PartDesign Вырез

This page is a translated version of the page PartDesign Pocket and the translation is 4% complete.

Outdated translations are marked like this.

Аддитивный клин

Отверстие

Верстак PartDesign

Расположение в меню
Вырез
Part Design → Create a substractive feature → Вырез
Верстаки
PartDesign
Быстрые клавиши
Нет
Представлено в версии
-
См. также
Выдавливание

Description

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

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

introduced in 26.3: The Pocket tool extrudes a sketch or a face along a straight path to create a Pocket feature that is either the result of a Cut or an optional Common operation.

Cut Operation

Cuts the overlapping portion of the extruded shape from the base feature.

Existing solid (base feature) and a profile sketch → "Subtraction" preview mode → Resulting solid (Pocket feature)

Common Operation

Keeps the overlapping portion of base feature and extruded shape.

Existing solid (base feature) and a profile sketch → "Common" preview mode → Resulting solid (Pocket feature)

Usage

Select a single sketch or one or more faces from the Body.
There are several ways to invoke the tool:
- Press the Pocket button.
- Select the Part Design → Subtractive Features → Pocket option from the menu.
The Pocket Parameters Task Panel opens.
- Optionally toggle the Operation mode (introduced in 26.3):
  - Subtraction (default) activates the boolean Cut operation.
  - Common activates the boolean Common operation.
- Optionally adjust further Pocket parameters, see Options below.
Press the OK button to close the TaskPanel and finish the tool.

Options

When creating a pocket, or after double-clicking an existing pocket in the Tree View, the Pocket parameters task panel is shown. It offers the following settings:

Start

Sets where the pocket begins. By default the pocket starts at the sketch or face used as its profile. introduced in 26.3

Profile plane (default): the pocket starts directly at the profile's sketch plane or face.
Offset: the pocket starts at a numeric distance from the profile, entered in the Start Offset field.
Reference: the pocket starts at a face, datum plane, or sketch selected with the Pick Reference button.

This is useful to create multiple features from a single master sketch without needing separate offset planes for each one.

Direction

You can select how the pocket is created:

One sided: the pocket extends on one side of the face.
Two sided: the pocket extends on both sides of the face. Two sub-menus (Side 1 and Side 2) appear to define the pocket for each side.
Symmetric: the pocket is symmetrical with respect to the original face.

Type

Type offers five different ways of specifying the length of the pocket:

Dimension

Enter a numeric value for the Length of the pocket. With the option Symmetric to plane the pocket will extend half the given length to either side of the sketch or face.

Through all

The pocket will extend up to the last face of the support it encounters in its direction. With the option Symmetric to plane the pocket will cut through all material in both directions. Note that 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 extend up to the first face of the support it encounters in its direction.

Up to face

The pocket will extend up to a face. Press the Select face button and select a face or a datum plane from the Body.

Two dimensions

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

Up to shape

introduced in 1.0: The pocket will extend up to the selected shape. Optionally press the Select shape button and select a shape. Leave the Select all faces checkbox enabled or disable it, press the Select button and select the faces up to which the pocket should be created.

Offset to face

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

Length

Defines the length of the pocket. This option is only available if Type is Dimension or Two dimensions. The length is measured along the direction vector, or along the normal of the sketch or face. Negative values are not possible. Use the Reversed option instead.

2nd length

Defines the length of the pocket in the opposite direction. This option is only available if Type is Two dimensions.

Symmetric to plane

Check this option to extrude half the given length to either side of the sketch or face, if Type is Dimension, or Through all if that is the Type.

Reversed

Reverses the direction of the pocket.

Direction

Direction/edge

You can select the direction of the extrusion:

Sketch normal or Face normal: The sketch or face is extruded in the opposite direction of its normal. If you have selected several sketches or faces to be extruded, the normal of the first one will be used.
Select reference…: The sketch or face is extruded in the opposite direction of a straight edge or a datum line selected from the Body.
Custom direction: The sketch or face is extruded in the direction of the specified vector.

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 or face normal, otherwise along the custom direction.

Taper angle

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

2nd taper angle

Tapers the pocket in the opposite extrusion direction by the given angle. See Taper angle. This option is only available if Type is Two dimensions.

Operation

Sets the boolean operation used to combine the pocket with the base solid. introduced in 26.3

Subtraction (default): the pocket removes the extruded volume from the base solid, as in previous versions.
Common: the pocket keeps only the volume shared between the extruded profile and the base solid, discarding everything else. This is useful, for example, to trim a solid down to the intersection with a reference shape.

Properties

Data

Part Design

ДанныеRefine (Bool): 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).
ДанныеOperation (Enumeration): sets the boolean operation used to combine the feature with the base solid (Subtraction, Common), see Options. introduced in 26.3

Pocket

ДанныеType (Enumeration): Defines how the pocket will be extruded, see Options.
ДанныеLength (Length): Defines the length of the pocket, see Options.
ДанныеLength2 (Length): Second pocket length in case the ДанныеType is TwoLengths, see Options.
ДанныеUse Custom Vector (Bool): If checked, the pocket direction will not be the normal vector of the sketch but the given vector, see Options.
ДанныеDirection (Vector): Vector of the pocket direction if ДанныеUse Custom Vector is used.
ДанныеReference Axis (LinkSub)
ДанныеAlong Sketch Normal (Bool): If true, the pocket length is measured along the sketch normal. Otherwise and if ДанныеUse Custom Vector is used, it is measured along the custom direction.
ДанныеUp To Face (LinkSub): A face the pocket will extrude up to, see Options.
ДанныеOffset (Length)
ДанныеTaper Angle (Angle)
ДанныеTaper Angle2 (Angle)

Sketch Based

ДанныеProfile (LinkSub)
ДанныеMidplane (Bool)
ДанныеReversed (Bool)
ДанныеAllow Multi Face (Bool)

Start

ДанныеStart Type (Enumeration): sets how the pocket start is defined (Profile plane, Offset, Reference), see Options. introduced in 26.3
ДанныеStart Offset (Length): distance between the profile and the start of the pocket. Only used if ДанныеStart Type is Offset. introduced in 26.3
ДанныеStart Reference (LinkSub): a face, plane, or sketch the pocket starts from. Only used if ДанныеStart Type is Reference. introduced in 26.3

Limitations

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