Toolpaths: what each one is for
Short answer
A toolpath is a set of movements built from a shape plus a tool plus depths. Profile follows an outline. Pocket clears an area. V-carve varies depth to make crisp lettering. Drilling makes holes. The rest are variations on those four ideas.
The map
| Toolpath | What it does | Typical tool |
|---|---|---|
| Profile | Follows an outline to cut a shape out or trim an edge | End mill |
| Clears all the material inside a closed shape | End mill | |
| V-carve | Varies depth so a V-bit touches both walls of a shape | V-bit |
| Engraving | Follows a line at a fixed depth with a V-bit or engraver | V-bit, engraver |
| Drilling | Plunges at points to make holes | Drill or end mill |
| Fluting | Runs a shaped bit along a line to cut a decorative groove | Core box, ball nose, V-bit |
| Texture | Covers an area with a repeating or random pattern | Ball nose, V-bit |
| Prism carving | Raises a shape as a faceted prism rather than cutting it in | V-bit |
| Inlay | Cuts a pocket and a matching plug that fills it | V-bit or end mill |
| 3D roughing | Removes bulk material from around a 3D model | Flat end mill |
| 3D finishing | Follows the model surface in close passes | Ball nose |
| Rest machining | Cuts only what a previous larger tool could not reach | Smaller end mill or ball nose |
| Surfacing | Skims a large flat area level | Surfacing bit |
Settings nearly all of them share
| Setting | What it means | Common mistake |
|---|---|---|
| Start depth | How far below zero the toolpath begins cutting | Leaving it at 0 when the area was already cleared by an earlier pass |
| Cut depth | How deep the toolpath goes, measured from the start depth | Reading it as depth from zero when it is depth from start depth |
| Depth per pass | How much each pass takes. See depth per pass. | Too deep for the machine |
| Stepover | Sideways distance between passes. See stepover. | Using a percentage on a ball nose finishing pass |
| Allowance | Material deliberately left for a later pass | Forgetting to remove it in the finishing operation |
| Safe Z / clearance | Height for rapid moves between cuts | Set lower than a clamp or a fixture |
| Cut direction | Climb or conventional. See climb versus conventional. | Ignoring it on finishing passes where it shows |
| Ramp / lead in | How the tool enters the material | Not using one, and breaking bits on plunge |
Order of operations
The sequence matters more than people expect, because each operation changes what is holding the workpiece and what the tool can reach.
- Surface or flatten the stock if it needs it, while it is still a full solid piece.
- Drill and pocket internal features while the material is still fully supported and held.
- Carve and engrave decorative detail.
- Profile last. Once the outline is cut, the part is only held by tabs.
The most common ordering mistake
Cutting the profile before the pocket. Once the part is free of the sheet, it moves under the cutter, and everything after that is wrong or dangerous. If your CAM lets you drag toolpaths into order, check that order every time before posting.Tool changes
Group toolpaths by tool where you can, so you change bits as few times as possible. Each tool change is a chance to lose Z zero, so:
- Re-zero Z after every tool change unless you have an automatic tool length sensor.
- Do not re-zero XY. That has not moved, and re-doing it introduces error.
- Check the bit is actually the one the next toolpath expects. A 1/8 inch path run with a 1/4 inch bit is an immediate ruined part.