Lofted shape

This command allows you to create a shape by selecting a profile, segment or face.

Creation Stages / Use:

Click on the icon or choose the command Surface > Lofted... from the drop down menu.

Choose the type of loft: closed or open (periodically or not).
Select loft profiles.
Choose the synchronization mode.
Choose if you want the lofted shape to be surfacic or solid.

To define the sections of a loft, it is possible to select a sketch, a segment of a sketch, or a planar face (only for the extremities sections of the loft)

Available Options:

Closed:

This option creates a periodic loft, turning back on itself. TopSolid also links the first and the last section.

No option	With the option

Surfacic:

If you check this check box, then the lofted shape will be surfacic and open at its extremities

Guides:

Guide profiles constrain the lofted shape to change along the profile between sections.

No option	With the option

Options on section labels:

On each section, there is an arrow and a label.

The arrow's hook point corresponds to the origin of the section, and the arrow indicates the profile's direction.

All sections must be in the same direction.

You can either edit the value in the label (Coefficient varying from 0 to 1), or dynamically move the point indicated by the label by dragging it with the mouse. Another way is to double click the symbol of the label to switch to point, double click again to edit the label and select a point.

The position of the origins on each section is very important and greatly influences the final result of the lofted shape.

Tangency and curvature constraints (popup menu on the section):

To use this option, right-click the desired section and select "Add Constraint".

This option allows you to apply a constraint to the lofted shape at this section.

There are two types of constraints:

Curve: The lofted shape is adjusted so as to be tangent to the reference face and so as to follow the curve of the latter.

Tangency: The lofted shape is adjusted to be tangent to the selected data reference face or plane.

Double click on the plane or surface icon in the label to change from one to the other.

A coefficient defines the magnitude of the tangency. The higher the coefficient, the more the tangency is pronounced.

Constraint = None	Constraint = Tangency	Constraint = Curvature

Guides synchronization:

The synchronization represents the way TopSolid make the section correspond with each other.

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

Curvilinear: When you use curvilinear 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.

Parametering: When you use parametric 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]

With the local and arc length modes, the edges of the obtained surface are created by approximation with some BSpline (curve), by following either the curvilinear abscissa either the reference profile arc length.

With the free mode, TopSolid does not use the approximation with BSplines to ensure that the simplification (lofted advanced option) gives better results.

Only exceptions where the approximation is used in free mode:

- In the profile/profile correspondence if the number of profiles segments is different.
- In the point/point correspondence if the number of segments between consecutive points is different.

Correspondence points:

This option defines points of correspondence between sections in order to structure the change of the lofted shape.

You can:

add a new set of correspondence points
delete an existing correspondence
insert a new correspondence.

When you enable this option, a box appears, where you add all of the points (in order) for a set of correspondences. Once the set has been defined, validate it with . You can then select the next list of points. Once all correspondence point sets have been defined, click in the box to finish defining correspondences.

The set of correspondence points must be defined in order, depending on the profile direction.

Each point in a set must also be selected in the same order as the sections.

Correspondence:

Different types of correspondence are:

Profile to profile: During the shape creation, TopSolid overall matches profiles regarding their built settings (example: a circle is parameterized by an angle). It is the default mode, it usually gives satisfying results.

Segment to segment: During the shape creation, TopSolid tries to match two by two segments of each profiles. The result is a surface for each pair of segments. This option is only available when profiles have the same number of segments.

Point to point: If this mode is selected, you have to select manually corresponding points two by two between profiles.

With the profile/profile correspondence, if you select guides curves, the synchronization will be applied by section (by intersection between guides curves and profiles defining correspondence points).
With other correspondences (Segment to segment and Point to point) the user has to check that guides curves don't intersect the correspondence.

When adding a batch of points with the contextual menu, TopSolid updates the point position during the first profile selection. TopSolid also checks the consistency of other points during the correspondent point selection on the second profile.
All correspondences in this dialog are saved. It allows to switch from points/points to profile/profile and switch back to points/points.

Division of faces:

	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 segment of the section.
	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.

Derivation magnitude:

This option allows to smooth or not the derivation magnitude between profiles.

Single: the derivation magnitude is alone.

Smooth: the derivation magnitude is smoothed between profiles for a more aesthetic result.

Simplify Surfaces :

This option simplifies the geometry of some surfaces.

By default, surfaces from this command are b-spline surfaces. According to the reference profiles, some surfaces could be simplified into planar, cylindrical or conical surfaces.