PartDesign Groove/ru

Проточка
Расположение в меню
Part Design → Create a substractive feature → Проточка
Верстаки
PartDesign
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Нет
Представлено в версии
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См. также
Фигура вращения

Описание

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.

Применение

1. Select a single sketch or one or more faces from the Body.
2. There are several ways to invoke the tool:
   • Press the Groove button.
   • Select the Part Design → Subtractive Features → Groove option from the menu.
3. Set the Groove Parameters, see Options below.
4. Press the OK button.

Опции

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

Type

introduced in 1.0

Type offers five different ways of specifying the angle of the groove:

Angle

Enter a numeric value for the Angle of the groove. With the option Symmetric to plane the groove will extend half the given angle to either side of the sketch or face.

Through all

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

To first

The groove will extend up to the first face of the support it encounters in its direction.

Up to face

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

Two angles

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

Start

Sets the angular starting position of the groove around the axis. By default the groove starts at the sketch plane. introduced in 26.3

• Profile plane (default): the groove starts directly at the profile's sketch plane.
• Offset: the groove starts at an angular offset from the profile, entered in the Start Offset field.
• Reference: the groove starts at a face, datum plane, or sketch selected with the Select reference button, set in the Start Reference field.

Axis

Specifies the axis of the groove:

• Vertical sketch axis: selects the vertical sketch axis.
• Horizontal sketch axis: selects the horizontal sketch axis.
• Construction line: selects a construction line from the sketch used by the groove. The dropdown list will contain an entry for each construction line. The first construction line will be labelled Construction line 1.
• Base (X/Y/Z)-axis: selects the X-, Y- or Z-axis of the Body's origin.
• Select reference…: allows the selection of a straight edge or a datum line from the Body.

Note that when changing the axis, the Reversed option may be (un)checked automatically.

Angle

Defines the angle of the groove. This option is only available if Type is Angle or Two angles. Angles larger than 360° are not possible. Nor are negative values, use the Reversed option instead.

introduced in 1.1: If the Show interactive draggers when editing features preference is selected, the angle can be adjusted with an interactive gizmo in the 3D View.

2nd angle

introduced in 1.0

Defines the angle of the groove in the opposite direction. This option is only available if Type is Two angles and Angle is smaller than 360°.

Symmetric to plane

Check this option to extend the groove half the given angle to either side of the sketch or face. This option is only available if Type is Angle or Through all.

Reversed

Reverses the direction of the groove.

Operation

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

• Subtraction (default): the groove removes the revolved volume from the base solid, as in previous versions.
• Common: the groove keeps only the volume shared between the revolved profile and the base solid, discarding everything else.

Свойства

Data

Groove

• ДанныеType (Enumeration)
• ДанныеBase (Vector): (read-only)
• ДанныеAxis (Vector): (read-only)
• ДанныеAngle (Angle)
• ДанныеAngle2 (Angle)
• ДанныеUp To Face (LinkSub)
• ДанныеReference Axis (LinkSub)

Part Design

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

Sketch Based

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

Start

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

Notes

• 0.21 and below: A ShapeBinder cannot be used for the profile.
• 0.21 and below: When using a SubShapeBinder for the profile, selecting the binder in the Tree View will fail, instead the binder's face has to be selected in the 3D View.