Sketch Operations

Sketch operations transform 2D profiles into 3D solids. They are essential for creating parts with complex geometry that cannot be achieved with primitives and booleans alone.

Overview

All sketch operations require a closed profile—a series of connected line and arc segments that form a closed loop.

Extrude

Sweeps a closed profile along a linear direction to create a prismatic solid.

Part::extrude(
    plane: SketchPlane,
    origin: Vec3,
    segments: &[SketchSegment2D],
    direction: Vec3,
) -> Part

Creates:

• 2 cap faces (start and end profiles)
• N lateral faces (one per profile segment)

// L-shaped bracket profile
let profile = vec![
    SketchSegment2D::line([0.0, 0.0], [20.0, 0.0]),
    SketchSegment2D::line([20.0, 0.0], [20.0, 5.0]),
    SketchSegment2D::line([20.0, 5.0], [5.0, 5.0]),
    SketchSegment2D::line([5.0, 5.0], [5.0, 30.0]),
    SketchSegment2D::line([5.0, 30.0], [0.0, 30.0]),
    SketchSegment2D::line([0.0, 30.0], [0.0, 0.0]),
];

// Extrude 50mm along Z
let bracket = Part::extrude(
    SketchPlane::XY,
    Vec3::new(0.0, 0.0, 0.0),
    &profile,
    Vec3::new(0.0, 0.0, 50.0),
);

When to Use Extrude

• Parts with constant cross-section
• Plates, brackets, structural members
• Features like bosses and ribs
• Quick prototyping of mechanical parts

Revolve

Rotates a closed profile around an axis to create a solid of revolution.

Part::revolve(
    plane: SketchPlane,
    origin: Vec3,
    segments: &[SketchSegment2D],
    axis_origin: Vec3,
    axis_dir: Vec3,
    angle_deg: f64,
) -> Part

Creates:

• Full 360-degree rotation: closed toroidal/cylindrical surfaces
• Partial rotation: wedge with cap faces at start/end angles

// Wine glass profile (cross-section)
let profile = vec![
    SketchSegment2D::line([0.0, 0.0], [30.0, 0.0]),   // base
    SketchSegment2D::line([30.0, 0.0], [30.0, 5.0]),
    SketchSegment2D::line([30.0, 5.0], [5.0, 5.0]),
    SketchSegment2D::line([5.0, 5.0], [3.0, 50.0]),   // stem
    SketchSegment2D::line([3.0, 50.0], [20.0, 60.0]), // bowl
    SketchSegment2D::arc([20.0, 60.0], [25.0, 80.0], [22.0, 70.0]),
    SketchSegment2D::line([25.0, 80.0], [0.0, 80.0]),
    SketchSegment2D::line([0.0, 80.0], [0.0, 0.0]),
];

// Full revolution around Y axis
let glass = Part::revolve(
    SketchPlane::XY,
    Vec3::ZERO,
    &profile,
    Vec3::new(0.0, 0.0, 0.0),  // axis through origin
    Vec3::new(0.0, 1.0, 0.0),  // Y axis
    360.0,
);

Partial Revolve

// Quarter pie slice
let pie_slice = Part::revolve(
    SketchPlane::XY,
    Vec3::ZERO,
    &profile,
    Vec3::ZERO,
    Vec3::new(0.0, 0.0, 1.0),  // Z axis
    90.0,  // 90-degree wedge
);

When to Use Revolve

• Rotationally symmetric parts (wheels, pulleys, knobs)
• Turned parts (lathe operations)
• Bottles, vases, bowls
• Pie-chart style wedges

Sweep

Moves a closed profile along a 3D path curve with optional twist and scale.

Part::sweep(
    plane: SketchPlane,
    origin: Vec3,
    segments: &[SketchSegment2D],
    path: &PathCurve,
    options: SweepOptions,
) -> Part

SweepOptions

// Curved pipe
let circle_profile = vec![
    SketchSegment2D::arc([5.0, 0.0], [-5.0, 0.0], [0.0, 5.0]),
    SketchSegment2D::arc([-5.0, 0.0], [5.0, 0.0], [0.0, -5.0]),
];

let curved_path = PathCurve::arc(
    Vec3::new(0.0, 0.0, 0.0),
    Vec3::new(50.0, 50.0, 0.0),
    Vec3::new(50.0, 0.0, 0.0),
);

let pipe = Part::sweep(
    SketchPlane::YZ,
    Vec3::ZERO,
    &circle_profile,
    &curved_path,
    SweepOptions::default(),
);

Sweep with Twist

// Twisted ribbon
let rect_profile = vec![
    SketchSegment2D::line([0.0, -1.0], [0.0, 1.0]),
    SketchSegment2D::line([0.0, 1.0], [10.0, 1.0]),
    SketchSegment2D::line([10.0, 1.0], [10.0, -1.0]),
    SketchSegment2D::line([10.0, -1.0], [0.0, -1.0]),
];

let straight_path = PathCurve::line(
    Vec3::new(0.0, 0.0, 0.0),
    Vec3::new(0.0, 0.0, 100.0),
);

let ribbon = Part::sweep(
    SketchPlane::XY,
    Vec3::ZERO,
    &rect_profile,
    &straight_path,
    SweepOptions {
        twist_angle: std::f64::consts::PI,  // 180-degree twist
        ..Default::default()
    },
);

Helix (Spring)

// Compression spring
let wire_profile = vec![
    SketchSegment2D::arc([1.5, 0.0], [-1.5, 0.0], [0.0, 1.5]),
    SketchSegment2D::arc([-1.5, 0.0], [1.5, 0.0], [0.0, -1.5]),
];

let helix = PathCurve::helix(
    radius: 10.0,
    pitch: 5.0,   // 5mm per revolution
    turns: 8.0,
);

let spring = Part::sweep(
    SketchPlane::XY,
    Vec3::new(10.0, 0.0, 0.0),
    &wire_profile,
    &helix,
    SweepOptions::default(),
);

When to Use Sweep

• Pipes, tubes, and conduits
• Rails and extrusions along curves
• Springs and helical features
• Handles and curved structural members
• Wire/cable routing visualization

Loft

Interpolates between multiple profiles at different positions to create a smooth transition solid.

Part::loft(
    profiles: &[LoftProfile],
    closed: bool,
) -> Part

LoftProfile

Each profile contains:

Requirements:

• Minimum 2 profiles
• All profiles must have the same number of segments
• Profiles should be at different positions in 3D space

// Transition from square to circle
let square_profile = vec![
    SketchSegment2D::line([-10.0, -10.0], [10.0, -10.0]),
    SketchSegment2D::line([10.0, -10.0], [10.0, 10.0]),
    SketchSegment2D::line([10.0, 10.0], [-10.0, 10.0]),
    SketchSegment2D::line([-10.0, 10.0], [-10.0, -10.0]),
];

// Approximate circle with 4 arcs to match segment count
let circle_profile = vec![
    SketchSegment2D::arc([-10.0, 0.0], [0.0, -10.0], [-7.0, -7.0]),
    SketchSegment2D::arc([0.0, -10.0], [10.0, 0.0], [7.0, -7.0]),
    SketchSegment2D::arc([10.0, 0.0], [0.0, 10.0], [7.0, 7.0]),
    SketchSegment2D::arc([0.0, 10.0], [-10.0, 0.0], [-7.0, 7.0]),
];

let adapter = Part::loft(
    &[
        LoftProfile {
            plane: SketchPlane::XY,
            origin: Vec3::new(0.0, 0.0, 0.0),
            segments: square_profile,
        },
        LoftProfile {
            plane: SketchPlane::XY,
            origin: Vec3::new(0.0, 0.0, 50.0),
            segments: circle_profile,
        },
    ],
    false,
);

Multi-Profile Loft

// Airfoil transitioning along span
let profiles = vec![
    LoftProfile {
        plane: SketchPlane::XZ,
        origin: Vec3::new(0.0, 0.0, 0.0),
        segments: root_airfoil.clone(),
    },
    LoftProfile {
        plane: SketchPlane::XZ,
        origin: Vec3::new(0.0, 100.0, 5.0),
        segments: mid_airfoil.clone(),
    },
    LoftProfile {
        plane: SketchPlane::XZ,
        origin: Vec3::new(0.0, 200.0, 10.0),
        segments: tip_airfoil.clone(),
    },
];

let wing = Part::loft(&profiles, false);

Closed Loft (Tube)

// Torus-like shape
let profile = create_circle_profile(5.0);

let ring = Part::loft(
    &[
        LoftProfile {
            plane: SketchPlane::YZ,
            origin: Vec3::new(30.0, 0.0, 0.0),
            segments: profile.clone(),
        },
        LoftProfile {
            plane: SketchPlane::XZ,
            origin: Vec3::new(0.0, 30.0, 0.0),
            segments: profile.clone(),
        },
        LoftProfile {
            plane: SketchPlane::YZ,
            origin: Vec3::new(-30.0, 0.0, 0.0),
            segments: profile.clone(),
        },
        LoftProfile {
            plane: SketchPlane::XZ,
            origin: Vec3::new(0.0, -30.0, 0.0),
            segments: profile.clone(),
        },
    ],
    true,  // Connect last to first
);

When to Use Loft

• Transitioning between different shapes
• Organic forms (bottles, vases, aerodynamic shapes)
• Turbine and propeller blades
• Ductwork and HVAC transitions
• Ergonomic handles and grips

Sketch Segments

Profile geometry is defined using 2D segments:

Line Segment

SketchSegment2D::line(start: [f64; 2], end: [f64; 2])

Arc Segment

SketchSegment2D::arc(start: [f64; 2], end: [f64; 2], mid: [f64; 2])

The mid point lies on the arc between start and end, defining the curve direction and radius.

Edge Cases

Operation Comparison