Part Loft

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Overview
The FreeCAD Loft tool (Part Workbench), is used to create a face, faces or a solid shape from two or more profiles. The profiles can be a point (vertex), line (Edge) or wire. Edges and wires may be either open or closed. There are various limitations and complications, see below, however the profiles may come from the Part Workbench primitives, some Draft Workbench features and be created in a Sketch.

The Loft has three parameters, "Ruled","Solid" and "Closed" each with a value of either "true" or "false".

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

If "Solid" is "true" FreeCAD creates a solid if the profiles are of closed geometry, if "false" FreeCAD creates a face(s) for open profiles, or a shell from closed profiles.

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



limitations and complications

 * A vertex or point
 * vertex or point may only be used as the first and/or last profile in the list of profiles.
 * For example
 * you can not loft from a circle to a point, to a ellipse.
 * However you could Loft from a point to a circle to an ellipse to another point.
 * Open or closed geometry profiles can not be mixed in one single Loft
 * In one Loft, all profiles (lines wires etc.) must be either open or closed.
 * For example
 * FreeCAD can not Loft between one Part_Circle and one default Part_Line.
 * Draft Workbench features
 * Draft Workbench features can only be directly used if they have open geometry. Draft Workbench creates a face for all its closed features. It is possible to use the Draft upgrade/downgrade tools on a Draft closed geometry to create a wire which can then be used in a Loft.
 * For example
 * You can not directly use a Draft Polygon (unless you use the Draft downgrade tool).
 * You can directly use a Draft wire or Draft B-spline but only if it is not closed. If you close one, you would then have to use the Draft downgrade tool
 * 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_CreatePrimitives tool
 * The following Part geometric primitives can be a valid profile
 * Helix
 * Circle
 * Ellipse
 * Line (Edge)
 * Point (Vertex)
 * 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 tool is in the Part Workbench, menu Part -> Loft... or via the icon in the tool bar.



In the "Tasks" will be two lists: "node / wire" and "free form".



Selection of the elements
In the "node / wire" the available items are displayed. Two elements must be selected one after the first in this list.



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



The selected items must be of the same type, so.

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

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



result
From closed lines arise surfaces which might be taken at a superficial look for solids / solids.



If indeed a solid / solid to be created, can be used either when you create the button "Create Solid" or after creating the field properties tab data created the free-form surface of the switch "Solid" by pop be set to "true" / set properly.

The procedure is analogous open polylines.

FreeCAD Version

 * added Version 0.13
 * "closed" property added Version 0.14