6.1 Revolve Boss & Revolve Cut

6.1 Revolve Boss & Revolve Cut

Quick Answer: Revolved Boss/Base adds material by spinning a sketch profile around an axis (usually a centerline or model edge). Revolved Cut removes material the same way. Default angle is 360°. Keep the profile entirely on one side of the axis—never crossing it—and use a closed profile for solid revolves or Thin Feature for constant-thickness walls.

On the CSWA skill map, Intermediate Part Creation and Modification explicitly includes revolve techniques alongside circular patterns and multi-step feature stacks. When an exam drawing shows a shaft shoulder, pulley half-section, conical boss, or circular groove cut into a body, you should reach for Insert → Boss/Base → Revolve or Insert → Cut → Revolve rather than trying to fake the shape with many extrudes.

What a revolve actually builds

A revolve sweeps every point of the selected sketch contour around the axis through the revolve angle. A rectangle fully offset from a vertical centerline, revolved 360°, becomes a cylinder (or annular ring if the rectangle does not touch the axis). A triangle revolved about one side becomes a cone. An arc-and-line half-profile revolved about its centerline becomes a pulley or handle silhouette.

Base vs boss: the first solid in a new part is often Revolved Base; later revolves on existing geometry are boss features. On the exam the PropertyManager label may read Boss/Base—functionally you still pick the correct sketch and axis.

Choosing the axis of revolution

SOLIDWORKS accepts several axis definitions for a revolve:

1. Centerline in the revolve sketch (most common exam workflow)
2. Construction line marked as construction in the same sketch
3. Model edge that is linear (for example, a cylinder’s silhouette edge or a rectangular face edge)
4. Temporary axis of a cylindrical face or a reference axis created under Reference Geometry
5. Sketch line that is not the profile contour but lies in the sketch as a separate entity used only as axis

Exam habit: Draw the half-profile of the part on Front (or the plane the drawing implies), add a centerline on the symmetry axis shown on the sheet, fully define the profile relative to that centerline, then select the centerline as the revolve axis in the PropertyManager.

Axis traps that ruin mass

If the drawing shows Ø dimensions to a centerline, that centerline (or an equivalent model edge) is your revolve axis—not a random vertical line near the profile.

Profile rules (closed, open, and “must not cross”)

Closed profile for solid revolve

For a standard solid Revolved Boss/Base or Cut, the contour should be a closed region: lines and arcs meet at endpoints with no gaps. Tiny gaps prevent the feature from recognizing a solid region. Zoom endpoints and apply coincident relations just as you would before an extrude.

Multiple closed contours in one sketch require careful contour selection (same idea as multi-contour extrude). On timed CSWA items, prefer one clean closed half-profile plus centerline unless the drawing clearly shows multiple regions.

Profile must not cross the axis

Hard rule: geometry that will be revolved as a solid must lie on one side of the axis (or touch the axis along an edge that becomes a filled solid to the center). If a line or arc crosses the axis so part of the profile sits on both sides, SOLIDWORKS reports an error about invalid or self-intersecting geometry.

Touching the axis is allowed when the solid should fill to the center (for example, a half-disk profile that includes a radius from the centerline produces a full solid disk/sphere segment). Crossing is not allowed.

Exam scenario: A half-section pulley sketch has an outer rim, a web, and a hub bore. The hub bore is an open rectangular notch above the centerline, not a rectangle that straddles both sides of the axis. Sketch only the upper (or lower) half relative to the axis; revolving 360° creates the full bore.

Open profiles and Thin Feature

An open profile (for example, a single polyline representing a wall centerline or wall outer face) cannot create a solid revolve without Thin Feature. Enable Thin Feature in the Revolve PropertyManager and set:

• Thickness value (match the drawing wall thickness)
• Direction: one direction, mid-plane, or two direction

Thin revolves appear when drawings show a constant-thickness revolved shell—think spun sheet or thin ring—without modeling both inner and outer closed walls as a full solid profile. If the drawing already gives a closed annular cross-section with inner and outer radii, a solid revolve of that closed profile is usually clearer and more exam-stable than thin feature.

Angle, direction, and partial revolves

If the exam sheet shows a full pulley, leave 360°. If it shows a quarter-turn stop or a pie-shaped solid, set the explicit angle. Wrong angle is less common than wrong axis, but it directly scales volume: a 180° revolve of a closed profile has roughly half the volume of a 360° revolve of the same profile (exact mass still depends on material and whether the solid fills to the axis).

Revolved Cut workflow

1. Create the base solid (often Extrude or prior Revolve).
2. Open a sketch on a plane that cuts through the symmetry axis (Front is common).
3. Sketch the cut profile on one side of the axis—groove cross-section, undercut shape, or tapered cut outline.
4. Add or select the axis (centerline or temporary axis of the cylindrical face).
5. Revolved Cut → confirm 360° or partial → verify the cut does not destroy needed structure.
6. Run Mass Properties after the cut; undercuts and grooves are frequent mass reducers on modification steps.

Design intent tip: Dimension the groove to datums that match the drawing (distance from a face, depth, radii). When the exam says “change groove width from 4 mm to 6 mm,” one driving dimension should control that width.

Revolve vs Extrude: when to choose which

Do not revolve a full circular sketch about a diameter when a simple extrude of a circle is enough—extra complexity burns time and risks axis mistakes. Use revolve when the cross-section is the story (variable radii along an axis of symmetry).

Fully defining the revolve sketch

Before accepting the feature:

1. Profile closed (or intentionally open for thin revolve).
2. No blue free endpoints on the contour.
3. Centerline related with colinear or coincident to origin/axes as the drawing requires.
4. Diameters as diameter dimensions where the sheet uses Ø callouts—remember that on a half-profile, a horizontal dimension from axis to outer edge is a radius; double-check whether the drawing lists radius or diameter and dimension accordingly (or dimension diameter across full model edges after feature if clearer).
5. Status: Fully Defined.

Radius vs diameter trap: A half-profile dimension of 25 mm from centerline to outer edge is Ø50 mm on the finished solid. Misreading Ø50 as a 50 mm radial offset doubles the size and destroys mass.

Modification questions involving revolves

Intermediate and advanced CSWA items often:

• Change an outer diameter or shoulder length on a revolved shaft
• Deepen a revolved groove
• Switch material after the revolve stack is complete
• Add fillets (next section) on revolved edges after the solid exists

Workflow under the clock:

1. Build the revolve with dimensions that map 1:1 to the sheet.
2. Name or remember which dimension is which (FeatureManager sketch edit).
3. On the modification step, Edit Sketch or Edit Feature—do not rebuild the whole revolve from scratch unless the change is structural.
4. Rebuild → Mass Properties → enter the value with required decimals.

Checklist before leaving a revolve feature

• Correct plane and half-profile orientation
• Axis selected; preview matches drawing silhouette
• Profile does not cross axis
• Angle 360° unless drawing shows otherwise
• Solid vs thin choice matches wall definition on the sheet
• Fully defined sketch; correct units (often MMGS)
• Mass Properties sanity-check (order of magnitude vs overall size and material)

Revolve mastery is high leverage on intermediate part questions: one correct half-profile and axis can replace dozens of extrude steps and still absorb diameter modifications cleanly when design intent is dimensioned to the centerline.