Simple Hole PropertyManager

The Simple Hole PropertyManager appears when you create a new Simple Hole in a part, or when you edit an existing simple hole feature.

To open this PropertyManager:

Click Simple Hole (Features toolbar) or Insert > Features > Hole > Simple.

From

Sets the starting condition for the simple hole feature.

Sketch Plane Starts the simple hole from the same plane on which the sketch is located.
Surface/Face/Plane Starts the simple hole from one of these entities. Select a valid entity for Surface/Face/Plane .
Vertex Starts the simple hole from the vertex you select for Vertex .
Offset Starts the simple hole on a plane that is offset from the current sketch plane. Set the offset distance for Enter Offset Value.

Direction 1

Some fields that accept numeric input allow you to create an equation by entering = (equal sign) and selecting global variables, functions, and file properties from a drop-down list. See Direct Input of Equations in PropertyManagers.
  End Condition Select from the available end condition types.
Direction of Extrusion Extrudes the hole in a direction other than normal to the profile of the sketch. Select any of the following:
   
  • Cylindrical faces
  • Conical faces
  • Planar faces
  • Sketch points
  • Vertices
  • Linear edges
  • Linear sketch entities
  • Reference axes
  • Reference planes
  • Points in reference geometry
   

Normal to sketch extrusion

Direction vector extrusion
Face/Plane Select a face or plane in the graphics area to set the hole depth when you choose Up To Surface or Offset From Surface as the End Condition.
Offset Distance Set the hole depth or offset distance when you choose Blind or Offset From Surface as the End Condition. Optionally, select the following:

Reverse offset

Applies the specified Offset Distance in the opposite direction from the selected Face/Plane .

Translate surface

Applies the specified Offset Distance relative to the selected surface or plane. To use a true offset, clear Translate surface.
   

True offset - Translate surface check box cleared

Translated surface - Translate surface check box selected
Vertex Select a vertex or midpoint in the graphics area to set the hole depth when you select Up To Vertex as the End Condition.
Hole Diameter  
Draft On/Off Adds draft to the hole. Set Draft Angle to specify the degrees for the draft. Optionally, select the following:

Draft Outward

Creates an outward draft angle when you select Draft On/Off .

Feature Scope

Specifies which bodies or components you want the feature to affect.
  • For multibody parts, see Feature Scope in Multibody Parts.
  • For assemblies, see Feature Scope in Assemblies.