Toolpath Strategies & Simulation

The "what kind of cut" decisions inside CAM — facing, pocketing, contour, adaptive clearing, V-carving — and the simulators that catch your mistakes before the spindle does. Strategy choice depends on machine rigidity (machine type), tooling, and material. This page is reference-style: a vocabulary and a list of tools, not a textbook.

Core 2.5D strategies

• Facing — flatten the top of stock; large-diameter face mill or surfacing bit (½"–2"). Spoilboard surfacing routine on routers; soft-jaw prep on mills.
• Profile / contour — cut around the outside of a part (or inside a slot); the bread-and-butter cut.
• Pocketing — clear material inside a closed boundary. Sub-strategies: offset (zigzag from boundary), raster (back-and-forth), spiral, morphed spiral.
• Drilling / peck drilling — straight Z plunges; G81/G83 canned cycles. Peck is for deep holes to clear chips.
• Engraving — small V-bit or single-flute, shallow Z, fast feed. Often combined with V-carving.
• V-carving — depth varies with corner geometry; V-bit angle defines stroke width; the cornerstone of sign work. Vectric / Carveco / Estlcam / Carbide Create all do this well; Fusion 360 added it but it's clunky.

3-axis / 3D finishing

• Parallel / raster finishing — pass after pass in X (or Y); easy, slow.
• Scallop / constant-stepover finishing — keeps the cusps consistent across changing slopes; better-looking finish.
• Pencil tracing — tiny ball mill into corners to clean up after a larger ball.
• Steep & shallow — splits regions by surface angle and uses parallel for shallow + waterline for steep. Fusion / MeshCAM standard.
• Waterline / Z-level — horizontal slices with the ball mill; great for steep walls.

Adaptive / high-speed machining (HSM)

• Adaptive clearing — variable-engagement toolpaths that keep tool engagement constant by curving the path. Originated in Fusion HSM (now Fusion 360); now in many CAMs. Lets a tiny hobby spindle take deep, narrow cuts safely. The single biggest CAM advance for hobby CNC in the last decade.
• Trochoidal milling — circular tool motion in a slot; reduces heat and tool deflection.
• Ramping vs. plunging — ramp at a shallow angle to enter material instead of plunging straight down (most endmills hate plunging; only center-cutting bits handle it well).
• Pre-drilled lead-in — drill an entry hole, then start the adaptive path inside it. Works around non-center-cutting endmills.

Hobby-specific tricks

• ★ Dogbones / T-bones / fillets in inside corners — endmills can't cut sharp inside corners; "dogbone" overcuts give a square peg a place to seat. Estlcam, Vectric, Carbide Create all do this automatically.
• Tabs / onion skin — leave thin connective material so parts don't fly out at the end of a contour cut. Manual cleanup with a flush-cut bit.
• Climb vs. conventional milling — climb (down-milling) on rigid machines, conventional (up-milling) on hobby routers with backlash. Vectric and Estlcam expose this clearly.
• Stepover / stepdown — radial vs. axial engagement; the two knobs every hobby CAM exposes. Rules of thumb: 40% stepover for rough, 5–15% for finish; 50–100% diameter stepdown for adaptive.
• Tool tabs / fixturing tabs — fixed locations where the cutter avoids cutting through; lets parts stay attached to a sheet.

Simulation & verification (before you cut air)

• ★ CAMotics — open source (GPLv2+); standalone simulator with material removal preview. Drop in your G-code, watch the cut. Catches collisions, missed Z-clears, and rapid moves into stock. Free, cross-platform. The default for hobby G-code sanity-checking.
• ★ NC Viewer (ncviewer.com) — free in-browser G-code viewer; no install. Quick sanity-check that the toolpath looks right.
• OpenBuilds CONTROL preview — free; shows the toolpath in 3D before you hit start.
• G-Wizard Editor (CNCCookbook) — paid (~$80/yr); G-code editor + simulator + feeds-and-speeds combined; popular among Mach users.
• CutViewer Mill / Turn — paid Windows tools; classic CAM-simulator software.
• Vericut — paid, industrial; mentioned for completeness — extreme overkill for hobby.

Drag-knife / V-carve / specialty pathing

• Drag-knife paths — Donek Tools D2/D4 require swivel-corner moves at vertices; Estlcam, Vectric, and DeskProto generate these natively. Stepcraft and FoxAlien have their own.
• Hot-wire 4-axis (XYUV) paths — for foam wings; GMFC, DevWing Foam, JediCut generate them; output is often Mach3/GRBL-compatible.
• Lithophane / displacement maps — Carveco / Vectric / MeshCAM bake heightmaps into 3D toolpaths; the cheap "give them a custom photo on wood" deliverable.

Probing and adaptive G-code

• See Touch Probes & Zeroing — auto-zero and probing macros are themselves a kind of toolpath, just one that touches off rather than cutting.

Pick this if…

• Verify any G-code before cutting: CAMotics or NC Viewer.
• Tiny hobby spindle, want to push it: adaptive clearing in Fusion 360 (or Estlcam's "high-feed" mode).
• Sign making / inlays: V-carving in Vectric or Carveco.
• 3D figures from STL on a router: parallel + scallop in MeshCAM, or Fusion 3D toolpaths.
• Drag-knife on a router: Estlcam (cheap, very good at it) or Vectric.
• Foam-wing hot-wire: GMFC or JediCut.