Core Feature

The Core Feature command extends the internal shape of a cavity. A spatial volume replaces material volume only where the Core feature intersects with the shellable or external feature within the same body. The Core feature is most useful if you want to create a uniquely shaped shell with varying wall thicknesses.
Open the Core.CATPart document.

 

 

  1. Click the Core Feature icon .
    Core features can have different shapes. The Core 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 Prism, Sweep, Revolve, Thick Surface or External Shape tasks. For the purposes of our scenario, keep the default option.

  3. Select Sketch.2 as the profile you wish to extrude. If no profile is defined, clicking the Sketcher icon enables you to sketch the profile you need.

  4. In the Limits tab, enter 20 mm to define First length, enter 0mm for Second length and click the Reverse Direction button.

  5. Optionally, set the parameters and options you wish to make the shape more complex as explained in Prism (or Sweep) page.

  6. Click OK to confirm and create the core feature. Core Prism.X is added to the specification tree in the Solid Functional Set.X node.

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.

The Core feature can only be used for Shellable and External features.