaps between them (see Figure 6.45: 2D Interface with Penetration and Gaps). For the interface wall boundary zones created as part of such interfaces, via Mapped Interface is automatically selected from the Thermal Conditions list in the Thermal tab of the Wall dialog box, in order to interpolate the thermal data.
Important: Note that thermal coupling calculations will not be performed at mapped interfaces for the Eulerian multiphase model.
For more details about mapped interfaces, see The Mapped Option and Using a Non-Conformal Mesh in ANSYS Fluent.
Such boundaries also allow you to specify the standard heat transfer boundary condition settings, such as 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; if you want to check or modify the properties of the selected material, you can click to open the Edit Material dialog box (this dialog box contains just the properties of the selected material, and not the full contents of the standard Create/Edit Materials dialog box). You can specify the thickness in the Wall Thickness number-entry box and the heat generation rate in the Heat Generation Rate number-entry box. Note that the Shell Conduction option is not available with the via Mapped Interface thermal condition.
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 want 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:
Click the Species tab in the Wall Dialog Box to view the species boundary conditions for the wall (see Figure 6.46: The Wall Dialog Box for Species Boundary Condition Input).
Under Species Boundary Condition, select Specified Mass Fraction (rather than Zero Diffusive Flux) in the drop-down list to the right of the species name. The dialog box will expand to include a field for Species Mass Fractions.
Under Species Mass Fractions, specify the mass fraction for the species.
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 Defining Zone-Based Reaction Mechanisms for more information about defining reaction mechanisms.
You can also model unresolved surface washcoats, which greatly increase the catalytic surface area, by specifying the Surface Area Washcoat Factor. The surface washcoat increases the area available for surface reaction.
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 6.46: The Wall Dialog Box for Species Boundary Condition Input), 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.
If you are using the gray P-1, DTRM, DO, surface-to-surface, or MC models, 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.
For the non-gray P-1, DO, or MC models, specify a constant Internal Emissivity for each wavelength band in the Radiation tab of the Wall dialog box (the default value in each band is 1). Alternatively, you can specify the internal emissivity using a boundary condition parameter (see Creating a New Parameter). If you are using the non-gray DO model, you will also need to define the wall as opaque or semi-transparent in the Radiation tab. See Defining Boundary Conditions for Radiation for details. If you are using the MC models, you can enable a Boundary Source option, which allows you to specify the Beam Direction and the Direct Irradiation.
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 Setting Boundary Conditions for the Discrete Phase for details.
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 Steps for Setting Boundary Conditions for details.
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 Setting Up UDS Equations in ANSYS Fluent for details.
If you are using the Eulerian Wall Film model (see Modeling Eulerian Wall Films for details), you can set liquid film conditions at the wall in the Wall Film tab of the Wall dialog box. This tab is available only if you have enabled the Eulerian Wall Film model in the Models Task Page.
For details, see Setting Eulerian Wall Film Solution Controls.
The default thermal boundary condition is a fixed heat flux of zero. Walls are, by default, not moving.
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 Near-Wall Treatments for Wall-Bounded Turbulent Flows in the 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.
In a laminar flow, the wall shear stress is defined by the normal velocity gradient at the wall as
(6–114) |
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 Mesh Element Distribution.
Wall treatments for turbulent flows are described in Near-Wall Treatments for Wall-Bounded Turbulent Flows in the Theory Guide.
When a fixed temperature condition is applied at the wall, the heat flux to the wall from a fluid cell is computed as
(6–115) |
| where | |
| | |
| | |
| | |
| |
Note that the fluid-side heat transfer coefficient is computed based on the local flow-field conditions (for example, turbulence level, temperature, and velocity profiles), as described by Equation 6–122.
Heat transfer to the wall boundary from a solid cell is computed as
(6–116) |
| where | |
| | |
| | |
| |
When you define a heat flux boundary condition at a wall, you specify the heat flux at the wall surface. ANSYS Fluent uses Equation 6–115 and your input of heat flux to determine the wall surface temperature adjacent to a fluid cell as
(6–117) |
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
(6–118) |
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
(6–119) |
| where | |
| | |
| | |
| |
Equation 6–119 assumes a wall of zero-thickness.
When the external radiation boundary condition is used in ANSYS Fluent, the heat flux to the wall is computed as
(6–120) |
| where | |
| | |
| | |
| | |
| | |
| |
Equation 6–120 assumes a wall of zero-thickness.
When you choose the combined external heat transfer condition, the heat flux to the wall is computed as
(6–121) |
where the variables are as defined above. Equation 6–121 assumes a wall of zero-thickness.
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:
(6–122) |
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 [56]. See Standard Wall Functions in the separate Theory Guide for details.