PartDesign Groove

From FreeCAD Documentation
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PartDesign Groove

Menu location
Part Design → Create a substractive feature → Groove
Workbenches
PartDesign
Default shortcut
None
Introduced in version
-
See also
PartDesign Revolution

Description

The Groove tool revolves a selected sketch or profile about a given axis, cutting out material from the support .

Above: sketch (A) is revolved around axis (B); resulting groove on solid (C) is shown right.

Usage

  1. Select the sketch to be revolved.
    A face on the existing solid can alternatively be used. version 0.17 and above
    The sketch must be mapped to the planar face of an existing solid or Part Design feature, or an error message will appear. version 0.16 and below
  2. Press the Groove button.
  3. Set the Groove parameters (see next section).
  4. Press OK.

Options

When creating a groove, the Groove parameters dialogue offers several parameters specifying how the sketch should be revolved.

Type

Type offers five different ways of specifying the length to which the pocket will be extruded:

Dimension

Enter a numeric value for the length of the pocket. The default direction for extrusion is into the support, but it can be changed by ticking the Reversed option. Extrusions occur by default normal to the defining sketch plane. This can be changed by specifying another Direction introduced in version 0.20. With the option Symmetric to plane the pocket will extend half of the given length to either side of the plane. Negative dimensions are not possible. Use the Reversed option instead.

Through all

The pocket will extrude through all objects in the extrusion direction. With the option Symmetric to plane the pad will cut through all material in both directions.
Note: For technical reasons, Through All is actually a 10 meter deep pocket. If you need deeper pockets, use the type Dimension.

To first

The pocket will extrude up to the first face of the support in the extrusion direction. In other words, it will cut through all material until it reaches an empty space.

Up to face

The pocket will extrude up to a face in the model that can be chosen by clicking on it.

Two dimensions

This allows to enter a second length in which the pocket should extend in the opposite direction (into the support). The directions can be switched by ticking the Reversed option.

Length

Defines the length of the pocket. Multiple units can be used independently of the user's units preferences (m, cm, mm, nm, ft or ', in or "). This option is only available when Type is either Dimension or Two dimensions.

Axis

This option specifies the axis about which the sketch is to be revolved.

  • Vertical sketch axis: selects the vertical sketch axis .
  • Horizontal sketch axis: selects the horizontal sketch axis.
  • Sketch axis: selects a construction line contained in the sketch used by the Groove. The first construction line created in the sketch will be labelled Sketch axis 0. The drop down list will contain one custom sketch axis for each construction line. version 0.16 and below
  • Construction line: selects a construction line contained in the sketch used by the Groove. The drop down list will contain an entry for each construction line. The first construction line created in the sketch will be labelled Construction line 1. version 0.17 and above
  • Base (X/Y/Z) axis: selects the X, Y or Z axis of the Body's Origin; version 0.17 and above
  • Select reference...: allows selection in the 3D view of an edge on the Body, or a datum line. version 0.17 and above

Angle

This controls the angle through which the groove is to be formed, e.g. 360° would be a full, contiguous revolution. It is not possible to specify negative angles (use the Reversed option instead) or angles greater than 360° .

Symmetric to plane

If checked, the groove will extend half of the specified angle in both directions from the sketch plane .

Reversed

If checked, the direction of revolution is reversed from default clockwise to counterclockwise .

Properties

Below are properties which can be defined after creation of the feature. Data properties Base and Axis are uneditable .

  • DataAngle: angle of rotation. See Angle .
  • DataLabel: label given to the operation, can be changed at convenience.
  • DataMidplane: true or false. See Symmetric to plane.
  • DataReversed: true or false. See Reversed.
  • DataRefine: true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details. version 0.17 and above

Notes