パートデザイン・回転押し出し

This page is a translated version of the page PartDesign Revolution and the translation is 2% complete.

Pad

Additive Loft

PartDesign

Menu location
PartDesign Revolution
Part Design → Additive Features → Revolve
Workbenches
PartDesign
Default shortcut
None
Introduced in version
-
See also
PartDesign Groove

Description

The Revolution tool creates a solid by revolving a selected sketch or 2D object about a given axis.

Above: sketch (A) is revolved 270 degrees counter-clockwise around axis (B); resulting solid (C) is shown right.

Usage

Select a single sketch or one or more faces from the Body.
There are several ways to invoke the tool:
- Press the Revolve button.
- Select the Part Design → Additive Features → Revolve option from the menu.
Set the Revolution Parameters, see Options below.
Press the OK button.

Options

When creating a revolution, or after double-clicking an existing revolution in the Tree View, the Revolution 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 revolution:

Angle

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

To last

The revolution will extend up to the last face of the support it encounters in its direction. If there is no support, an error message will appear.

To first

The revolution will extend up to the first face of the support it encounters in its direction. If there is no support, an error message will appear.

Up to face

The revolution 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 revolution should extend in the opposite direction. The directions can be switched by checking the Reversed option.

Axis

Specifies the axis of the revolution:

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 revolution. 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.

Start

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

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

Angle

Defines the angle of the revolution. 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 revolution 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 revolution half the given angle to either side of the sketch or face. This option is only available if Type is Angle.

Project axis

introduced in 26.3: Projects the selected axis onto the profile plane if the profile is planar (only available for planar profiles). When unchecked (default), the axis is used in its original position and direction.

Reversed

Reverses the direction of the revolution.

Properties

Data

Part Design

データRefine (Bool)

Revolution

データType (Enumeration)
データBase (Vector): (read-only)
データAxis (Vector): (read-only)
データAngle (Angle)
データUp To Face (LinkSub)
データAngle2 (Angle)
データReference Axis (LinkSub)
データProject Axis (Bool): projects the reference axis onto the profile plane, see Options. introduced in 26.3

Sketch Based

データProfile (LinkSub)
データMidplane (Bool)
データReversed (Bool)
データAllow Multi Face (Bool)

Start

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

Limitations

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.