Part Loft

Description
The Part Loft command creates a face, a shell, or a solid shape from two or more profiles (cross-sections).

Usage

 * 1) There are several ways to invoke the command:
 * 2) * Press the button.
 * 3) * Select the option from the menu.
 * 4) The Loft dialog opens in the Task panel.
 * 5) In the Available Profiles list on the left click on the element to be used as sweep profile and click on the right arrow to place it in the Selected profiles list on the right.
 * Repeat for the second profile and again if more than two profiles are desired, then use the up and down arrows to reorder the selected profiles.
 * 1) Define options Create solid, Ruled surface, and Closed.
 * 2) 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 and complications, see below, however the profiles may come from Part Workbench primitives, Draft Workbench objects and Sketches.

Properties
See also: Property editor.

A Part Loft 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.
 * : true or false (default). True creates a solid.
 * : true or false (default). True creates a ruled surface.
 * : rue or false (default). True creates a closed loft by connecting last to first profile.
 * : Maximum degree.

Create solid
If "Create solid" is "true" FreeCAD creates a solid if the profiles are of closed geometry, if "false" FreeCAD creates a face or (if more than one face) a shell for either open or closed profiles.

Ruled surface
If "Ruled surface" is "true" FreeCAD creates a face, faces or a solid from ruled surfaces. Ruled surface page on Wikipedia.

Closed
If "Closed" is "true" FreeCAD attempts to loft the last profile to the first profile to create a closed figure.

For more info on how the profiles are joined together, refer Part Loft Technical Details page.



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 can not Sweep from a circle to a point, to a ellipse.
 * However you could Sweep from a point to a circle to an ellipse to another point.

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

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

PartDesign 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)

Part Workbench
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)

Closed Lofts

 * The results of closed lofts may be unexpected - the loft may develop twists or kinks. Lofting is very sensitive to the Placement of the profiles and the complexity of the curves required to connect the corresponding vertices in all the profiles.

An example Loft
The Loft command is in the Part Workbench, menu Part -> Loft... or via the icon in the toolbar.



In the "Tasks" will be two lists: "Available" and "Selected".



Selection of the sections
In the "Available" the available items are displayed. Two sections must be selected one after the first in this list.



Thereafter, with the blue arrow that item is added to the list of "Selected".



The selected items must be of the same type.

Tip: the active/selected items in the list are displayed in the 3D area as active/selected.

Command complete
If both sections are selected, the command can be completed with "OK".



Result
From closed lines we get surfaces which might be taken as a superficial look for solids.



If indeed a solid needs to be created, used the button "Create Solid" or after creating the Loft switch to its properties tab data and set the switch "Solid" to true.

The procedure is the same as described above with open polylines.

Changing the selection of sections
If you want to change the selection of the sections after creation of the loft, you can select the field Sections in the Data tab and click the occuring ellipsis button. The list of all selectable sections occurs, the current selection is highlighted. You can remove or add additional sections.

The sequence of sections depends on the sequence of clicks in the list. If you want to make substantial changes it is recommended to first deselect all and then start selection in the right order.