Boss and Cut Features: Extrude, Revolve, and Fillet

Boss and Cut Features: Extrude, Revolve, and Fillet

Why Parametric Solid Modeling Matters

In manufacturing and marine drafting, parts must be communicated with absolute precision. A shaft collar that is 0.5 mm too short or a bracket with bolt holes in the wrong location can shut down a production line or compromise a vessel's structural integrity. SolidWorks builds parts parametrically: every dimension you enter is stored and can be changed later, and the model updates automatically. This lesson covers the four features you will use most often in the CSWA exam and on the job: Extruded Boss/Base, Extruded Cut, Revolved Boss, and Fillet.

Workspace Safety

Before you sit at a CAD workstation, confirm the following:

• Adjust the monitor height so the top of the screen is at or just below eye level to prevent neck strain.
• Keep cables and bags clear of walkways to avoid trip hazards.
• If you work near a shop floor where machined parts are being handled, wear safety glasses rated to ANSI Z87.1 whenever you leave the CAD area.
• Save your work frequently (Ctrl+S) and use the SolidWorks auto-recover setting. Losing an hour of modeling is a real workflow hazard.

Extruded Boss/Base

An Extruded Boss/Base takes a closed 2D sketch and adds material by pushing it a specified distance along an axis perpendicular to the sketch plane. It creates the first solid body — called the Base feature — or adds more material to an existing body (a Boss).

Key inputs:

• Depth (D1): the linear distance the sketch is extruded. Enter this in the same units as your document template (millimeters for metric, inches for US customary).
• Direction: by default the extrusion goes in one direction; choose Blind, Through All, Up to Surface, or Mid-Plane.
• Draft Angle: tilts the walls of the extrusion inward or outward, useful for cast marine housings or injection-molded brackets.

Workflow: Sketch on a plane → close all contours → exit sketch → Features tab → Extruded Boss/Base → set depth → OK (green check).

Extruded Cut

An Extruded Cut removes material using the same extrusion logic but in the opposite sense. Use it for holes, slots, pockets, and keyways. The sketch must lie on a face of the existing solid or on a reference plane offset from it.

For bolt holes, sketch a circle of the correct diameter on the bracket face. For a keyway slot, sketch a rectangle centered on the shaft axis. End conditions matter: choose Through All when the cut must pass completely through the part regardless of thickness variations; choose Blind when depth must be controlled exactly (e.g., a keyway that must not break through the opposite wall).

Revolved Boss

A Revolved Boss rotates a 2D profile around a centerline to create an axisymmetric solid. This is the correct tool for any part with a circular cross-section: shafts, shaft collars, flanges, and marine pipe fittings.

Key inputs:

• Axis of Revolution: draw a construction line (or use a model edge) as the centerline. The profile must be entirely on one side of the axis.
• Angle: a full revolution is 360°. A partial revolution (e.g., 270°) creates a swept sector shape.
• Thin Feature: check this if you want to revolve an open profile and give it a wall thickness, useful for thin-walled tubes.

Workflow: Sketch profile and centerline on the same plane → exit sketch → Features → Revolved Boss/Base → confirm axis and angle → OK.

Fillet

A Fillet rounds a sharp edge by adding a curved blend of constant or variable radius. Fillets serve two engineering purposes: they reduce stress concentration at inside corners (critical for dynamically loaded marine parts) and they remove sharp burrs that could injure assembly workers.

• Constant Radius Fillet: one radius value applied to all selected edges simultaneously. Most common in basic modeling.
• Variable Radius Fillet: different radius values at each vertex of the selected edge, useful for complex hull forms.
• Full Round Fillet: replaces a face with a tangent arc between two adjacent faces.

Select the edges you want to round, then enter the radius. Apply fillets after cuts are complete so that the fillet geometry does not interfere with cut sketches. This is a common CSWA exam trap.

Chamfer vs. Fillet: A chamfer cuts a flat bevel at a specified angle and distance; a fillet creates a curved radius. Chamfers are common on bolt-hole entries and the ends of shafts. SolidWorks places Chamfer on the same Features menu as Fillet.

Reading the Feature Manager Design Tree

The Feature Manager tree on the left side of the screen lists every feature in creation order. You can right-click any feature to edit its sketch or definition. If your Mass Properties result does not match the answer key, roll back the model (drag the rollback bar above the suspect feature) and inspect dimensions one at a time. This systematic audit is faster than guessing.

Mass Properties Check

Go to Tools → Mass Properties (or the Evaluate tab). SolidWorks reports:

• Volume (in³ or mm³)
• Surface Area
• Center of Mass (X, Y, Z coordinates)
• Mass (requires a material to be assigned)

Assign material before checking: right-click Material at the top of the Feature Manager tree and choose from the SolidWorks material library (e.g., AISI 1020 Steel for a shaft collar). A ±1% tolerance on volume means your dimensions must be very close to correct; even a 0.5 mm error in a critical depth can push volume outside tolerance on a small part.

Connecting to the CSWA Exam

The CSWA Part Modeling section asks you to build a part from a dimensioned drawing and report a mass property value. Examiners change one or two dimensions and ask for the new mass. Practice the full workflow — sketch, feature, material, Mass Properties — until it takes less than 10 minutes per part.