PartDesign Revolution/ja

PartDesign Revolution
Menu location
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

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

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.

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)

Sketch Based

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

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.