PartDesign AdditiveLoft
PartDesign AdditiveLoft |
Menu location |
---|
Part Design → Additive loft |
Workbenches |
PartDesign |
Default shortcut |
None |
Introduced in version |
0.17 |
See also |
PartDesign AdditivePipe |
Description
Additive Loft creates a solid in the active Body by making a transition between two or more sketches (also referred to as cross-sections). If the Body already contains features, the additive loft will be merged to them.
On the left: cross-sections (A), (B) and (C); created Additive loft on the right.
Usage
Dialog-based workflow
- Press the Additive loft button.
- In the Select feature dialog, select a sketch to be used as base profile object and click OK.
- Alternatively, a single sketch can be selected prior to pressing the Additive loft button.
- In the Loft parameters, press the Add Section button.
- Select the next sketch in the 3D view. Repeat to select more sketches in the order you want them to be lofted through.
- Set options if needed and click OK.
Selection-based workflow
- Select several sketches. It is hereby important in what order you select them:
- The sketch selected at first will become the base profile object in the next step
- The sketches selected after the first one will become the loft sections. Also here the selection order is important: The sketch selected as second will become the first loft section, the one selected as third becomes the second section and so on.
- Press the Additive loft button.
- Set options if needed and click OK.
Options
- Ruled surface: makes straight transitions between cross-sections. Dos not apply to a loft with two cross-sections. If not checked, transitions will be smooth.
- Closed: makes a transition from the last cross-section to the first, creating a loop.
Properties
- DataLabel: name given to the operation, this name can be changed at convenience.
- DataSections: lists the sections used.
- DataRuled: see Options.
- DataClosed: see Options.
- DataRefine: true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details.
- DataProfile: the see base profile object of the loft.
- DataMidplane: non applicable.
- DataReversed: non applicable.
- DataUp To Face: non applicable.
- DataAllow Multi Face: non applicable.
Limitations
- Sketches must form closed profiles.
- It is not possible to loft to a vertex.
- A cross-section cannot lie on the same plane as the one immediately preceding it.
- To better control the shape of the loft, it is recommended that all the cross-sections have the same number of segments. For example, for a loft between a rectangle and a circle, the circle may be broken down into 4 connected arcs.
- Loft will be created in the order that cross sections were added
Known Issues
- Some failure modes will turn the part black
Links
- Part Loft Technical Details explains how a Part Loft is created, much of its content is relevant to the PartDesign Additive loft.
PartDesign
- Structure tools: Part, Group
- Helper tools: Create body, Create sketch, Edit sketch, Map sketch to face
- Modeling tools
- Datum tools: Create a datum point, Create a datum line, Create a datum plane, Create a local coordinate system, Create a shape binder, Create a sub-object(s) shape binder, Create a clone
- Additive tools: Pad, Revolution, Additive loft, Additive pipe, Additive helix, Additive box, Additive cylinder, Additive sphere, Additive cone, Additive ellipsoid, Additive torus, Additive prism, Additive wedge
- Subtractive tools: Pocket, Hole, Groove, Subtractive loft, Subtractive pipe, Subtractive helix, Subtractive box, Subtractive cylinder, Subtractive sphere, Subtractive cone, Subtractive ellipsoid, Subtractive torus, Subtractive prism, Subtractive wedge
- Transformation tools: Mirrored, Linear Pattern, Polar Pattern, Create MultiTransform, Scaled
- Dress-up tools: Fillet, Chamfer, Draft, Thickness
- Boolean: Boolean operation
- Extras: Migrate, Sprocket, Involute gear, Shaft design wizard
- Context menu: Set tip, Move object to other body, Move object after other object, Appearance, Set colors
User documentation
- Getting started
- Installation: Download, Windows, Linux, Mac, Additional components, Docker, AppImage, Ubuntu Snap
- Basics: About FreeCAD, Interface, Mouse navigation, Selection methods, Object name, Preferences, Workbenches, Document structure, Properties, Help FreeCAD, Donate
- Help: Tutorials, Video tutorials
- Workbenches: Std Base, Arch, Assembly, CAM, Draft, FEM, Inspection, Mesh, OpenSCAD, Part, PartDesign, Points, Reverse Engineering, Robot, Sketcher, Spreadsheet, Start, Surface, TechDraw, Test Framework, Web
- Hubs: User hub, Power users hub, Developer hub