Create a rib

Learn how to use the Rib command to create a thin feature from an open sketch profile, in a direction parallel to the sketch plane, extruded to the nearest faces on a solid body in Fusion.

1. On the toolbar, click Solid > Create > Rib .

   The Rib dialog displays.

2. In the canvas, select an open sketch profile to use as the Profile.

3. In the dialog, select a Thickness Direction:

   • Symmetric: Extrudes half the thickness value to each side of the sketch profile.
   • One Side: Extrudes the full thickness value to one side of the sketch profile.

4. Select a Start option:

   • From Top: Measures thickness starting from the top.
   • From Bottom: Measures thickness starting from the bottom.

5. Specify the Thickness value to extrude the rib, perpendicular to the sketch plane:

   • In the canvas, drag the distance manipulator handle.
   • Or specify an exact value.

6. Select an Extent Type, then adjust its associated settings:

   • To Next: Extrudes the rib from the sketch profile to the nearest faces on a solid body.
   • Distance: Extrudes the rib from the sketch profile to a specified depth.
     • Depth: Specify the distance to extrude the rib, parallel to the sketch plane, toward the nearest faces on a solid body.

7. Optional: Apply draft and fillets to the rib feature:

   Fusion Design Extension

   This feature is part of an extension. Extensions are a flexible way to access additional capabilities in Fusion. Learn more.

   • Specify a Draft Angle value.
   • Select a plane or face to define the Draft Pull Direction.
   • Click Flip Pull Direction to flip the pull direction of the draft.
   • Specify a Fillet Radius value to apply fillets to the base of the rib feature.

8. Click OK.

The rib feature is extruded in a direction parallel to the sketch plane, and displays on the solid body in the canvas.

Tips

• Click the Flip icon to flip the direction in which the rib is extruded.