The Revolve PropertyManager appears when you create a new revolve feature, or when you edit an existing revolve feature. You can specify separate end conditions for each direction (clockwise and counterclockwise from the sketch plane).
To open this PropertyManager, click one of the following tools:
- Revolved Boss/Base
(Features toolbar) or .
- Revolved Cut
(Features toolbar) or .
- Revolved Surface
(Surfaces toolbar) or .
Some fields that accept numeric input allow you to create an equation by entering = (equal sign) and selecting global variables, functions, and file properties from a drop-down list. See Direct Input of Equations in PropertyManagers.
Axis of Revolution
 |
Axis of Revolution |
Select an axis around which the feature revolves. This can be a centerline, line, or an edge, depending on the type of revolve feature you create. |
Direction1
Defines the revolve feature in one direction from the sketch plane.
Revolve Type |
Sets the end condition of the revolve feature relative to the sketch plane. To reverse the revolve direction, click Reverse Direction . Select one of these options:
Blind
|
Creates the revolve in one direction from the sketch. Set the angle covered by the revolve in Direction 1 Angle .
|
Up to Vertex
|
Creates the revolve from the sketch plane to the vertex you specify in Vertex .
|
Up to Surface
|
Creates the revolve from the sketch plane to the surface you specify in Face/Plane .
|
Offset from Surface
|
Creates the revolve from the sketch plane to a specified offset from the surface you specify in Face/Plane . Set the offset in Offset Distance . To offset in the opposite direction, select Reverse offset.
|
Mid-Plane
|
Creates the revolve in the clockwise and counterclockwise directions from the sketch plane, which is located at the middle of the revolve Direction 1 Angle .
|
|
Merge result (Boss/Base revolves only) |
Merges resultant body into an existing body if possible. If not selected, the feature creates a distinct solid body.
|
Direction2
(Optional.) After completing Direction1, select Direction2 to define the revolve feature in the other direction from the sketch plane.
The options are the same as in Direction1.
Thin Feature
|
Type |
Defines the direction of thickness. Select one of these options:
One-Direction
|
Adds the thin-walled volume in one direction from the sketch.
To
reverse the direction in which the thin-walled volume is
added, click
Reverse Direction
.
|
Mid-Plane
|
Adds the thin-walled volume using the sketch as the middle, and applying thin-walled volume equally on both sides of the sketch.
|
Two-Direction
|
Adds the thin-walled volume on both sides of the sketch. Direction 1 Thickness adds thin-walled volume outward from the sketch. Direction 2 Thickness adds thin-walled volume inward from the sketch.
|
|
 |
Direction 1 Thickness |
Sets the thin-walled volume thickness for One-Direction and Mid-Plane thin feature revolves. |
Feature Scope
Specifies which bodies or components you want the feature to affect.
- For multibody parts, see Feature Scope in Multibody Parts.
- For assemblies, see Feature Scope in Assemblies.