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:
Open a sketch on the inside face of the Cavity Body, as shown.
Sketch the outline of the core you want to create.
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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.
Close the sketch.
With the sketch selected, click Core
on the Mold Tools toolbar, or click Insert,
Molds, Core.
In the PropertyManager,
set the options as described below, then click OK
.
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.