PartDesign AdditiveLoft

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.



Dialog-based workflow

 * 1) Press the  button.
 * 2) In the Select feature dialog select a sketch to be used as base profile object and click.
 * 3) * Alternatively, either a single sketch or the face of a 3D object can be selected prior to pressing the Additive loft button.
 * 4) In the Loft parameters, press the  button.
 * 5) Select the next sketch in the 3D view. Repeat to select more sketches in the order you want them to be lofted through. (You can change the section order any time later in the loft dialog by dragging sections in the list to the desired position.)
 * 6) Set options if needed and click.

Selection-based workflow

 * 1) Select several sketches. It is hereby important in what order you select them:
 * 2) * The sketch selected at first will become the base profile object in the next step
 * 3) * 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. (You can change the section order any time later in the loft dialog by dragging sections in the list to the desired position.)
 * 4) * The first or last selection can also be a face of a 3D object
 * 5) Press the  button.
 * 6) Set options if needed and click.

Options

 * Ruled surface: makes straight transitions between cross-sections. Does 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

 * : name given to the operation, this name can be changed at convenience.
 * : lists the sections used.
 * : see Options.
 * : see Options.
 * : true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details.
 * : the see base profile object of the loft.
 * : non applicable.
 * : non applicable.
 * : non applicable.
 * : non applicable.

Limitations

 * Only up to : It is not possible to loft to a Vertex. Since you can loft from or towards single vertices of sketches or bodies.
 * A cross-section cannot lie on the same plane as the one immediately preceding it.
 * Vertices can only be either the start or end of a loft. Otherwise the loft body would consist at its thinnest section only of a point. This would violates the CAD kernel's definition of a 3D object.
 * If the sketch has inner geometry, i.e. the loft is supposed to have holes, then the order in which the sketch geometry is created, should be the same for all sections: Either start all sections with the inner geometry or start them all with the outer. Otherwise an invalid loft can be created where inner and outer walls cross.
 * It is not possible to loft disjoint or crossing loops.

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.