Part Loft
Part Loft |
Menu location |
---|
Part → Loft... |
Workbenches |
Part |
Default shortcut |
None |
Introduced in version |
0.13 |
See also |
Part Sweep |
Description
The Part Loft command creates a face, a shell, or a solid shape from two or more profiles (cross-sections).
Part Loft from three profiles which are two Part Circles and one Part Ellipse. Parameters are Solid "True" and Ruled "True".
Usage
- There are several ways to invoke the command:
- Press the Loft... button.
- Select the Part → Loft... option from the menu.
- The Loft task panel opens.
- In the Available Profiles list on the left select the first 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.
- Optionally use the up and down arrows to reorder the selected profiles.
- Define options Create solid, Ruled surface, and Closed.
- Click OK.
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.
- 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. introduced in version 0.20
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
Loft
- DataSections (
LinkList
): lists the sections used. - DataSolid (
Bool
): true or false (default). True creates a solid. - DataRuled (
Bool
): true or false (default). True creates a ruled surface. - DataClosed (
Bool
): rue or false (default). True creates a closed loft by connecting last to first profile. - DataMax Degree (
IntegerConstraint
): 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.
Limitations and complications
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.
- Primitives: Box, Cylinder, Sphere, Cone, Torus, Tube, Create primitives, Shape builder
- Creation and modification: Extrude, Revolve, Mirror, Fillet, Chamfer, Make face from wires, Ruled Surface, Loft, Sweep, Section, Cross sections, 3D Offset, 2D Offset, Thickness, Projection on surface, Attachment
- Boolean: Make compound, Explode Compound, Compound Filter, Boolean, Cut, Fuse, Common, Connect, Embed, Cutout, Boolean fragments, Slice apart, Slice, XOR
- Measure: Measure Linear, Measure Angular, Measure Refresh, Clear All, Toggle All, Toggle 3D, Toggle Delta
- Getting started
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- Basics: About FreeCAD, Interface, Mouse navigation, Selection methods, Object name, Preferences, Workbenches, Document structure, Properties, Help FreeCAD, Donate
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