6.2 Sweep Boss/Base & Sweep Cut

6.2 Sweep Boss/Base & Sweep Cut

Quick Answer: A sweep moves a profile along a path to create (or cut) material. A solid sweep needs a closed profile in one sketch and a path in a different sketch, joined by a Pierce relation. SOLIDWORKS lists sweeps among CSWA's hands-on skills, so expect them on advanced-part items where an extrude or revolve simply cannot make the shape.

Section 6.1 covered Revolve, which spins a profile about an axis. Sweep is the next step in the same family: instead of spinning the profile through a fixed angle, you drive it along an arbitrary curve. The official SOLIDWORKS Design Associate page groups all four together—"boss and cut features: extrudes, revolves, sweeps, lofts"—which means an exam item can legitimately require one.

When a sweep is the right tool

Reach for sweep when the cross-section stays essentially constant but the centerline is not straight:

Typical CSWA-shaped geometry: a bracket with a Ø8 mm tube arm that bends 90° before meeting a flange; a gasket that follows a rounded rectangular face; an O-ring groove running around a non-circular boss; a rib following a curved edge.

The two-sketch rule

This is the single most common beginner error. For a sketch-driven sweep:

1. Sketch 1 = the path. Draw it on whatever plane matches the drawing (or as a 3D sketch). Fully define it.
2. Sketch 2 = the profile. Draw it on a different plane, ideally one that is normal to the path at the path's start point.
3. The profile and path must be in separate sketches. SOLIDWORKS will not let you select two contours from the same sketch as profile and path.

Getting the profile plane right

If the path starts on the Front plane and runs into the model, sketch the profile on the Front plane too. If the path starts somewhere awkward, build a reference plane first (Chapter 11):

• Insert → Reference Geometry → Plane
• First reference: the path's start point
• Second reference: the path curve itself, set to Normal to Curve (SOLIDWORKS calls this Perpendicular to the curve)

That gives a plane square to the path start, which is exactly where a swept section belongs.

Pierce: the relation that makes sweeps work

A profile that merely sits near the path will sweep with an offset, and every downstream measurement drifts. Lock it with Pierce:

1. Open the profile sketch.
2. Ctrl-select the profile's center point (or a construction-line midpoint) and the path curve.
3. Choose Pierce in the Add Relations panel.

Pierce places the selected sketch point exactly where the path punches through the sketch plane. The sketch turns black (fully defined) and the swept solid now starts precisely on the path. Guide curves, if the drawing calls for a section that grows along the way, also require Pierce relations to the profile.

Trap: Coincident is not a substitute for Pierce. Coincident to the curve's endpoint works only when the path start happens to lie in the sketch plane; Pierce works in the general 3D case.

Sweep PropertyManager settings that change your mass

Circular Profile is your speed tool

If the drawing says "Ø10 mm rod following the path shown," you do not need a profile sketch:

1. Insert → Boss/Base → Sweep
2. Under Profile and Path, click the Circular Profile button
3. Select the path, type the diameter, click OK

That is roughly a 15-second feature versus a minute of plane-building and piercing. On a 15-point advanced-part item where the sweep is one of six features, that time is real.

Sweep Cut

Insert → Cut → Sweep uses the identical profile-plus-path recipe but removes material. Exam-relevant uses:

• An O-ring groove or retaining-ring groove that follows a curved or racetrack outline
• A machined slot that follows a bent path across a face
• A relief channel around a raised boss

Because sweep cuts remove volume, they move both mass and center of mass. A groove that is 0.5 mm too deep or too wide is the same category of all-or-nothing error covered in 1.2.

Why sweeps fail, and how to fix each one

The radius-of-curvature rule

Here is the mental check that prevents most sweep failures: the profile's half-width must be smaller than the smallest concave radius anywhere on the path. Sweep a 10 mm-wide square section around a 3 mm path fillet and the inside corners of the section collide with themselves—SOLIDWORKS cannot build a valid solid. Either the drawing gives you a larger path radius than you sketched, or you misread the section size. Re-read the drawing before you start deleting features.

Mass properties on swept geometry

A straight extrude of area A and length L has volume A × L. A sweep on a curved path does not. Material on the inside of a bend is compressed and material on the outside is stretched, so area × path length is only an approximation—and it drifts further the tighter the bend.

Practical rule for the exam: never hand-calculate swept volume. Build the feature, apply the specified material (Chapter 10), and read Mass Properties. Use area × path length only as a sanity band—if Mass Properties reports a number wildly outside that band, you probably swept the wrong profile or picked the wrong path segment.

Worked exam-style scenario

Drawing: base plate 80 × 50 × 10 mm on the Top plane. From the plate's top face, a Ø12 mm solid arm follows a path that runs 40 mm vertically, fillets R15, then runs 35 mm horizontally. Material 6061 Alloy. Report mass in grams.

Build order:

1. Set Document Properties → Units → MMGS first (Chapter 2).
2. Sketch the plate outline on Top; Extruded Boss/Base, Blind 10 mm.
3. Sketch the path on the Front plane: vertical 40 mm line, sketch fillet R15, horizontal 35 mm line. Fully define it and anchor its start to the plate's top face.
4. Insert → Boss/Base → Sweep → Circular Profile → select the path → diameter 12 → OK.
5. Check the radius rule: profile half-width 6 mm < R15 path fillet. Safe.
6. Apply 6061 Alloy, then Evaluate → Mass Properties, read mass in grams to two decimals.

The R15 number is not decoration—it is the drawing telling you the sweep will build. If you had sketched an R4 corner from memory, the sweep would fail and you would burn minutes debugging a self-inflicted error.

Section checklist

1. Path in one sketch, profile in another, both fully defined.
2. Profile plane normal to the path start when the path leaves the sketch plane.
3. Pierce relation between a profile point and the path.
4. Profile half-width < smallest concave path radius.
5. Prefer Circular Profile whenever the drawing gives a plain diameter.
6. Apply material, then read Mass Properties—never estimate swept volume by hand.