Sew

This command sews together a set of surfaces.

Creation Stages / Use:

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

Select the surface shape or the main surface on which to sew the other surfaces.
Select other surface shapes or surfaces to sew.

The sewing combines 2 separated faces by merging their common edges of these 2 faces.

Available Options:

Hide:

The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Tolerance:

This option defines the sewing tolerance between the faces.

For two surfaces to be able to be sewed together, the edges common to these two surfaces must not be farther apart than the sewing tolerance.

Number of iterations:

Using this option, you can optimize the sewing of a set of faces.

This is how this option functions:

If you validate the function, a first sewing is made as per the tolerance given. However, surfaces that are too far from each other will not be sewn.
The value of the tolerance is thus multiplied by 2 and new sewing of the remaining surfaces occurs with this new tolerance.
The value of the tolerance is then multiplied by 2 again and so on; as many times as the number of iterations.

For example, for a initial tolerance of 0.01mm and a number of iterations of 3, here is what will happen:

first sewing at the 0.01mm tolerance
second sewing has a tolerance of 0.02mm (0.01mm x 2)
third sewing at a tolerance of 0.04mm (0.02mm x 2)

The maximum number of iterations is 10. And the minimum number is 1 (the first sewing).

Separate:

Without this option, when sewing separated batches of surfaces in a single sewing operation, TopSolid generates a single shape made of several bodies. When using this options, the separated batches of surfaces are sewed as independent shapes. In the example bellow, we can get a single shape with four surfaces into two bodies (without "separate" option) or two shapes made of 2 faces each (with the "separate" option)

Sewing of separated surfaces

Sewing result with 2 shapes made of 2 faces

Associative:

This option allows to keep the sewing information as an operation that can be edited from the operation tree. When this option is not activated, the result of the sewing is a non associative part. it is to say that the shape does not have historic of the operations made previously on it and it will not be possible to edit them anymore. The result is the equivalent of an imported shape.

It is not possible to modify the associativity type afterward. If it has been made in non associative mode, it will not be possible to modify the operation made previously on the part. The shape has become a non associative body.

Preserve colors:

This option allows to keep the entity color on tool faces and this, after sewing.

If some faces have been colored with the Coloring command, the color will be kept on these faces during the sew, even if the option is not checked.

The Preserve colors option only takes in account the color attribute of shapes.

Advanced options:

Merge:

This option allows to merge the imprinted surfaces with the sewing.

Sewing with an imprinted surface (the rectangular surface in the middle)

Sewing result

Create boundary edges:

This option allows to create boundary edges. Only surfaces have boundary edges. A solid has not.

Modifications / Additional information:

If the sewing has been made in associative mode, it is possible to edit the operation and add or extract surfaces from the list of surfaces to sew.

At the end of the sewing operation, a message indicates the number of solid, surfaces and holes.

If the message displays "solid=1", the part is a solid shape.
If the message displays a number of surfaces and holes, the sew is not complete. Some missing surfaces have to be created before trying to sew again.