PartDesign Hole

Other languages:
Pocket
Groove
PartDesign

PartDesign Hole

Menu location
Part Design → Create a substractive feature → Hole
Workbenches
PartDesign
Default shortcut
None
Introduced in version
0.17
See also
PartDesign Pocket

Description

The Hole feature creates one or more holes from a selected sketch's circles and arcs. If arcs are present they must be part of closed contours. All non arc/circle entities are ignored but they still must form closed contours. Many parameters can be set such as threading and size, fit, hole type (countersink, counterbore, straight) and more.

The centers of the circles and arcs are used to position the holes, but please note that their radii are not taken into account. The generated holes will be identical even if the radii vary.

Countersunk (to the left) and counterbored (to the right) holes longitudinal section.

Usage

  1. Press the Hole 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 OK.

Options

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

If set to None, no threading info is defined, and the diameter needs to be set manually.
When set to a supported standard the diameter and other parameters can be set automatically.
If checked, the provided diameter will be the recommended drill size for post-processing with a cutting tap.
If unchecked, the diameter is set according to Clearance to pass-through a thread without contact.
If checked a real thread is modeled. This consumes much computing power and is usually not used for models, except for display purposes or sometimes for 3D prints. If it is used, it is advised to check it as one of the last actions done to the model, because it will increase recomputation time significantly.
Sets the thread direction as Right Hand or Left hand.
Sets the thread size. Requires Profile to not be None
Determines the distance from the thread crest to the side of the hole. Can be understood as how tight a bolt will pass-through.
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.
Dimension: Enables a field to enter a value.
Through All: Will cut the hole through the whole Body
To reduce the file size, do not use Through All if Model Thread is checked, specify a minimal depth instead.

Hole cut

Drill point

Misc

90 degrees sets a straight hole.
Under 90 generates a smaller hole radius at the end, larger at the start.
Over 90 generates a larger hole radius at the end, smaller at the start.

Properties

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

Limitations

Cut Type Definitions

Cut types (screw-types) are defined in json files. There is a set of files distributed with FreeCAD, but users can create their own definitions. Files are searched in <UserAppDataDir>/PartDesign/Hole. The UserAppDataDir can be found by typing App.getUserAppDataDir() in the Python console.

The file should contain:

Example: 

{
    "name": "DIN 7984",
    "cut_type": "counterbore",
    "thread_type": "metric",
    "data": [
        { "thread": "M2",   "diameter":  4.3, "depth":  1.6 },
        { "thread": "M2.5", "diameter":  5.0, "depth":  2.0 },
        …
    ]
}


Pocket
Groove
PartDesign
PartDesign
User documentation