Multiple Intersections

This command allows to create intersection profiles between a shape or faces and parallel planes.

These profiles could be used to define a shape with the Surface >Fitting... command.

Creation stages / Use:

Select the 3D Sketch > Operations > Multiple Intersections... command from the drop-down menu.

Select the shape or faces to intersect.
Select the definition mode of sections planes (parallel planes or from guide profiles).
Define the selected mode (profiles, points count, distribution, ...).
Validate.

Available options:

Parallel planes and guide profiles:

These area allows to define sections count and the construction rule of section planes.

Parallel planes: construction of parallel planes sections or radial sections.
Enter points count (equivalent to sections count).
Specify if the distribution is done along a direction (parallel planes sections) or around an axis (radial sections).
Select the direction or axis.


Distribution along a direction	Distribution around an axis

The guide profile is not trimmed with the useful part of selected faces.

In the distribution around an axis, sections count is calculated at 360°. In this case we could have a planes superposition and sections superpositions.

Distribution of 10 points around an axis

Sections 7, 8, 9 and 10 are superposed with 2, 3, 4 and 5

To limit sections distribution on the selected face, use the Profile extremities option.

Guide profiles with created points:
Selected guide profiles and make sure directions are the same on all profiles.
Enter points count (equivalent to sections count).
Specify the distribution mode (they are the same that in the Seedling on profile command). It can be by length profile (all points will be separated by an identical distance according to the curvilinear length), along a direction (all points will be separated by an identical distance according to a length projected on an axis) or around an axis (all points will be separated by an identical angle around an axis). This latest distribution mode is available with the One guide profile mode only.

By length distribution

Curvilinear lengths (green profiles and red profiles) are the same

Along a direction distribution

Lengths between each projected points are the same

Select the direction or axis.
Use tangent as planes normal direction: option available with One guide profile mode only. With this mode, to know the normal of section plane TopSolid uses a tangent on the guide profile on each points. Unchecking this option this normal can be replaced by a direction that will be the same for each points.


Checking the option, TopSolid uses a tangent on the guide profile on each points (here the used guide profile is the external edge of the shape)	Unchecking the 'option, all sections are normal to the profile used as fix direction (here the red dotted profile)

Gudie profiles with preexisting set of points: preexisting points allow to control and modify the exact position of each section.
Selected guide profiles and make sure directions are the same on all profiles.
Selected the preexisting set of points on the profile (equivalent to sections count). These points can be explicit points, serial points or seedling on profile.
Use tangent as planes normal direction: option available with One guide profile mode only. With this mode, to know the normal of section plane TopSolid uses a tangent on the guide profile on each points. Unchecking this option this normal can be replaced by a direction that will be the same for each points.

Profile extremities:

When the multiple intersection is created with the first mode Created points, then it is possible to trim the guide profile(s) between two points in order to work into a specific area without having to do preliminary construction. It is possible to use one point only (first or second) or both.

Example of trim between two points

Extension:

Sew:

Intersection between a plane and a set of faces can create one or several interrupted profiles (when faces are drilled or with non convex set of faces).

These options allow to join interrupted profiles with a line or a tangent spline.


Example of interrupted section by a drilling using the Keep only one part mode	Using the Sew with line mode	Using the Sew with spline mode

Sections must pass by guide profiles:

These option allows to keep sections passing by the guide profiles only. It is useful working with a closed guide profile.


Unchecking the option all sections are created	Checking the option TopSolid keeps sections passing by the guide profile only

Make sections closed:

Open sections will be closed adding a tangent spline.

Extend sections at beginning / at end:

Sections can be extended at each extremity with a giving value.

Curvature: the radius curvature is constant.
Tangency: the segment is tangent with the section.
Exact: the extension follows the probable evolution of the curve based on its last points.

Trimming:

It is possible to trim sections with surfaces at start, at end or both ends. This in order to control the fitting surface.

Advanced options:

Tolerance between faces:

This option allows to work with faces which are not perfectly joined. Distant between edges must not be higher than the given tolerance.

Smooth sections:

In order to have a smooth lofted shape, sections can be smoothed with a points count identical for all profiles. This smoothing is done by default.

TopSolid computes the number of interpolation points automatically but user can modify it here unchecking the option Compute automatically the number of interpolation points.

Discard some sections:

According to faces configuration and guide profiles, sections at both ends could be too short or interfere with the creation of a lofted shape.

It is possible to enter a number of section to remove at start and at end.

Modifications / Additional information:

The element thus created is an operation, its updating is carried out after solving the sketch.

This element is not therefore visible during editing the sketch and cannot be limited by a sketch element nor used as a limitation to the sketch element.

Profiles origin: working with closed profiles, it is important to check the origin position (they must be at the same position on each profile). Otherwise the points correspondence could give us an unexploitable result. To modify profiles origin use the 3D sketch operation Profiles origin and orientation.


Without modification of profiles origin	After correction on profiles origin

Modification of generated sections: it is possible to modify or remove sections to be able to create a shape, adding operations on 3D sketch (Extension, Trimming or Segments removing). These operations work on a profile by memorizing its rank into the set of profiles (modifying the number of sections, added operations could be done on an unexpected profile).

Intersection with 5 points

Extension on the profile in the middle (third profile)

Modification of points count with 7 sections

The extension is still done in the third profile (not in the middle anymore)

Smoothing of modified profiles: it is important to smooth modified profiles with the same number of points than the one used in the Multiple intersection operation.