Revolve PropertyManager

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 Insert > Boss/Base > Revolve.
Revolved Cut (Features toolbar) or Insert > Cut > Revolve.
Revolved Surface (Surfaces toolbar) or Insert > Surface > Revolve.

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

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 .

Flip side to cut

(Revolved cuts and extruded cuts only) Removes all material from the outside of the profile. By default, material is removed from the inside of the profile.


Model with revolve sketch	Flip side to cut cleared	Flip side to cut selected

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.

Selected Contours

Use this option when you create a revolve using multiple contours.

Selected Contours

Select contours in the graphics area to create the revolve, as follows:

Hover over the region in the graphics area with the pointer . The region changes color.
Click in the region in the graphics area to create a preview of the revolve. You can select any combination of regions to create single or multibody parts.
Click .