For information about shell conduction considerations, see the following sections:
By default, ANSYS Fluent treats walls as having zero-thickness and presenting no thermal resistance to heat transfer across them. If a thickness is specified for a wall (thereby making it a thin wall, as described in Thin-Wall Thermal Resistance Parameters) then the appropriate thermal resistance across the wall thickness is imposed, although conduction is considered in the wall in the normal direction only. There are applications, however, where conduction in the planar directions of the wall is also important. For these applications, you have two options: you can either mesh the thickness, or you can use the shell conduction approach. Shell conduction can be used to model one or more layers of wall cells without the need to mesh the wall thickness in a preprocessor. When the shell conduction approach is utilized, you have the ability to easily switch on and off conjugate heat transfer on any wall. If you create a shell—either by enabling Shell Conduction in an individual Wall dialog box (as described in Shell Conduction) or by defining multiple walls as shell conduction zones using the Shell Conduction Manager dialog box (as described in Managing Shell Conduction Walls)—and define the settings for the shell layer(s) using the Shell Conduction Layers dialog box, then ANSYS Fluent will automatically grow the specified layers of cells for the wall during the solution process. The cells that are grown will be either prism cells or hex cells, depending on the type of face mesh that is utilized; at no point are the cells visible in the displayed mesh.
Shell conduction can be used to account for thermal mass in transient thermal analysis problems (see Locking the Temperature for Solid and Shell Zones for more information). It can also be used for multiple junctions and allows heat conduction through the junctions. Shell conduction can be applied on boundary walls as well as two-sided walls.
In the case where shell conduction is applied on a boundary wall, the original surface is referred to as the “wall surface” and is always adjacent to the fluid / solid cells. As part of the solution, layers of wall cells are grown away from the fluid / solid zone. These layers are numbered sequentially, starting with the one closest to the wall surface. See Figure 12.5: A Boundary Wall with Shell Conduction for a visualization of how the solver treats shells.
For the most part, the boundary conditions that you specify for the boundary wall are applied to the layer surface that is furthest from the wall surface; only the internal emissivity is applied at the wall surface. The sides of the shell zone require boundary conditions as well. If the shell is connected to another wall that does not have shell conduction enabled, the shell side will take the boundary condition of the attached wall. The sides will be adiabatic if they are connected to face zones that have a boundary condition type other than wall. If the attached wall has shell conduction enabled, then the common sides at the junction will be coupled.
The layers of cells grown for two-sided walls can be visualized in a similar way to Figure 12.5: A Boundary Wall with Shell Conduction, except that the layer surface that is furthest from the wall surface is also adjacent to a shadow wall (which is then adjacent to the other fluid / solid zone).
The following is a list of limitations for the shell conduction model:
Shells cannot be created on non-conformal interfaces, including mapped interfaces.
Shell conduction cannot be used on moving wall zones.
Shell conduction cannot be used with FMG initialization.
Shell conduction is not available when the wall is set up to receive thermal data via system coupling.
Shell conduction is not available for 2D.
Shell conduction is available only when the pressure-based solver is used.
Shell conducting walls cannot be split or merged. If you need to split or merge a shell conducting wall, you will need to turn off the Shell Conduction option for the wall (in the Wall dialog box), 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. This will ensure that adaption is not performed on the shell conducting wall.
Fluxes at the ends of a shell conducting wall are not included in heat balance reports. These fluxes are accounted for correctly in the ANSYS Fluent solution, but are not listed in the flux report.
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).
Shells with a sharp bend may yield non-physical temperature fields when using Green-Gauss Node Based gradients. This applies to any angle (acute or obtuse) with the effect worsening as the angle approaches 90 degrees. To resolve the issue, you should consider breaking the sharp angled shells into multiple shells or, in the event that this cannot be done, enabling Warped Face Gradient Correction.
The Shell Conduction Manager dialog box provides a convenient way for you to manage, define, and display multiple shell conduction zones. You can
display any wall zone
enable or disable shell conduction for a wall
define the settings for shell conduction walls or layers, such as thickness, material, and heat generation rate
Note that you can still enable shell conduction for a wall and define the related settings using the Wall dialog box, as described in Shell Conduction. However, the Shell Conduction Manager dialog box provides you with an alternative to do such activities from a single dialog box for all the walls, instead of visiting the individual Wall boundary condition dialog boxes.
Setting Up Physics → Model
Specific → Shell Conduction...
To manage shell conduction using the Shell Conduction Manager dialog box, perform the following steps:
(optional) If you have previously generated a CSV file that contains shell conduction settings for the layers of the walls, you can read it by clicking at the bottom of the Shell Conduction Manager dialog box and using the dialog box that opens; otherwise, you should proceed to the steps that follow.
Using a CSV file can be helpful when you have a large number of layers and walls. It is not necessary to create the CSV file from nothing, as you can create a simplified CSV file with sample values using the button (as described in step 5.), and then revise the settings using a spreadsheet program. See Shell Conduction Settings File Format for details about the format of the CSV file.
Use the
and
buttons to move the selected zones from one list to
another, and thereby define whether they are shells. Zones with shell
conduction enabled are listed under Shell Conduction
Zones and those without shell conduction are listed under
Wall Zones. In essence, the
button disables shell conduction and the
button enables shell conduction.
Click the button to display the selected walls in the graphics window. Note that you can select walls with or without shell conduction. The zones will be displayed with different colors depending on the option selected in the Mesh Colors dialog box, which is accessible from the Mesh Display dialog box.
Define settings for all of the shells by performing the following steps:
Select walls from the Shell Conduction Zones for which you want to define the same settings.
Click the button to open
the Shell Conduction Layers dialog box
(Figure 12.8: Shell Conduction Layers Dialog Box). There you
can specify the number of layers, and then define the thickness,
material, and heat generation rate for each layer. Note that you
have the option of defining the heat generation rate using a
user-defined function (UDF) that utilizes the
DEFINE_PROFILE macro; for more
information on creating and using user-defined functions, see
the Fluent Customization Manual.
Important: You must specify a nonzero-thickness for every layer.
Click to save your settings for the selected walls and close the Shell Conduction Layers dialog box.
If you want to save all of the settings you specified using the Shell Conduction Manager dialog box as a CSV file, click and specify a name in the dialog box that opens. You can edit the shell conduction settings in this CSV file using a spreadsheet program, and then read it in this or a separate case file, as described in step 1. Note that information will not be written for any wall that defines the heat generation rate using a UDF.
Note that you have the option of disabling shell conduction in every wall with a single action, by using the following text command. This capability is available in both serial and parallel mode.
define →
boundary-conditions →
modify-zones →
delete-all-shells
Shell zones can be patched using the Patch dialog box, as described in Patching Values in Selected Cells.
Solution →
Initialization
Patch...
You can lock (or “freeze”) the temperature values for all the
cells in shells and solid zones (including those to which you have a hooked an
energy source through a UDF) by using the
solve/set/lock-solid-temperature? text command, as
described in Locking the Temperature for Solid and Shell Zones.
In order to facilitate the postprocessing of shells, surfaces (referred to as “shell surfaces”) are created at the interface of adjacent layers, as well as at the layer surface that is furthest from the wall surface. Note that shell surfaces are not created on the sides of the shell zones or in the interior of the layers. The shell surfaces can then be selected from the Surfaces list available in a variety of dialog boxes (for example, the Contours dialog box, the Surface Report Definition dialog box, and the Solution XY Plot dialog box) in the same way as the surfaces for the wall and (for two-sided walls) the shadow wall. When visualized in the graphics display window, these shell surfaces will be coincident with the wall they are associated with.
The default naming convention for these shell surfaces is <wall_name>-<c0>:<c1>, where:
<wall_name> is the name of the wall on which the layers have been grown.
<c0> is the rank of the layer on the c0 side of the interface (that is, the layer closest to the wall surface).
<c1> is the rank of the layer on the c1 side of the interface (that is, the layer furthest from the wall surface). Note that the layer surface that is furthest from the wall surface does not have a layer on the c1 side, and so a different convention is used: for boundary walls, <c1> is set to external; for two-sided walls, <c1> is set to the name of the fluid / solid adjacent to the shadow wall.
You have the ability to rename the shell surfaces, if you want. The following figures illustrate the default naming convention, where the wall/shadow surfaces are displayed in red and the shell surfaces are displayed in black.
You can use the walls, shadow walls, and shell surfaces to display the temperature of the interfaces and adjacent cells. The Temperature... category provides two options: the temperature of the cell on the c0 side of the surface is stored as Static Temperature; and the temperature of the surface itself is stored as Wall Temperature. 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.
The following examples illustrate how to postprocess the surfaces shown in Figure 12.9: Shell Surface Names for a Boundary Wall:
The Static Temperature and Wall Temperature of Bwall will provide the temperature of the fluid cells adjacent to Bwall and the temperature of the Bwall surface itself, respectively.
The Static Temperature and Wall Temperature of Bwall-1:2 will provide the temperature of the cells of Layer 1 and the temperature of the interface between Layer 1 and Layer 2 (that is, the Bwall-1:2 shell surface), respectively.
The Static Temperature and Wall Temperature of Bwall-3:external will provide the temperature of the cells of Layer 3 and the temperature of the layer surface that is furthest from the wall surface (that is, the Bwall-3:external shell surface), respectively.
The following examples illustrate how to postprocess the surfaces shown in Figure 12.10: Shell Surface Names for a Two-Sided Wall:
The Static Temperature and Wall Temperature of 2Swall-4:air will provide the temperature of the cells of Layer 4 and the temperature of the interface between Layer 4 and the shadow wall (that is, the 2Swall-4:air shell surface), respectively.
The Static Temperature and Wall Temperature of 2Swall-shadow will provide the temperature of the air cells adjacent to 2Swall-shadow and the temperature of the shadow wall, respectively.
When postprocessing shells, note the following limitations:
You should not enable Node Values when postprocessing any surfaces associated with shells (that is, the wall, shadow wall, or shell surfaces). The layers share nodes at the edges, and thus the averaging at such nodes is erroneous.
You cannot postprocess shells in ANSYS CFD-Post, as shell surfaces are not supported.