Rib

This task shows you how to create a rib, that is how to sweep a profile along a center curve to create material.

To define a rib, you need a center curve, a planar profile and possibly a reference element or a pulling direction. 

To create ribs you can combine the different elements as follows:
Open profile Closed profile Pulling direction
Open center curve

Closed planar center curve  
Closed 3D center curve    

Moreover, 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.

Open the Rib1.CATPart document.
1.  Click the Rib icon .

The Rib Definition dialog box is displayed.
 

2. 

Select the profile you wish to sweep, i.e. Sketch.2 . Your profile has been designed in a plane normal to the plane used to define the center curve. It is a closed profile.
 

About Profiles

In some cases, you can define whether you need the whole sketch, or sub-elements only. For more information, refer to 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 use an open profile provided existing material can trim the rib.
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:

Profiles

Result
3. Select the center curve,  i.e. Sketch.1.

The center curve is open. To create a rib you can use open profiles and closed center curves too. 3D Center curves must not be discontinuous in tangency.
  You can also use planar wireframe geometry as your profile or center curve.
  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. 
The application now previews the rib to be created.

You can control its 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.
4.  To go on with our scenario, let's maintain the Keep angle option. Remember, the angle value is 90 degrees.
5.  Click OK.

The rib is created. The specification tree mentions this creation.
The Merge ends option is to be used in specific cases. It create materials between the ends of the rib and existing material provided that existing material trims both ends.
6.  Delete this rib to create another one by using the Pulling direction option. After setting this option, select plane xy to define z axis as the pulling direction. The plane used to define the profile will remain normal to plane xy.

 The preview looks like this:

And the rib like this:

7. Delete this rib to create another rib by using the Reference surface option. 

First, display the loft in the Show space, then set the Reference surface option and select the loft as the reference surface. The angle value between h axis and the surface equals 0. It remains constant.

The preview looks like this:

And the rib like this:

8. Check the Thick Profile option to add thickness to both sides of Sketch.2. New options are then available:
  9. Enter 2mm as Thickness1's value, and 5mm as Thickness2's value, then preview the result.

Material is added to each side of the profile.
 

Checking the "Merge Ends" option trims the rib to exiting material.
  10. To add material equally to both sides of the profile, check "Neutral fiber" and preview the result.

The thickness you defined for Thickness1 (2mm) is now evenly distributed: a thickness of 1mm has been added to each side of the profile.
  11.

Click OK to create the rib.

The rib looks like this:
 

A Few Words about the Keep Angle Option

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

 
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