Sweeps build a 3D shape with a profile and a path.
What do you need to build a sweep? A profile and a path. The profile can be sketches, an existing part face or an existing solid. Sketch the path or use existing edges. You can sweep along 2D and 3D paths.
Pro Tip: Ensure you are orientating sketched profiles properly to the path. A good rule is to have the profile’s plane intersect the path at its starting point.
As with all Create features, you can build the feature as a solid or as surfaces. For solid sweeps, you can select closed 2D or 3D sketch profiles or a closed face loop. For surface sweeps, select open or closed sketch profiles or a face loop of the part.
If there is only one profile in the sketch, Inventor automatically selects it.
When the sweep is the first feature, Inventor adds it as a new solid. When sweeping as a secondary feature, you can add volume (Join), remove volume (Cut) or build intersections (Intersect).
When you need a hollow body, consider shelling the model instead of using a multi-loop profile, especially if you are making more complex models.
The default Orientation is Follow Path. This means Inventor keeps the profile constant and normal to the path as it moves along the path.
With Follow Path, use the Taper option to scale the profile up or down from the starting profile.
With single-loop profiles, a positive angle tapers away from the profile, increasing the section area as it transitions along the path. A negative angle decreases the area. Note that specifying a negative taper could lead to the sweep finishing before the end of the path.
With multi-loop nested profiles, Inventor applies the taper angle to the outer loop. Inner loops get the opposite angle.
The Twist option manages the profile rotation as it follows the selected path. The angle sets how much the profile twists (rotates) around the path’s axis. Positive angles mean a counterclockwise rotation and negative angles mean a clockwise rotation.
Twist is a useful feature, especially when you are sweeping along 3D paths to get the desired profile result at the end of the path.
Toolbodies
Within Inventor, you sweep an existing solid along a path. The selected solid is called a toolbody. Use this to model complex shapes, create mechanical designs (like threads, springs, grooves) and to simulate toolpaths.
The toolbody can be any solid object, in any shape. You can sweep toolbodies along 2D- or 3D-sketched paths. Inventor combines the toolbody with the path during the sweep to create a new solid.
More Sweep Types
With the Fixed orientation, the profile retains the same orientation throughout the sweep.
Guide Rails are sketched curves that provide more control over the shape. Consider the rails constraints that limit profile movement. The path and rail must intersect the profile plane.
The chosen Profile Scaling option determines how the swept profile scales to meet the guide rail. Select None when you want to keep the profile in a constant shape and use the rail only to manage a twist. A value for X will have Inventor scaling the profile only in the X direction. With X & Y values, Inventor scales the profile in both directions as the sweep progresses.
You can also use surfaces (including faces) as guides. The selected surface controls the profile twist, keeping the profile aligned with the surface as it transitions through the sweep. Think of the profile like an airplane and the surface managing the orientation of the wings.
It is easy to fall into the habit of using sweeps only for tube, pipes, hosing and springs. However, there are plenty of other opportunities to use them. Channels, grooves, slides and even lawn mower blades are all best modeled with sweeps.
