More about Ribs

You can sweep a profile along a center curve to create a rib. This topic provides you with the information you need to create a rib.

The following are discussed:

Related Topics
Creating Ribs
Trimming Ribs or Slots

Rib Definition Dialog Box

This section describes the various options available in the Rib Definition dialog box to create a rib.

Profile Control

You can control the profile's position by choosing one of the following options:


  • Keep angle: Keeps the angle value between the sketch plane used for the profile and the tangent of the center curve.
  • Pulling direction: Sweeps the profile with respect to a specified direction. To define this direction, you can select a plane or an edge. For example, you need to use this option if your center curve is a helix. In this case, you will select the helix axis as the pulling direction.
  • Reference surface: The angle value between axis h and the reference surface is constant.
  • Contextual commands creating the directions you need are available from the Selection box:
    • Create Line: For more information, see Generative Shape Design User's Guide: Creating Wireframe Geometry: Creating Lines..
    • Create Plane: see Generative Shape Design User's Guide: Creating Wireframe Geometry: Creating Planes..
    • X Axis: the X axis of the current coordinate system origin (0,0,0) becomes the direction.
    • Y Axis: the Y axis of the current coordinate system origin (0,0,0) becomes the direction.
    • Z Axis: the Z axis of the current coordinate system origin (0,0,0) becomes the direction.
    • Create Join: Joins surfaces or curves. See Generative Shape Design User's Guide: Performing Operations on Shape Geometry: Joining Surfaces or Curves.
    • Create Extrapol: Extrapolates surface boundaries or curves. See Generative Shape Design User's Guide: Performing Operations on Shape Geometry: Extrapolating Surfaces and Extrapolating Curves.

    If you create any of these elements, the application then displays the corresponding icon in front of the Selection box. Clicking this icon enables you to edit the element.

  • If you have chosen to work in a hybrid design environment, the elements created on the fly via the contextual commands mentioned above are aggregated into sketch-based features.
  • Move profile to path: easily associates profiles with center curves but also allows a single sketch to be swept along multiple center curves. This option can be accessed if Pulling direction of Reference surface is already on, and builds the profile with the following understanding:
    • The origin of the sketch plane (i.e. 0,0) will be swept along the path.
    • The vertical axis of the sketch plane (i.e. 0,1) will be kept parallel to either the pulling direction (if the profile control is set to Pulling direction) or the normal to the Reference surface (if profile control is set to Reference surface). In this example, the profile to be swept is a square (shown by the arrow). The circles which belong to the same sketch are used as center curves and plane yz is set as the pulling direction.



      Once the geometry is selected and Move profile to path on:

      • the moved profile turns blue,
      • a blue arrow is displayed at the origin of the transformed profile. Clicking on this arrow reverses the profile direction and rotates it 180 degrees about the pulling direction.
      • an orange arrow is parallel to the pulling direction. Clicking on this arrow reverses the profile direction and rotates it 180 degrees about the blue arrow.



      The resulting rib looks like this:



      Merge rib's ends:

      The Merge rib's ends option is to be used in specific cases. It creates materials between the ends of the rib and existing material provided that existing material trims both ends. For an example, see Trimming Ribs or Slots.

      Merge Ends:

      Merge Ends trims the rib to exiting material. For more information, see Trimming Ribs or Slots.

Defining Ribs

This section describes the combination of the different elements to create a rib.

To define a rib, you need a center curve, a planar profile and possibly a reference element or a pulling direction . You can combine the different elements as follows:

  Closed Profile Open Profile
Open Center Curve



(existing material)

(Thick Profile option, no existing material)


(Thick Profile option, existing material)
Closed Planar Center Curve



(Thick Profile option, no existing material)
Closed 3D Center Curve



(Thick Profile option)

About Profiles

This section provides information on the profiles used to create a rib.


  • In some cases, you can define whether you need the whole sketch, or sub-elements only. For more information, see Using the Sub-Elements of a Sketch.
  • Clicking the icon opens the Sketcher . You can then edit the profile. Once you have done your modifications, you just need to quit the Sketcher. The Rib Definition dialog box then reappears to let you finish your design.
  • If you launch the Rib command with no profile previously defined, just click the icon to access the Sketcher and then sketch the profile you need.
  • You can also create your profile by using any of these creation contextual commands available from the Profile box:
    • Create Sketch: launches the Sketcher after selecting any plane, and lets you sketch the profile you need as explained in the Sketcher User's Guide.
    • Create Join: joins surfaces or curves. See Generative Shape Design User's Guide: Performing Operations on Shape Geometry: Joining Surfaces or Curves.
    • Create Extract: generates separate elements from non-connex sub-elements. See Generative Shape Design User's Guide: Performing Operations on Shape Geometry: Extracting Geometry: Extracting Elements.

    If you create any of these elements, the application then displays the corresponding icon in front of the box. Clicking this icon enables you to edit the element.

    If you have chosen to work in a hybrid design environment, the elements created on the fly via the contextual commands mentioned above are aggregated into sketch-based features.


  • You can use an open profile provided existing material can trim the rib. For more information, see Trimming Ribs or Slots.
  • Ribs can also be created from sketches including several profiles. These profiles must be closed and must not intersect. For example, you can easily obtain a pipe by using a sketch composed of two concentric circles:
    Profile


    Result


Center Curves

This section describes the rules for creating a rib.

Before using center curves, the following rules should be kept in mind:


  • 3D center curves must be continuous in tangency
  • If the center curve is planar, it can be discontinuous in tangency.
  • center curves must not be composed of several geometric elements

Clicking the icon opens the Sketcher to let you edit the center curve. Once you have done your modifications, you just need to quit the Sketcher. The Rib Definition dialog box then reappears to let you finish your design.

Recommendation

This section provides the recommendations for creating a rib.

It is recommended that the profile be on the center curve in a plane normal to the center curve. Otherwise, it very often leads to an unpredictable rib shape.

The position of the profile in relation to the center curve determines the shape of the resulting rib. When sweeping the profile, the application keeps the initial position of the profile in relation to the nearest point of the center curve. The application computes the rib from the position of the profile.

In both examples below, the application computes the intersection point between the plane of the profile and the center curve, then sweeps the profile from this position.



In this particular example, the profile is not located on the center curve. Is this context, the shape obtained is unpredictable.

Keep in mind that when the profile is not on the center curve, even if you use any of the Profile control options (Keep angle, Pulling direction, Reference surface) , you cannot predict the final rib shape. The use of the Profile Control options never helps in anticipating the final rib shape. Consequently, it is preferable not to use such profile types.