Example of Creating a Core

In this example, the recessed feature on the front of the plastic part is a trapped molding area that requires a core.

First, you create a sketch on a tooling solid (in this case, the Cavity Body) to define the outline of the core. Then use the Core tool to create the core.

To create a core:

1. Open a sketch on the inside face of the Cavity Body, as shown.
   
   
2. Sketch the outline of the core you want to create.

   Front view	Right view

   The plane on which you create a core sketch does not need to be perpendicular to the extraction direction of the core. In this case, the sketch is on the inside face of the cavity body, which is drafted 5° from the direction the core travels.

   Extraction direction

   Away from extraction direction

3. Close the sketch.
4. With the sketch selected, click Core on the Mold Tools toolbar, or click Insert > Molds > Core.
5. In the PropertyManager, set the options as described below, then click .
   A new body is created for the core and is subtracted from the Cavity Body.
   
   

   In the FeatureManager design tree, in the Solid Bodies folder , the new core appears in the Core bodies folder .

Selections

Bounding sketch for core	Select the core sketch created in step 2.
Extraction direction	Select the front face of the cavity body as shown.
Core/Cavity body	Displays the name of the cavity body.

Parameters

Draft On/Off	Click to add draft, then set Draft Angle to 5.
Draft outward	Select to create an outward draft angle.
End Condition	Select Blind for the end condition in the extraction direction, then set Depth along extraction direction to 50.
End Condition	Select Blind for the end condition away from the extraction direction, then set Depth away from extraction direction to 25.
Cap ends	Select to define the end surface of the core.