Swept

This command allows you to create a surface or solid shape by making one or more sections (open or closed) run along one or two trajectories.

Creation Stages / Use:

Click the icon or select the Surface > Swept... command from the drop-down menu.

Select the path or paths.

Then select the sections and their hooking points on the paths.

Available Options:

Paths:

This path corresponds to the trajectory followed by the sections in order to generate the surface.

By checking the "Second path" check box, you can select a second trajectory.

The shape is thus created by making the sections travel between two paths by applying a scale on the sections in order to follow the evolution of the paths.

One path	Two Paths

An arrow is hooked to the start of each path and thus indicates the travel direction. When two paths are used, the travel directions must be the same on each path.

To invert the direction, simply double-click the arrow of the path in question.

Sections:

This option allows you to define the section(s) of the swept shape.

The sections must be designed in place.

They must be planar and all be open or all be closed

For each section, it is necessary to define:

- the profile to use as a section

- its position and hooking point on each path.

The positioning point corresponds to the point that will act as a reference to calculate the movement of the section along the path.

The "Automatic hooking" allows you to automatically use the intersection point, detected between the plane of the section and the path, as the positioning point.

Warning, if the plane of a section intersects the path several times (in the case of a closed path for example), the point chosen by the software might not be correct. Therefore you should verify which point has been chosen by using the list of sections in the dialog.

On each section an origin and a "drawing direction" of this profile represented by a point and arrow are defined.

The coefficient (variable from 0 to 1) determines the origin position of the profile (0: at the start; 1: at the end). Double-click the numeric value to modify it.

By double-clicking the small symbol in front of the coefficient, you can change the definition mode of the origin position.

The "point" mode allows you to select a point on the profile as being the new origin rather than using a coefficient.

In order for the swept shape to be created correctly and for it not to twist, the section origins must be aligned.

Alignment:

This option allows you to define how the section travels along the path.

Normal: The section moves while remaining normal to the path.
Vertical: The section moves while keeping an orientation in relation to a defined direction.
Parallel: This section moves in a manner parallel to its initial orientation.

You will find more options on the Section alignment page.

Surface:

By checking this option, the shape obtained will be a hollow surface without thickness and not a full shape.

Limits:

This option allows to define limits of a swept surface by adding start and end points on each path.

Example of a swept surface with start and end limits.

Start points can only be selected if the first section is not on the origin of the path. These points have to be before or on the first section position.
End points have to be on or after the last section position.

Advanced Options:

Synchronization:

The sections Synchronization define the way TopSolid make the sections corresponds with each other.

Free: This test mode adapts sweeping best between section using a combination of various methods.

Local: When you use local synchronization for the sweep, this means that when the shape is created, the sweep on the curves in done in proportion to the length of each one.

Arc length: When you use arc length synchronisation for the sweep, this means that when the shape is created, the software tries to correspond to the nature settings of the sections.

Example:

The parametric extension for a line is [0;1] (length)

The parametric extension for a circle is [0;360] (angle)

a: Line : parametric extension [0;1]

b: Arc: Parametric Extension [0;54]

	Minimal division of faces. This mode allows you to smooth the section and the path in order to obtain the face minimum on the resulting form.
	Division of the faces into columns, according to the segments of the section. . Only the path is smoothed in order to obtain faces for each section segment.
	Division of the faces into the grid, according to the segments of the section and of the path. . No smoothing is performed, and a face grid is generated by the segments of the section and the path.

Mixing:

This option allows you to determine the manner in which the shape changes from one section to another. The details explaining this mode are provided on the page: Section mixing.

Repair self-intersections:

This option deletes auto-intersections between surfaces of the shape when this is the case.

Create sections:

This option allows to create different sections of the surface to create. The number of wanted sections has to be entered.