SOLIDWORKS’ Rib Feature’s Unique Options

Article by John Landis updated May 30, 2023


SOLIDWORKS’ Rib feature provides a powerful way to quickly create thin extruded features with a minimum of effort. Ribs are often overlooked when part modeling as most users use the traditional Extrude feature to create these types of structures. Let’s explore the utility and benefits of leveraging the SOLIDWORKS Rib feature.

I like to think of the Rib feature as a special case of an Extrude-Thin Boss.

What makes the Rib feature so special?

It will only create Thin structures. You must specify a thickness parameter that is then applied to the referenced sketch entities. The thickness is centered on the sketch entities, or it can be biased in one or the other direction.

Rib 3

It has only one End condition, Up To Next. This is implied with the Rib feature, and there are no selectable termination options.  You simply specify the direction the feature is generated. SOLIDWORKS does a hemispherical scan in that direction and automatically finds all the Next faces the extrusion will encounter, through 180°. The solid feature develops in all directions and terminates when it “hits” these faces.

The feature must be wholly, totally, and completely terminated by the Next faces. This is the same cardinal rule obeyed by all features using Up To Next termination logic; if any portion of the solid feature generated does not “hit” a Next face if it can see infinity, then the feature cannot be created.

rebuild errors in solidworks rib feature

It is okay to use sketches that are not fully defined. This can be a huge benefit. Although using fully defined sketches in SOLIDWORKS is a fundamental best practice, the Rib feature allows an exception. Because the Rib feature scans through 180° you only need to supply a sufficient amount of Design Intent (dimensions & relations) in your sketch. This can speed up the sketching process significantly. You can rely on the feature being extended Up to Next.

SOLIDWORKS rib feature

The feature can be generated parallel to the sketch plane. This is a real mind blower! Typically, extrusions are created perpendicular (normal) to the sketch plane or in a specified direction, and the thickness is applied in-plane. As a result, the beginning of the feature must be a single planar face. However, the rib feature offers an option that allows the thickness to be applied out-of-plane and the volumetric solid is extruded parallel to the sketch plane. This can generate a feature start that is not limited to a single planar face.

sketch rib feature

Again, to quickly and easily create thin bosses the rib feature can’t be beat. How do you use the SOLIDWORKS Rib feature?

SOLIDWORKS rib feature model

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John Landis

John Landis started with TriMech in 2006, bringing nearly 20 years of real-world engineering, design and manufacturing exposure. He has experience with chemical processing equipment, industrial kilns and design for close tolerance high precision machining. In addition to his expertise in SOLIDWORKS, he also is a 3D Printing Field Engineer.