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Creating Sew Surfaces

Sewing is a Boolean operation combining a surface with a body. This capability adds or removes material by modifying the surface of the solid.You can sew all types of surfaces onto bodies. Depending on your geometry, two kinds of sewing operations can be performed:

  • If the surface has been designed so that its boundary entirely lays on the solid, you can sew it using the surface boundary projection onto the solid. In this case you can use the Simplify Geometry option or not (unchecked option).

Sewing features (in boundary projection mode) is more productive (CPU cost) and more stable (geometric tangency condition) than creating a solid using the Close Surface command (when possible) because no surface/surface intersections are computed.

  • If the surface crosses the solid, you can make the application compute the intersection of the surface with the solid prior to sewing the surface. In this case, you need to use the Intersect body option.

This task shows you both methods.

Open the SewSurface.CATPart document.
  1. The surface boundary is on the solid. Select Join.1 as the surface you wish to sew onto the body.

    5.1

  2. Click Sew Surface 5.2.
    The Sew Surface Definition dialog box is displayed:5.3
    Keep the
    Simplify geometry option active. Using this option, if in the resulting solid there are connected faces defined on the same geometric support (faces separated by smooth edges), these faces will be merged into one single face.

    With topology simplification

    Arrows appear indicating the side where material will be added or kept. Note that clicking an arrow reverses the given direction. The arrows must point towards the solid.

  3. Click OK.
    The surface is sewn onto the body. You may notice that the bottom of the solid is made of one single face. The specification tree indicates you performed the operation.
  4. To see the simplification, just hide Join.1.

    5.4

    Sewn Geometry

    Filleted Edge

    5.5 5.6

    Without topology simplification

    Some operations you perform after sewing using Simplify geometry may make the simplified geometrical result disappear. As shown in the example below, filleting an edge belonging to a sewn surface makes the sewn geometry disappear.

  5. Double-click SewSurface.1 in the specification tree to edit it and deactivate the Simplify geometry option.
  6. Click OK.
    The bottom of the solid is made of three connected faces. The smooth edges resulting from the sewing appear because no topological simplification has been performed.

    5.7

Using the “Intersect body” option

You will use the Intersect body option when the surface straightly crosses the solid without being tangent. The application then needs to compute the intersection between the surface and the solid, the portions of surface with “free edges” being eventually removed.

Note that Intersect body should not be used in case of solids having Through holes or pockets and where it is not possible for surface to add material for sew operation.

5.8
In the following example, the application can compute the intersection:

5.9

Checking Intersect body in the Sew Surface Definition dialog box automatically activates the Simplify geometry option.The arrow indicates the portion of material that will be kept:

5.10

The surface is sewn onto the body. Some material has been removed.

5.11

If you have a Cast and Forged Part Optimizer license, you can also remove faces while sewing surfaces onto bodies.

Hybrid Design

When adding a surface-based feature or a surface feature modifying another surface-based feature or surface belonging to the same body, Part Design features based on that second feature then reference the new added feature. In other words, a replace operation is automatically performed. For an example, refer to Creating Splits.

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