Part Sweep

Description
The Part Sweep command creates a face, a shell, or a solid shape from one or more profiles (cross-sections) distributed along a spine.

The Part Sweep command is similar to Part Loft with the addition of a spine.



Usage

 * 1) There are several ways to invoke the command:
 * 2) * Press the button.
 * 3) * Select the option from the menu.
 * 4) The Sweep task panel opens.
 * 5) In the Available Profiles list on the left select a profile and click on the right arrow to place it in the Selected profiles list on the right.
 * 6) Repeat if more than one profile is desired.
 * 7) The up and down arrows have no purpose, the position of the profiles along the spine determines in what order they are used.
 * 8) Click on the  button, then choose either mode of selection:
 * 9) * Segment selection: select one or more contiguous edges in the 3D view (press for multiple selection) and click . The sweep will only be generated along the selected edges.
 * 10) * Complete path selection: switch to the Tree view, select the object to be used as spine, switch back to the task panel and click . The sweep will be generated along all the contiguous edges found in the object.
 * 11) Define options Solid and Frenet.
 * 12) Click.

Accepted geometry

 * Profiles: can be a point (vertex), line (edge), wire or face. Edges and wires may be either open or closed. There are various Limitations, see below.


 * Path: can be a line (edge) or a series of connected lines, a wire or various Part Workbench objects, Draft Workbench objects or a Sketch. The path may be either open or closed.


 * App Link objects linked to the appropriate object types and App Part containers with the appropriate visible objects inside can also be used as profiles and paths.

Properties
See also: Property editor.

A Part Sweep object is derived from a Part Feature object and inherits all its properties. It also has the following additional properties:

Data

 * : lists the sections used.
 * : spine (path) to sweep along.
 * : true or false (default). True creates a Solid.
 * : true or false (default). True uses Frenet algorithm.
 * : transition mode. Options are Transformed, Right corner or Round corner.

Solid
If "Solid" is set to "true", FreeCAD creates a solid, provided the profiles are closed; if set to "false", FreeCAD creates a face or a shell for either open or closed profiles.

Frenet


The "Frenet" property controls how the profile orientation changes as it follows along the sweep path. If "Frenet" is "false", the orientation of the profile is kept consistent from point to point. The resulting shape has the minimum possible twisting. Unintuitively, when a profile is swept along a helix, this results in the orientation of the profile slowly creep (rotate) as it follows the helix. Setting "Frenet" to true prevents such a creep.

If "Frenet" is "true" the orientation of the profile is computed basing on local curvature and tangency vectors of the path. This keeps the orientation of the profile consistent when sweeping along a helix (because curvature vector of a straight helix is always pointing to its axis). However, when path is not a helix, the resulting shape can have strange looking twists sometimes. For more information, see Frenet Serret formulas.

Transition
"Transition" sets the transition style of the Sweep at a joint in the path, if the path does not define the corner transition (for example where the path is a wire). The property is not exposed in the Task panel and can be found in properties after the Sweep has been created.

Vertex or point
A vertex or point may only be used as the first and/or last profile in the list of profiles. For example:
 * You cannot Sweep from a circle to a point, to an ellipse.
 * You can however Sweep from a point to a circle to an ellipse to another point.

Profiles
In one Sweep, all profiles (lines wires etc.) must be either open or closed. For example:
 * FreeCAD cannot Sweep between one Part Circle and one Part Line.

Sketches

 * The profile may be created with a sketch. However only a valid sketch will be shown in the list to be available for selection.
 * The sketch must contain only one open or closed wire or line (can be multiple lines, if those lines are all connected as they are then a single wire).

Draft Workbench objects
Draft Workbench objects can be directly used as a profile. For example the following Draft objects can be used as profiles in a Part Sweep:
 * Point
 * Line, Wire
 * B-spline, Bezier Curve
 * Circle, Ellipse
 * Rectangle, Polygon

Part Workbench objects
The profile can be a valid Part geometric primitive which can be created with the Part Primitives command. For example the following Part geometric primitives can be a valid profile:
 * Point (Vertex)
 * Line (Edge)
 * Helix, Spiral
 * Circle, Ellipse
 * Regular Polygon
 * Plane (Face)

Links

 * Since Sweep is often used to create threads for screws, you should see Thread for Screw Tutorial.