Sweep Features in Parametric 3D CAD

Overview

A Sweep is a fundamental feature in 3D CAD modelling that creates complex geometry by moving a 2D cross-sectional shape (profile) along a defined trajectory (path). Sweeps are essential for creating pipes, wires, springs, custom mouldings, threads, and advanced surface geometry where basic extrusions or revolves are insufficient.

Key Concepts

• Sweep – generates a 3D feature by driving a 2D profile along a path
• Profile – the closed 2D cross-sectional shape being swept
• Path – the trajectory the profile follows (can be 2D, 3D, or an existing edge)
• Guide Curve – an additional sketch that controls how the profile scales or deforms during the sweep
• Pierce Relation – a sketch constraint that forces a profile point to intersect a curve passing through the sketch plane
• Swept Cut – a sweep operation used to remove material instead of adding it

The Basic Sweep

• A basic sweep requires two separate sketches: a Profile and a Path
• Profile: A closed 2D sketch defining the cross-sectional shape (e.g., circle for a pipe, rectangle for a rail)
• Path: An open or closed sketch (2D or 3D) defining the trajectory the profile will follow

Rules for Basic Sweeps

• The profile and path sketches must intersect
• The profile must be a closed contour for solid sweeps
• The profile cannot intersect itself as it travels along the path

Basic Sweep Process

1. Create the Path sketch
2. Create the Profile sketch on a plane that intersects the path
3. Select the Swept Boss/Base feature
4. Select the Profile sketch
5. Select the Path sketch
6. Complete the feature

Path Options

• Paths are not limited to a single sketch; multiple types of geometric entities can serve as sweep paths

Valid Path Selections

Selection Manager

• When a path consists of multiple segments (e.g., a chain of edges or parts of a larger sketch), the Selection Manager is used to choose specific segments
• Options include selecting a full loop, an open loop, or individual segments rather than the entire sketch or body

Guide Curves

• A basic sweep keeps the profile size constant; Guide Curves alter the profile's size and shape as it travels along the path
• Guide curves are additional sketches or model edges that the profile must stay in contact with during the sweep
• As the distance between the path and the guide curve changes, the profile scales or deforms to maintain contact

Rules for Guide Curves

• The guide curve must be a separate sketch from the path and profile
• The profile sketch must intersect the guide curve (add a Pierce or Coincident relation between a point on the profile and the guide curve)
• The profile cannot intersect itself as it scales

Multiple Guide Curves

• More than one guide curve can be used for extreme control over the profile's shape throughout the sweep
• Common in complex surfacing or consumer product design (e.g., aerodynamic shapes, ergonomic handles)
• The profile must be properly constrained to each guide curve
• This may require splitting geometric shapes (e.g., an ellipse) into segments to create distinct points that can be pierced to each guide curve

Profile Orientation

• On curved 3D paths, the profile's orientation must be controlled to prevent twisted or self-intersecting geometry

Orientation/Twist Types

Twist

• A deliberate rotation can be applied to the profile as it travels along a path
• Useful for drill bits, twisted wire, decorative elements, and similar geometry

How to Apply Twist

1. In the sweep options, change the orientation/twist type to Twist Along Path
2. Define the twist using one of the following methods:

Cutting with Sweeps (Swept Cut)

• The sweep mechanism can remove material as well as add it
• Uses the Swept Cut feature instead of Swept Boss/Base
• Still requires a closed profile and a path

Common Swept Cut Applications

• Cutting custom threading on a cylinder (using a helix as the path)
• Creating complex grooves or channels
• Simulating machining toolpaths into a solid body

Thread Creation (Swept Cut Application)

• Threading is a specialised application combining a helix path with a swept cut

Thread Creation Process

1. Create the base cylinder – the foundational geometry
2. Create a helix path:
   • Select the flat circular face of the cylinder
   • Start a sketch and use Convert Entities to capture the circular edge
   • Use the Helix/Spiral tool under Curves
   • Define the helix using Pitch (distance between threads) and Revolutions (number of thread turns)
3. Create the cutting profile:
   • Create a reference plane perpendicular to the end of the helix path
   • Sketch the thread profile (typically a V-shape or trapezoid) on this plane
   • Apply a Pierce relation between the profile and the helix end
4. Perform the swept cut:
   • Use the Swept Cut tool, selecting the profile and helix path
5. Clean up:
   • Chamfer or revolve-cut the start and end of threads to remove sharp, incomplete geometry

Comparison Tables

Sweep Types Comparison

Profile Orientation Comparison

Diagrams

Basic Sweep Process

flowchart TD
    A[Create Path Sketch] --> B[Create Profile Sketch on Intersecting Plane]
    B --> C[Select Swept Boss/Base Feature]
    C --> D[Select Profile]
    D --> E[Select Path]
    E --> F[Complete Sweep Feature]

Guide Curve Workflow

flowchart TD
    A[Create Path Sketch] --> B[Create Profile Sketch]
    B --> C[Create Guide Curve Sketch]
    C --> D[Add Pierce/Coincident Relation Between Profile and Guide Curve]
    D --> E[Select Sweep Feature]
    E --> F[Assign Profile, Path, and Guide Curve]
    F --> G[Profile Scales/Deforms Along Path Based on Guide Curve]

Thread Creation Process

flowchart TD
    A[Create Base Cylinder] --> B[Select Circular Face]
    B --> C[Create Helix Path: Define Pitch and Revolutions]
    C --> D[Create Reference Plane at Helix End]
    D --> E[Sketch Thread Profile on Reference Plane]
    E --> F[Pierce Profile to Helix End]
    F --> G[Perform Swept Cut]
    G --> H[Clean Up: Chamfer Start/End of Threads]

Sweep Feature Decision Map

flowchart TD
    A[Need to Create Complex Geometry?] -->|Yes| B{Adding or Removing Material?}
    B -->|Adding| C[Swept Boss/Base]
    B -->|Removing| D[Swept Cut]
    C --> E{Need Profile Shape Control?}
    D --> E
    E -->|Constant Shape| F[Basic Sweep: Profile + Path Only]
    E -->|Variable Shape| G[Add Guide Curves]
    G --> H{How Many Control Curves?}
    H -->|One| I[Single Guide Curve]
    H -->|Multiple| J[Multiple Guide Curves with Separate Pierce Points]
    F --> K{Need Orientation Control?}
    K -->|Perpendicular to Path| L[Follow Path]
    K -->|Fixed to Starting Plane| M[Keep Normal Constant]
    K -->|Rotation Along Path| N[Twist Along Path]

Key Terms

• Sweep – a 3D modelling feature that creates geometry by moving a 2D profile along a defined path
• Profile – the closed 2D cross-sectional shape being swept along a path
• Path – the trajectory (2D, 3D, or model edge) that guides the profile's movement
• Guide Curve – a secondary sketch or edge used to scale or deform the profile during the sweep
• Pierce Relation – a sketch constraint that forces a point on the profile to intersect a curve passing through the sketch plane; essential for guide curve connections
• Follow Path – a sweep orientation option where the profile remains perpendicular to the path tangent at all points
• Keep Normal Constant – a sweep orientation option where the profile's plane remains fixed relative to its starting orientation
• Twist Along Path – a sweep option that rotates the profile around the path axis by a specified amount
• Swept Cut – a sweep operation that removes material from an existing body rather than adding it
• Helix/Spiral – a curve type defined by pitch and revolutions, commonly used as a path for thread creation
• Selection Manager – a tool for selecting specific segments from multi-segment paths (loops, open loops, individual edges)
• Convert Entities – a sketch tool that captures existing geometry (e.g., a circular edge) into the active sketch

Quick Revision

• A sweep creates 3D geometry by driving a 2D profile along a path
• The profile and path must intersect and be separate sketches
• Paths can be 2D sketches, 3D sketches, model edges, helices, or composite curves
• Guide curves change the profile's size/shape during the sweep; the profile must be pierced to each guide curve
• Multiple guide curves provide extreme shape control but require distinct pierce points on the profile
• Follow Path keeps the profile perpendicular to the path; Keep Normal Constant locks it to the original plane
• Twist Along Path rotates the profile by a defined number of degrees, radians, or turns
• Swept Cuts remove material using the same profile/path logic as additive sweeps
• Thread creation combines a helix path with a swept cut using a V-shape or trapezoid profile
• Always clean up thread start/end geometry with chamfers or revolve cuts to remove incomplete threads