How to Use Rib in CATIA

This guide shows how to use rib in CATIA V5 with the Stiffener feature in the Part Design workbench. You sketch a profile, fully constrain it, and turn it into a stiffener between two plates. You then repeat the process on a cylinder-and-base part, using Multi-Pad and projected edges to build the reference geometry.

Stiffener types

CATIA stiffeners come in two types:

• Type 1: Both faces are flat.
• Type 2: One face is flat and one face is rounded.

You can use either type in Part Design.

Prerequisites

• CATIA V5 with access to the Part Design workbench.
• A part with two plates to connect, or a base profile that you sketch yourself in the first steps.

Part 1: Create a stiffener between two plates

Step 1. Open the Part Design workbench

From the CATIA V5 main menu, choose Start > Mechanical Design > Part Design.

Step 2. Begin sketching the base profile

Start a new sketch in the Part Design workbench. The sketcher opens and shows the Profile, Operation, and Constraint toolbars. As you draw a vertical line, the endpoint coordinates appear (for example, V: -1.515mm, L: 86.216mm, A: 268.884deg).

Step 3. Continue the profile without full constraints

Keep sketching the profile by adding horizontal and vertical lines. At this stage the sketch is not fully constrained, so the lines appear green but not every constraint is applied. The endpoint coordinates for the current line might read V: -16.12mm, L: 69.027mm, A: 90deg.

Step 4. Set the pad dimensions

Exit the sketch and create the pad that forms the plates. In the Pad Definition dialog:

• Set the First Limit type to Dimension.
• Enter the required length (for example, 20mm or 30mm).
• Select the sketch for the pad profile (for example, Sketch1).
• Use the Mirrored extent option if your design requires symmetry about a plane.
• Click OK to create the pad.

Step 5. Select the middle plane for the stiffener sketch

In the tree, select the middle plane where the stiffener will be sketched (for example, the zx plane). Then click the Sketch icon to enter the Sketcher workbench.

Step 6. Draw the stiffener sketch

In the Sketcher, use the Profile toolbar to draw a line that connects the two plates where the stiffener will sit. The endpoint coordinates are displayed for precision (for example, End Point H: 109.625mm, V: 16.755mm, A: 220.372deg).

Step 7. Fully constrain the sketch

Apply geometric and dimensional constraints with the Constraint toolbar. Add coincidence, length, and angle constraints as needed. For example, right-click or use the context menu to set a Coincidence constraint between the line and the plate edges.

You must fully constrain the sketch. Otherwise, the stiffener feature may not work correctly.

Step 8. Check that the sketch is fully constrained

Confirm that all lines in the sketch turn green. This indicates that the sketch is locked in position and dimension.

Step 9. Exit the Sketcher workbench

Click the Exit workbench icon to return to the Part Design workbench. The stiffener sketch is now visible on the model.

Step 10. Create the stiffener feature to use a rib in CATIA

Select the stiffener sketch, then click the Stiffener icon in the Sketch-Based Features toolbar. In the Stiffener Definition dialog:

• Set Mode to From Side.
• Enter Thickness1 as 5mm, or your required value.
• Check or uncheck Neutral Fiber, depending on whether you want the thickness centered on the sketch or offset to one side.
• Use Reverse direction if the stiffener appears on the wrong side.
• Click Preview to visualize the stiffener.

Step 11. Adjust the direction and confirm

If the stiffener appears on only one side, click Reverse direction to switch sides. When the placement is correct, click OK to finalize the feature.

Part 2: Build a stiffener on a cylinder and base with Multi-Pad and projected edges

Step 12. Remove an unwanted sketch element

Select the top plane (for example, the xy plane) in the specification tree or on the model. Click the Sketch icon to enter the Sketcher workbench. Select the geometry you want to remove, such as the center circle, and delete it.

Step 13. Sketch on the center plane

Make sure you are sketching on the center plane (for example, the zx plane) for proper alignment and reference. Draw or modify the geometry you need, such as a circle at the center of the rectangle.

Step 14. Apply the Multi-Pad feature

Exit the Sketcher workbench to return to Part Design. Select the sketch that contains multiple domains (for example, a rectangle and a circle), then click the Multi-Pad icon in the Sketch-Based Features toolbar. In the Multi-Pad Definition dialog:

• Set the First Limit type to Dimension.
• Enter Length = 60mm for one domain and Length = 10mm for the other.
• Assign each thickness value to the appropriate domain (the rectangle or the circle).
• Click OK to create the feature.

Step 15. Select the middle plane for the next sketch

In the specification tree, select the middle plane (for example, the zx plane). Click the Sketch icon to create a sketch on this plane. The model displays the new multi-pad feature.

Step 16. Project 3D silhouette edges

In the Sketcher workbench on the selected plane, use the Project 3D Silhouette Edges tool from the Operation toolbar. It projects the edges of the 3D geometry onto the sketch plane, where they serve as references for further sketching.

Step 17. Draw reference lines from the projected edges

Click the projected edge or point where you want the reference line to start. Draw a line to the location you need (for example, from the top of the cylinder to the front). Adjust the line to match your design intent.

Step 18. Complete the reference geometry

Continue clicking points and moving them as needed. Position the lines according to your design requirements.

Step 19. Fully constrain the sketch

Select the relevant point and line in your sketch and apply the necessary constraints. Confirm that the sketch is fully constrained. All geometry turns green, or the constraint status indicates full constraint.

Step 20. Convert the shell out edges to construction geometry

Select both shell out edges in your sketch. Change their status to construction geometry with the construction tool in the toolbar. These edges are then used only for reference and do not create solid features.

Step 21. Exit the Sketcher and open the stiffener tool

Click Exit Workbench to leave the Sketcher and return to Part Design. Then select the Stiffener tool from the Sketch-Based Features toolbar. The Stiffener Definition dialog appears.

Step 22. Set the thickness to use a rib in CATIA on the cylinder and base

In the Stiffener Definition dialog, set the following parameters:

• Mode: Select From Side.
• Thickness1: Enter the thickness you want (for example, 1mm initially).
• Thickness2: Leave it at 0mm unless you need a second thickness.
• Neutral Fiber: Check or uncheck it as your design requires.
• Profile: Make sure the correct sketch (for example, Sketch.2) is selected.

Click Preview to visualize the stiffener. When you are satisfied with the thickness and placement, click OK. The stiffener now appears as a solid feature connecting the cylinder and the base.

Step 23. Review the final model

Rotate and inspect the model to make sure the stiffener is correctly placed and fully integrated with the cylinder and base. Save your work to preserve the completed part.

Summary

To use a rib in CATIA V5 successfully, follow these practices:

• Fully constrain your sketches before using them to create features.
• Use Neutral Fiber and Reverse direction to control stiffener placement.
• Preview the stiffener before you confirm it.
• Sketch on the correct reference plane to maintain alignment.
• Use Multi-Pad to extrude multiple domains with different thicknesses in one operation.
• Project 3D edges into your sketch for accurate references.
• Use construction geometry for reference edges that should not create solid features.

What's next

Try both stiffener types (flat-flat and flat-rounded) on your own parts. Adjust the stiffener thickness to suit your design requirements.