The profile can be revolved through any angle measuring between zero and 360 degrees around an axis. The axis of revolution can be part of the profile or offset from it. The profile and axis must be coplanar.
The Revolve command is used to create features having radial symmetry, such as stepped shafts, cylindrical containers, or O-rings. Such features can define the overall shape of a part (a base feature) or become details such as fins, webs, or struts.
Revolving around an axis on the sketch produces solid features, such as disks, hubs, and beveled gear blanks. Revolving around an axis that is offset from the sketch creates solids with holes, such as washers, flasks, and conduits.
When you specify a sphere or torus in the Primitives panel, the sketch creation and revolve process is automated. You can select a start plane for the sketch, create the profile, and then create a solid. The primitive shape creation commands create full revolutions and do not create surfaces or partial revolutions.
Shape propagation only applies to open profiles. It describes solutions that are defined through the extension of the open ends of the profile and by the shape of the body. Shape propagation generates a feature that is robust to topology changes in the part body caused by editing features higher up in the feature tree. The revolved feature is not dependent upon a strictly defined profile consisting of specific referenced edges and sketch lines.
There are two types of shape propagation: Match Contour and Match Shape.
Match Contour When the Match Shape option is disabled, the open profile is closed by extending the open ends of the profile until they intersect the solid body. If the sketch plane of the profile lies on a planar face, the loops of the face are used to close the profile. Otherwise, the edges defined by the intersection of the profile plane with the body are used to close the profile. A valid profile exists if both ends of the open profile intersect either the body or the revolve axis. Mixed sets are not valid. When a closed profile is created, you select Side to Keep for the profile.
Match Shape When the Match Shape option is selected, a flood-fill type solution is created. The open ends of the profile are extended to the axis of revolution, if possible, or to the bounding box of the body. The Match Shape revolution generates a stable and predictable body for topology changes on the defining faces. The revolved feature is not dependent on a strictly defined profile consisting of sketch lines and referenced edges.
On the Model tab, Create panel, click Revolve to create a feature by rotating one or more sketched profiles around an axis. The axis and the profile must be coplanar. The first feature is the base feature.
Selects a profile to revolve. If there are multiple profiles and none are selected, click Profile, and then click one or more profiles in the graphics window. Press Ctrl, and then click to remove a profile from the selection set.
Single Profile Automatically selects a profile.
Multiple Profiles Selects multiple profiles from same sketch plane. Selections are highlighted.
Nested Profiles Selects multiple nested profiles. The result of revolving an interior loop is opposite the result of revolving an exterior loop. For example, revolved concentric circles form a hollow torus.
Selects the axis of revolution. The axis can be a work axis, a construction line, or a normal line.
Selects the participating solid body in a multi-body part.
Specifies the sketch plane or the participating solid bodies.
Plane Selects a 2D plane or planar face.
| ||Solids Selects the participating body in a multi-body part.|
Specifies if the revolved feature is a solid or surface.
Creates a solid feature from an open or closed profile. Open profile is not available for base features or primitives.
Creates a surface feature from an open or closed profile. Can be used as a construction surface on which other features terminate or used as a split tool to create a split part.
Specifies whether the revolution joins, cuts, or intersects with another feature. Not available for base features but required for all other features.
Join Adds the volume created by the revolved feature to another feature.
Cut Removes the volume created by the revolved feature from another feature or body.
Intersect Creates a feature from the shared volume of the revolved feature and another feature. Material not included in the shared volume is deleted.
| ||New solid Creates a new solid body. This is the default selection if the revolve is the first solid feature in a part file. Select to create a new body in a part file with one or more solid bodies. Each body is an independent collection of features separate from other bodies. A body can share features with other bodies.|
Determines the method for the revolution and sets the angular displacement of the profile around a centerline. Click the arrow to list the extent methods, select one, and then enter a value. Revolutions can be a specific distance or can terminate on a work plane or part face.
Angle - Angle Accepts two different angular values to revolve the profile in two directions - one positive and one negative. Click Asymmetric to activate and enter the second angular displacement value.
To - Next Selects the next possible face or plane on which to terminate the revolution in the specified direction. Dragging the profile flips the revolution to either side of the sketch plane. Not available for base features. Terminator selects a solid or surface on which to terminate the revolution. Flip specifies the direction.
Match Shape When the Match Shape option is selected, a flood-fill type revolved feature is created. The open ends of the profile are extended to the axis of revolution (if possible), or to the bounding box of the body. The Match Shape revolution generates a stable and predictable body for topology changes on the defining faces.
Match Contour If you cancel the Match Shape option, the open profile is closed by extending the open ends of the profile to the part, and closing the gap between them by including edges defined by the intersection of the sketch plane and the part. The extrusion is created as if you specified a closed profile.
Select the check box to place an iMate automatically on a full circular edge. Autodesk Inventor LT attempts to place the iMate on the closed loop most likely to be useful. In most cases, place only one or two iMates per part.