PartDesign Hole

Description
The Hole feature creates one or more holes from a selected sketch. Many parameters can be set such as threading and size, fit, hole type (countersink, counterbore, straight) and more.



How to use

 * 1) Press the  button.
 * 2) If an existing unused sketch is found, it will be automatically be used. If more than one sketch is found, a Select feature panel appears to make a selection. Alternatively, a sketch can be selected before launching the Hole command.
 * 3) Define the Hole parameters. See Options.
 * 4) Press.

Options
Depending on which selection is made, some fields will activate or stay disabled.



Threading and size

 * Profile: if set to None, no threading info is defined. ISO and UTS thread profiles enable the Direction, Size, Fit and Class fields.
 * Threaded: check will add threading data to the Hole feature and the hole minor diameter is used. If left unchecked, the hole is considered non-threaded, and the nominal major diameter with defined Fit is chosen.
 * Direction: sets the thread direction (Right Hand or Left hand) if Threaded is checked.
 * Size: Sets the thread size. Requires Profile to be set to one of the ISO or UTS profiles.
 * Fit: defines standard or close fit for threaded profiles.
 * Class: defines the tolerance class.
 * Diameter: defines the hole diameter if the Profile was set to None.
 * Depth: depth of the hole from the sketch plane. Dimension enables a field to type a value. Through All will cut the hole through the whole Body.

Hole cut

 * Type: sets type of hole cut: None is a straight hole; other types are Counterbore, Countersink, Cheesehead, Countersink socket screw and Cap screw.
 * Diameter: sets the major diameter for all hole cut types except None. Value is non-editable if a thread profile was selected in Profile.
 * Depth: depth of the hole cut type from the sketch plane. Value is non-editable if a thread profile was selected in Profile.
 * Countersink angle: angle of the conical hole cut. Value is non-editable if a thread profile was selected in Profile.

Drill point

 * Type: defines the ending of the hole if Depth is set to Dimension. Flat produces a flat bottom; Angled sets a conical point.

Misc

 * Tapered: sets a taper angle to the hole. Value is calculated from the sketch plane normal. 90 degrees sets a straight hole. A value under 90 generates a smaller hole radius at the bottom; a value over 90 enlarges the hole radius at the bottom.

Properties
Much of the Data properties are the same as those shown in Options.


 * : name given to the object, this name can be changed at convenience.
 * : true or false. Reverses extrusion direction.
 * : true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details.

Limitations

 * The selected sketch must contain one or more circle(s). The radius of the circle(s) inside the sketch is not taken into account. The generated holes will be identical even if the circles in the sketch have varying radii.
 * By default, the hole feature extrudes below the sketch plane. If the solid lies on the XY_Plane, and the hole sketch is attached to the XY_Plane, it will try to extrude away from the solid and seemingly produce no result. In such a case, the Reversed property needs to be manually set to true; otherwise the sketch needs to be mapped to the bottom face of the solid.