PartDesign Hole/tr

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



Usage

 * 1) Press the  button.
 * 2) If an existing unused sketch is found, it will be used automatically. 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, that are described in section 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 Size fields.
 * Threaded: if checked threading data will be added 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 Clearance 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.
 * Clearance: sets either standard, close or wide clearance hole diameter. For ISO threads the diameters are according to the ISO 273 standard, for UTS they are calculated using a rule of thumb because there is no norm defining them. Only available for non-threaded holes.
 * Class: defines the tolerance class.
 * Diameter: defines the hole diameter if the Profile is 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. Note: For technical reasons, Through All is actually a 10 meter deep hole. If you need deeper holes, use Dimension.

Hole cut

 * Type: sets type of hole cut: None means no cut, other types are different norms for screws and the two generic types Counterbore and Countersink.
 * Diameter: sets the upper diameter (at the sketch plane) for the hole cut.
 * Depth: depth of the hole cut, measured from the sketch plane.
 * Countersink angle: angle of the conical hole cut. Only applicable for countersinks.

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. Its option Take into account for depth will subtract the conical height from the Dimension. So if for example Dimension is 7.00 and the option is not used, the cylindrical part of the hole will be 7.00 and the depth necessary for the conical part is added to the hole depth. If the option is used, the overall hole depth including the conical point will be 7.00.

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.
 * Reversed: reverses the hole extrusion direction. The default direction is the mapping direction of the hole sketch to its attachment.

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. If set to true, cleans the solid from residual edges left by features. See 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 option Reversed needs to be set; alternatively the sketch can be mapped to the bottom face of the solid.

Cut Type Definitions
Cut types (screw-types) are defined in json files since version 0.19. There is a set of files distributed with FreeCAD, but users can create their own definitions. Files are searched in. The can be found by typing  in the Python console.

The file should contain: Example:
 * name: The name of the definition. This must be unique as it will be used as identifier in the FreeCAD UI and as internal index.
 * cut_type: Either or.
 * thread_type: Either  or.
 * angle: The angle of a countersink (not necessary for counterbore).
 * data: A list of sizes, consisting of:
 * thread: Name of thread known to FreeCAD.
 * diameter: The diameter of the cut.
 * depth: Depth of the counterbore (not necessary for countersink).