Creating Shells from Parts

Simcenter STAR-CCM+ provides support for thin-walled structures that are best represented by a two-dimensional cell layer during simulation. These single-cell layers are known as shells.

Shell parts are a mathematical simplification of solids. One of the main advantages of using shell elements is that it reduces the computational time and resources required for simulations as fewer mesh elements are present. Shells are also easier to mesh and less prone to negative Jacobian errors which can occur when using extremely thin three-dimensional cells.

This section contains the recommended workflow for creating and setting up shells at the parts level.

To create a shell part use one of the following methods:
- To create shell parts when importing geometry, In the Import Surface Options dialog, activate the Create Shells option.
  
  For the single STL (.stl), database (.dbs), and JTOpen (.jt) surface mesh file types, if you wish to create one part for each cell type then set Parts Mode to One part per cell type.
- To create shell parts when transferring 3D-CAD model to geometry parts, In the Part Creation Options dialog, activate the Create Shells From Sheets option.
- To convert regular parts to shells in geometry parts, Under the Parts node, right-click the desired part and select Convert to Shell.

For regular shell parts any changes made to the original geometry are not transferred to the shell part. To connect the shell part to the underlying geometry you create an attached shell part.

To create an attached shell part use either:
- The Create Attached Shell(s) option:
  1. Expand the Parts node and multi-select the desired part surfaces.
    The selected part surfaces can either come from the same part or multiple parts.
  2. Right-click one of the selected parts and select Create Attached Shell(s).
    This action automatically transfers any tags defined on the source part surfaces to the attached shell part.
  3. If you wish to create a separate shell part for each part surface, within the Create Attached Shell Options dialog, activate Create one shell part per part surface and click OK.
    If the selected surfaces are from different parts, Create one shell part per part surface is the only option available. If you make any changes to the original part surface the shell part is automatically updated.
- The Attached Shells Creator operation:
  1. Right-click Operations and select New > Surface Preparation > Attached Shells Creator.
  2. In the Create Attached Shells Creator Operation dialog, define the Input Parts and Part Surfaces.
  3. If you want to create a shell part for each part surface, activate One Shell Part Per Part Surface.
  4. Click OK.
  5. Right-click the Operations > Attached Shells Creator and select Execute.
    If you make changes to the original parts or part surfaces the shell part is automatically updated when you re-execute the operation.
  When the attached shell part is updated any boundary conditions or mesh setting applied to the shell part are maintained.
When creating the shells, Simcenter STAR-CCM+ also creates surface contacts between the shells and the original parts, and any required edge contacts between the shells.
Shell parts can be represented by a number of different icons. Grey icons () represent shell parts which are linked to a 3D-CAD model, green icons () represent shell parts which do not have any 3D-CAD, blue icons () represent shell parts in which the original geometry is imported into Simcenter STAR-CCM+ and contains CAD data and as such are considered as static topologies, and attached shell icons () represent shell parts created using the Attached Shells Creator operation.
Conceptually, the shell approximates a thin 3D object so that the single surface in the geometry presents two sides (front and back) in the physics:

A shell part has two part surfaces—a front and a back surface. You can apply physics and boundary conditions on the part surfaces respectively. For example, you can set different thermal boundary conditions on either surface. The front and back surfaces of a shell part are highlighted in different colors. The front surface appears in dark blue, whereas the back surface appears in light blue:

After creating the shell part, the part curves from the original part are split into perimeter curves and interior curves. A perimeter curve is represented by the or icon whereas an interior curve is represented by the or icon. You can set edge boundary conditions on the perimeter curve. For attached shell parts, if a free edge is not captured as a perimeter or interior curve, a separate curve is generated under the shell part.

The orientation of the part surfaces is important when you want to set physics conditions or report vector quantities. In cases where you want to control and determine which side is front and which side is back, edit the Orientation method:

To set the Orientation method:
1. Select the Geometry > Parts > [shell parts] > Orientation node and set Method to Point.
2. Select the Orientation > Point node and set Orientation Point to the correct coordinate values.
You can activate the point tool and use it to drag the point until it is positioned on the front side of the shell.

Before assigning shell parts to regions, create an empty shell region first, because you cannot create shell regions automatically using the Assign Parts to Regions dialog.

To create a region with shell topology, right-click the Regions node and select New > Shell Region.
This distinction is important because you can only create hub interfaces if the shells are assigned to shell regions. A region type cannot be changed afterwards.

You can assign both sides of a shell part to the same shell boundary, or you can assign them to different boundaries. If you assign them to different boundaries then you can apply specific boundary conditions on each side.

Shell edge boundaries are associated with perimeter part curves which correspond to free edges on the shell part and are associated with a conceptual boundary on the side of an idealized thin part.

To create a Shell Edge Boundary, right-click the Boundaries node and select New > Shell Edge Boundary.
To assign shell parts to regions, do one of the following:
- Right-click one of the Geometry > Parts > [shell part] nodes and select Assign Parts to Regions.
- Within Geometry > Parts, right-click each shell part, shell part surface, or shell perimeter curve and assign them to appropriate regions and boundaries individually. see 壳区域参考
After assigning the shell parts to a region, you create hub interfaces if you want to transfer solution data between the shell parts. Hub interfaces can join shell edges to shell edges or shell edges to shell surfaces. You can create the hub interfaces at either the parts level or the region level.
- To create a boundary-based hub interface, under the Boundaries manager node of a shell region, select one or more shell boundary edges or surfaces, right-click one of them, and select Create Hub Interface.
- To create a parts-based hub interface, within the Geometry > Parts node, select the desired part curves or part surfaces from the respective Curves or Surfaces nodes of shell parts only. Right-click on one of the selected entities and select Create Hub Interface.
- To create an empty hub interface, right-click the Interface node and select New Hub Interface > Boundary-Mode or Part Entity-Mode. You can then populate the interface manually using the property selectors.
- To create an empty hub interface from existing solid shell regions, under the Regions manger node, select one or more solid shell regions, right-click one of them, and select Create Interface > Boundary-Mode Hub Interface or Part Entity-Mode Hub Interface. You can then populate the interface manually using the property selectors.
For more information on hub interfaces, see 创建轮毂交界面.
To create a mesh on the shell parts, use the automated mesh operation.
1. Right-click the Geometry > Operations node and select New > Mesh > Automated Mesh (Shell) .
2. In the Create Automated Mesh (Shell) Operation dialog:
  1. Select the shell parts from which to create the mesh.
  2. Select a volume mesher:
    - Quadrilateral Mesher — generates quadrilateral cells on the input parts.
    - Triangular Mesher — generates triangle cells on the input parts.
3. Expand the Operations > Automated Mesh (Shell) > Default Controls node and set the appropriate values for Base Size, Target Surface Size, and Minimum Surface Size.
4. If you want to refine the mesh in specific locations, create custom controls. See Creating and Defining Custom Controls.
5. Execute the Automated Mesh (Shell) operation.
注 The exported mesh data from shell parts, in .ccm file format can not be imported to a 3D volume mesh.
Define the physics continua for the simulation.
For more information, see Finite Volume Heat Transfer in Solid Shells.

To display values on the front and back part surfaces in the same scene:

In the scalar displayer, set Face Culling to Back.