A multi-sections solid feature involves transitional surfaces being created between multiple selected sketches. The creation of a multi-sections solid between two sketched sections is shown in the image below.

The transitional surfaces are created by connecting the vertices of the selected sketches with splinar surfaces. The closing points indicate the first two vertices to connect. The system follows the sections in the direction indicated by the arrow.

The shape of a Multi-section's solid feature is controlled using one or more of the parameters described in the image below. These parameters are defined using the Multi-sections Solid Definition dialog box.

General Steps

Use the following general steps to create and control a multi-sections solid feature:

Start the creation of the multi-sections solid feature.
Control the profile geometry with guides and spines.
Set the Coupling and Relimitation options.

The techniques used to create sections for an advanced multi-sections solid are the same as those used to create sections for basic multi-sections solids.

To begin the creation of a multi-sections solid feature, select the icon in the Sketched-Based Features toolbar. The Multi-sections Solid Definition dialog box appears as shown in the image below.

Sections for the feature are added by selecting curve geometry or sketches from the model or specification tree. The sections are added to the top of the dialog box, as shown in the image below.

A section for a multi-sections solid can also be specified by selecting a face on the model that consists of a closed boundary. A multi-sections solid section requires the selection of curves; therefore, CATIA automatically adds an extract and boundary feature under the multi-sections feature. The extract feature creates an associative copy of the selected face. The boundary of the extract surface is then used as the multi-sections solid section. An example is shown in the image below.

Once the sections are selected, advanced options (such as guides and spines) can be added.

Guides

Guides provide an absolute path to blend the sections of the multi-sections solid together. The guide curve must intersect each section of the solid feature. More than one guide can be used to control the multi-sections solid. The multi-sections solid only progresses as far as the last section, regardless of the length of the guide.

Although a guide can be created using a sketch, the curve is typically three-dimensional and created using wireframe features (e.g, spline) from the Generative Shape Design workbench.

In the image below, a splinar guide is created that connects the two sketches and extends past the end section.

The intersection of the guide and the multi-sections solid creates a vertex.

To use the guide in the multi-sections solid feature, select it in the Guides tab of the Multi-sections Solid Definition dialog box, as shown in the image below, and select the guide from the screen.

The multi-sections solid shown in the image below is created with a guide to control the internal surface. Notice the difference between this multi-sections solid and the multi-sections solid in the image below.

Spine

A spine controls the shape of the multi-sections solid as it progresses from one section to the next. The cross-section of the multi-sections solid must always be perpendicular to the spine. Therefore, only one spine can be selected for a multi-sections solid. The spine can be defined by a sketch, edge, or curve.

To specify a spine, select the Spine tab in the Multi-sections Solid Definition dialog box, as shown in the image below, and select the spine geometry to use.

If the Multi-section feature cannot remain perpendicular to the spine while travelling through each section, the feature will fail.

If a spine is not specified, CATIA computes a default spine to control the shape of the multi-sections solid throughout its progression. To deselect a spine and specify a system-default spine, select the Computed spine option.

Coupling

The coupling option is used to define the transitions between the sections. These options are described in the image below.

If a coupling option is used and the criteria described is not met, an error message appears when attempting to generate the Loft feature. For example, setting the coupling option to Vertices results in an error message if attempting to create transitions between a square and a circular section. This error occurs because the circular section does not have any vertices to couple with the square section.

Relimitation

Relimitation controls the progression of the multi-sections solid feature beyond the sections. By default, a multi-sections solid is relimited at both the start and end sections. CATIA only creates the transitional surfaces of the multi-sections solid between the first and last selected sections.

By disabling multi-sections solid relimitation and using a guide, the geometry can extend as far as the shortest guide. the image below shows the same multi-sections solid in the image below, except that the Relimited on the end section option is not selected. Notice how the multi-sections solid now extends past the last section. The shape of the multi-sections solid's cross-section in this area is controlled by the last section. The trajectory of the multi-sections solid is controlled by the guide.

To specify Relimitation, select the Relimitation tab of the Multi-sections Solid Definition dialog box and clear the Relimited on the end section option.

A spine can also control the relimitation of a multi-sections solid. The two models shown in the image below are created with the Relimited on the end section option not selected.

Smooth Parameters

Smooth parameters provide additional control over the shape of the multi-sections solid feature by attempting to smooth its shape between sections. Access the smooth parameters options from the bottom of the Multi-sections Solid Definition dialog box, as shown in the image below. These options are described in the image below.