## 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 --- ## Detailed Notes ### 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 | Path Type | Description | |-----------|-------------| | **2D Sketches** | Lines, arcs, splines within a single sketch plane | | **3D Sketches** | Complex curves moving through all three axes (X, Y, Z) | | **Model Edges** | Existing edges of solid bodies used directly as a path (no separate sketch needed) | | **Curves** | Helices, spirals, composite curves, or projected curves | #### 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 | Option | Behaviour | |--------|-----------| | **Follow Path** (Default) | Profile remains **perpendicular** to the path at all times; it tilts to stay perpendicular to the local tangent of the curve | | **Keep Normal Constant** | Profile remains **parallel to its original starting plane** throughout the entire sweep; the path directs translation only, not rotation | --- ### 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: | Method | Description | |--------|-------------| | **Degrees** | Total rotation in degrees from start to finish | | **Radians** | Total rotation specified in radians | | **Turns** | Number of complete 360° revolutions along the path | --- ### 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 | Feature | Swept Boss/Base | Swept Cut | |---------|-----------------|-----------| | **Purpose** | Adds material | Removes material | | **Requires** | Closed profile + path | Closed profile + path | | **Typical Use** | Pipes, wires, rails, mouldings | Threads, grooves, channels, toolpaths | | **Process** | Identical sweep setup | Identical sweep setup | ### Profile Orientation Comparison | Setting | Profile Behaviour | Best For | |---------|-------------------|----------| | **Follow Path** | Perpendicular to path tangent | Pipes, conduits, rails following curves | | **Keep Normal Constant** | Fixed to original sketch plane | Flat profile shapes swept along curved paths | | **Twist Along Path** | Rotates around path axis | Drill bits, twisted wire, decorative elements | --- ## Diagrams ### Basic Sweep Process ```mermaid 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 ```mermaid 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 ```mermaid 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 ```mermaid 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