Shellable Feature

The Shellable Feature command is very often used to create the main shape of the part. It creates a hollow feature you can open via the Shell Properties command. Shellable features can have different basic shapes: Prism, Sweep, Revolve, Thick Surface or an External Shape.

The Shellable Feature command also adds material volume to the outside of another material volume that it intersects within the same body, thus extending the boundaries of the volume, as well as increasing the internal spatial volume of a shelled volume. The added volume inherits the shell properties (wall thickness) of the body.

This task shows you how to create a shellable prism.
To perform this scenario, sketch a rectangle in the Sketcher workbench then return to the Functional Molded Part workbench.

 

 

  1. Click the Shellable Feature icon .
    Shellable features can have different shapes. The Shellable Feature dialog box that appears displays the Prism icon as the default shape to be created.

  2. If you prefer a different shape, click any of the other four shapes available. To know how to create any of them, refer to the Sweep, Revolve or Thick Surface or External Shape tasks. For the purposes of our scenario, keep the default option

  3. Select the profile you wish to extrude. If no profile is defined, clicking the Sketcher icon enables you to sketch the profile you need.

  4. Create a basic prism as explained in the Prism task.

  5. Click OK to confirm and create the shellable feature. Shellable Prism.X is added to the specification tree in the Solid Functional Set.X node. By customizing the view (use the Hidden edges points option), you can notice that by default the wall thickness of prism  is zero and the shellable feature has no opening.

  6. To open it, just double-click the Shell Properties node in the Specification tree or click the Shell Properties command .

  7. For example, select the top face as the face to be removed and enter the value of your choice to define the wall thickness.

  8. Click OK to confirm the operation. One face has been removed.

  9. For more information, refer to Setting Shell Properties.

    Core

  10. Click the Core tab.
    The Core capability enables you to define a core body (offset) for a shellable feature. This sometimes becomes necessary if the geometrical complexity of the shellable feature is such that standard offsets fail.

    11. If your part contains two or more shellable features, you need to choose between three methods:

    • Isolated core
      Automatically generates the core at feature level through an offset of only this shellable features geometry (i.e. the feature is independently shelled).

    • Interconnected core
      Automatically generates the core at functional body level through an offset of the union of all shellable features contained within the same functional body.

    • Select core
      You can select any body to represent the core for  the shellable feature. Note that faces of features that have a "selected core" cannot be later selected in Shell Properties command as Face to remove or Face with special thickness.
 

More about Intersection Fillet

For the shape selected in the Shape definition area, you can apply an intersection fillet using following options available in the Intersection Fillet list of the Fillet tab:

  • Intersection with Core/Cavity
  • Intersection with Core
  • Intersection with Cavity

In this case following three options are available:

  • The Fillet radius option enables you to add material to the feature.
  • The Round radius option enables you to remove material from the feature.
  • The Preserve Thickness option enables you to keep the thickness applied on the part.