PartDesign Pocket

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PartDesign Pocket.svg PartDesign Pocket

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

Description

The Pocket tool cuts solids by extruding a sketch or a face of a solid along a straight path.

PartDesign Pocket example.svg

Sketch profile (A) was mapped to the top face of base solid (B); result after pocketing through on the right.

Usage

  1. Select the sketch or face to be pocketed. introduced in version 0.20: Alternatively you can select several sketches or faces.
  2. Press the PartDesign Pocket.svg Pocket button.
  3. Set the Pocket parameters, see the Options below.
  4. Click OK.

When selecting a single sketch, it can have multiple enclosed profiles inside a larger one, for example a rectangle with two circles inside it. But the profiles may not intersect each other. introduced in version 0.20

Options

When creating a pocket, the the Pocket parameters dialog will be shown. It offers the following settings:

Pocket parameters cropped.png

Type

Type offers four 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.

Offset to face

Offset from face at which the pocket will end. This option is only available when Type is either Through all, To first or Up to face.

Direction

introduced in version 0.20

Direction/edge

You can select the direction of the extrusion:

  • Face/Sketch normal The sketch or face is extruded along its normal. If you have selected several sketches or faces to be extruded, the normal of the first one will be used. introduced in version 0.20
  • Select reference... The sketch is extruded along an edge of the 3D model. When this is method selected, you can click on any edge in the 3D model and it becomes the direction vector for the extrusion.
  • Custom direction The sketch is extruded along a direction that can be specified via vector values.

Show direction

If checked, the pocket direction will be shown. In case the pocket uses a Custom direction, it can be changed.

Length along sketch normal

If checked, the pocket length is measured along the sketch normal, otherwise along the custom direction.

Symmetric to plane

Tick the checkbox to extrude half of the given length to either side of the sketch or plane.

Reversed

Reverses the direction of the pocket.

Taper angle

introduced in version 0.20

Tapers the pocket in the extrusion direction by the given angle. A positive angle means the outer pocket border gets wider. This option is only available if Type is either Dimension or Two dimensions. Note that inner structures receive the opposite taper angle. This is done to facilitate the design of molds and molded parts.

Limitations:

  • Sketches containing B-Splines often cannot be properly tapered. This is a limitation of the OpenCASCADE kernel that FreeCAD uses.
  • For larger angles tapering will fail if the end face of the pocket would have fewer edges than the start face/sketch.

2nd length

Defines the length of the pocket in the opposite extrusion direction. 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 if Type is Two dimensions.

2nd taper angle

introduced in version 0.20

Tapers the pocket in the opposite extrusion direction by the given angle. A positive angle means the outer pocket border gets wider. This option is only available if Type is Two dimensions. Note that inner structures receive the opposite taper angle. This is done to facilitate the design of molds and molded parts.

Properties

  • DataType: Type of ways how the pocket will be extruded, see Options.
  • DataLength: Defines the length of the pocket, see Options.
  • DataLength2: Second pocket length in case the DataType is TwoLengths, see Options.
  • DataUse Custom Vector: introduced in version 0.20 If checked, the pocket direction will not be the normal vector of the sketch but the given vector, see Options.
  • DataDirection: introduced in version 0.20 Vector of the pocket direction if DataUse Custom Vector is used.
  • DataAlong Sketch Normal: introduced in version 0.20 If true, the pocket length is measured along the sketch normal. Otherwise and if DataUse Custom Vector is used, it is measured along the custom direction.
  • DataUp To Face: A face the pocket will extrude up to, see Options.
  • DataRefine: True or false. Cleans up residual edges left after the operation. This property is initially set according to the user's settings (found in Preferences → Part design → General → Model settings). It can be manually changed afterwards. This property will be saved with the FreeCAD document.

Limitations

  • Use the type Dimension or Through All wherever possible because the other types sometimes give trouble when they are being patterned
  • Otherwise, the pocket feature has the same limitations as the Pad feature.


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