When you create a feature by adding volume to a profile, you can define the feature extent (termination) in several ways. Termination options are available for extrude, revolve, sweep, and loft features.
To update features correctly when you change a design, avoid using faces and edges that you can change or remove. Where possible, use inclusive termination options, such as Through All rather than Between, to ensure that the feature persists, even if its termination geometry is removed.
Tips for creating sketched feature
-
base features
require an
unconsumed sketch
.
- For base features, use the Distance, Distance-Distance, Angle, or Angle-Angle fixed termination methods (in the Extents drop-down list). To Next, Between, To, and All termination methods are only available for parts with more than one feature.
- Features created after the base feature can use either an unconsumed sketch or the boundary of another feature as a profile. To use an existing feature, set the
sketch plane
on a feature. Then click to select the boundary as the
profile
to use for the new feature.
- To select multiple profiles, click all the profiles you want to include. To remove profiles from the selection set, press and hold Ctrl and click. A profile can be a single loop, multiple loops, intersecting loops, nested loops, or islands.
Geometry for terminating sketched feature
In most cases, you can terminate a sketched feature on several types of geometry:
- Select a Construction surface as a termination plane. Profiles can be extruded, revolved, lofted, or swept to form construction surfaces.
- Terminate features and surfaces on any combination of solid and surface features.
- Terminate extrusions on extended faces with analytic geometry other than planes.
Surface types for extended face
In addition to flat faces, you can terminate features on the faces of cylinders, elliptical cylinders (with no draft), cones, spheres, and toroids.
Uses for Move Feature
You can drag a feature that belongs to a part file deep in the assembly hierarchy. It is not necessary to in-place activate any subassemblies, or the part containing the feature.
Drag to "cruise move" a feature to a new planar face. The feature sketch reattaches to the new plane, breaking its link with the original face. If the new position is not a planar face, a fixed work plane is automatically created on which to place the feature.