Slide 002: Toolpath Types & Operations¶

Slide Visual¶

Toolpath Types & Operations

Slide Overview¶

This slide covers the major toolpath types used in CNC routing, when to use each one, and how they differ in terms of tool engagement, material removal strategy, and finish quality.

Instruction Notes¶

Profile/Contour Toolpath¶

Cuts along the perimeter of a shape. Three offset options: - Outside: Tool center offset outward by tool radius — for cutting out parts - Inside: Tool center offset inward — for cutting holes and internal features - On the line: Tool center follows the design line — for engraving, V-carving centerlines

Key parameters: - Stepdown: Depth per pass (typically 50–100% of tool diameter in wood) - Tabs: Small bridges to hold cut pieces (0.125"–0.25" wide, 0.04"–0.08" tall) - Lead-in/out: Arc or line entry to avoid plunge marks on finished edge - Direction: Climb vs. conventional milling

Pocket Toolpath¶

Removes all material within an enclosed boundary to a specified depth. The tool must clear the entire interior area using multiple overlapping passes.

Clearing strategies: - Offset/Spiral: Tool follows the pocket boundary inward in concentric passes — clean finish, consistent tool load - Raster/Zigzag: Tool moves in parallel lines — faster but leaves scallops at direction changes - Adaptive/Trochoidal: Tool follows a constant-engagement path — reduces tool load, ideal for hard materials and deep pockets

Stepover: 40–60% of tool diameter for roughing; 5–10% for finishing passes.

Drill Toolpath¶

Positions the spindle over specified coordinates and plunges to depth. Cycle types: - Simple drill: Single plunge to depth — for shallow holes - Peck drill (G83): Plunges incrementally, retracts to clear chips — for deep holes - Holes larger than the drill bit require a pocket or helical bore operation

V-Carve Toolpath¶

Uses a V-bit (typically 60° or 90°) to carve text and designs. The tool depth varies to match the width of the design — narrow features are shallow, wide features are deep. This creates a natural beveled appearance. V-carving requires vector input (not raster images).

3D Contour/Surface Toolpath¶

Follows a 3D surface model using parallel passes (raster) or contour-following (Z-level) strategies. Requires: - Ball-nose end mill (creates scalloped surface) - Small stepover (5–15% of tool diameter) for acceptable surface finish - Roughing pass first to remove bulk material before finishing - Scallop height formula: h = r - √(r² - (s/2)²), where r = tool radius, s = stepover

Key Talking Points¶

Profile cuts along edges; pocket clears areas; drill makes holes — each has a specific purpose
Toolpath strategy (offset vs. raster vs. adaptive) affects finish quality and tool life
V-carving depth is variable — it follows the design geometry automatically
3D contouring requires ball-nose tools and small stepovers for smooth surfaces
Always choose the simplest toolpath type that achieves the desired result

Learning Objectives (Concept Check)¶

[ ] Describe 5 toolpath types and identify when to use each
[ ] Explain the difference between inside, outside, and on-the-line profile cuts
[ ] Calculate approximate scallop height for a 3D contour toolpath

Last Updated: 2026-03-19