The Rib capability adds strength to a shelled body and is typically applied inside of a shelled body, although it may extend outside the body as well.

This task shows you how to create a rib.

Open the Rib.CATPart document.
  1. Click the Rib icon .
    The Rib dialog box is displayed.

  2. Select Sketch.3 as the closed profile. If no profile is defined, clicking the Sketcher icon enables you to sketch the profile you need.

    If you are not satisfied with the profile you selected, note that you can:

    • click the Profile/Surface field again and select another sketch.

    • use any of these creation contextual commands available from the Profile/Surface field:

    Shape Definition

    The prism is the default shape. Just click the Sweep icon if you want to change. For the purposes of our scenario, keep the default option.

  3. Set the parameters and options as follows to define the shape as explained in Prism (or Sweep) page.

    • In the Distance tab

    First Limit: Length=20mm

    Second Limit: Length=-50mm

    To define limits, instead of using the Length option, you can set the:

    • To shell option. This capability extends the rib to a shellable volume in the active body, in the opposite direction of the height. The extension of the rib profile must fit inside the boundaries of the shellable volume. Otherwise, no extension will occur.

    • To Plane/Surface option. The plane or surface you then select trims the rib.

    Extension Type

  4. To define the extension type you want, you can set one of the three options available from the Extension type drop down list:

    • No extension: confines the rib to be created only within the walls of the shelled volume, even if the profile is outside of the walls of the volume.

    • Across removed face: Like no extension (above) except the rib is not confined within the wall of the deleted face of the shelled volume. Refer to Extend across removed faces option.

    • Add all:  creates the rib based on the specified length and width values, even if the values cause the rib to protrude outside of the volume to which it is applied.

    • Subtract all: subtracts the volume of the rib from the volume to which it is applied.


  5. For the purpose of our scenario, use the No extension option.

    Thin Solid

    To define the Thin Solid, you can set one of the two options available from the Type drop down list:

    • Use body thickness: the rib wall thickness is that of the active shelled body thickness.

    • Enter thickness: simply enter the value you want. After this option is selected, the value field becomes available. Wall thickness values can only by positive values.


    The Neutral fiber option adds the same thickness to both sides of the profile. When you uncheck the Neutral fiber option, Thickness1 and Thickness2 inputs are available. You can give the different thickness to the left/right side of the profile, and one of them can be 0mm.

  1. For the purposes of our scenario, check Neutral fiber option. Set the Enter thickness option and enter 7mm in the Thickness value field.



    Fillet tab adds the ability to have intrinsic fillets as part of the rib feature definition.

  1. Click the Fillet tab. Select First radius and enter 1mm.

  2. When you have the rib like below with the ends of the open profiles, you can add the fillets at the ends of the open profile with Lateral radius option and Fillet profile ends option. The Fillet profile ends can be combined with other radius options. Please see Prism for some examples.

  3. Click OK to confirm and create the rib. Rib.X is added to the specification tree in the Solid Functional Set.X node.


    The Posts tab provides options for creating conical ribs from non-construction point entities contained in the selected profiles sketch. These types of ribs are called "posts".

    Open the Rib_post.CATPart document.

  1. Click the Rib icon . The Rib dialog box is displayed.

  2. Select Post Points or three points in the geometry for Profile/Surface field.

  3. Enter 50mm for First Limit Length.

  4. Click the Posts tab.

  5. Check the Create Posts at points option.
    The application detects the points contained in the selected sketch.

  6. In the Diameter field, enter a value to define the rib post diameter which must be greater than zero. Each non-construction point within the selected profile's sketch is used as the center point for the diameter. For example, enter 13mm.

  7. The Taper Angle applies to each rib post. A non-zero angle results in the post taking the geometric form of a truncated cone. For example, enter 3deg. Select Preview button.

    The Reference field lets you choose between three types of elements used for neutral elements for applying the taper angle. The three elements available are:

    • Profile plane

    • First limit
      The reference will use the First Limit. Up to Surface is used for the First Limit, refer to the picture below for details:

    • Second limit
      The reference will use the Second Limit when you set Second Limit.

    Note that posts are not affected by the data you enter in features draft tabs.

  8. Select First Limit for Reference.

  9. Select Distance tab and select To Plane/Surface for First Limit. Select Up to Surface in the specification tree.

  10. Click OK to confirm and create the three posts.

More About Posts

In addition to points, sketches can contain curves, which enables you to obtain results as illustrated below: