CAM and Toolpaths

Roughing and finishing strategies, adaptive clearing, lead-ins, scallop height, simulation and post processors.

On this page

What CAM does
Setting up the job
Clearing strategies
Adaptive clearing
Entering the cut
Finishing and 3D surfaces
Tolerance, arcs and stock to leave
Nesting and sheet work
Simulation and verification
Post processors
FAQ

What CAM does

CAM (computer-aided manufacturing) turns a 3D model into toolpaths and then into G-code. You tell it what to cut (which faces, pockets and holes), with which tools, at which speeds, feeds and depths, and it computes where each tool should go. Good CAM is mostly good decisions about how to remove the material: where to take heavy cuts, where to finish lightly, and how to enter and leave the cut safely.

Free and low-cost CAM: FreeCAD Path, Fusion (personal use), Carbide Create, Estlcam, Vectric and others. The concepts below apply to all of them.
2D, 2.5D and 3D. 2D and 2.5D cut outlines and pockets at constant depths (most parts). 3D follows a surface in X, Y and Z at the same time.
CAM does not know your machine’s strength. You set the depths and feeds; a program that works on a mill will break a tool on a router.

Setting up the job

Stock. Enter the size of the raw material, and where the part sits in it. Leave extra stock to face and to clamp.
Work coordinate system (WCS). Put zero where you will set it on the machine: a corner of the stock, or the vise jaw, with Z zero on the top of the stock or the part.
Tool library. Create each tool with its true diameter, flutes, flute length, stick-out and holder, and its speeds and feeds. Keep the same numbers as the machine’s tool table.
Safe heights. The retract height must clear the clamps and the vise; the clearance height sets the rapid-move level.
Operations in order: face, rough, semi-finish, finish, drill and tap, chamfer, engrave. Rough with a big tool, finish with the smallest tool the corners require.

Clearing strategies

Four ways to clear a pocket: zigzag, offset contours, adaptive clearing and rest machining.

Strategy	How it works	Good for	Watch out for
Zigzag (parallel)	Straight passes back and forth	Large open areas; simple programs	Full-width engagement at the start of each pass; sharp turns at the ends
Offset (contour-parallel)	Concentric loops following the outline	Pockets with irregular shapes; a good finish	The tool is fully engaged where loops meet in corners
Adaptive / dynamic / high-efficiency	Loops with a constant, low engagement angle	Roughing hard metals; deep cuts; reducing tool wear	Needs a rigid machine and more power for the fast feeds; long programs
Rest machining	A smaller tool cuts only what the big tool left	Cleaning corners	The smaller tool must be short and stiff
Contour (profile)	Follows the outline	Walls and part outlines; finishing	Compensation errors in tight corners
Engrave / V-carve	Follows a line or fills a letter	Text and artwork	Cutting speed depends on the contact diameter

Adaptive clearing

A conventional path takes a wide slice (half the diameter or more), but its engagement jumps in corners and when the tool changes direction. Each jump is a load spike that wears the tool and can break it. An adaptive (also called dynamic, high-efficiency or trochoidal) path keeps the engagement angle constant and small, usually 5–15 % of the diameter, but uses the whole length of the flute. The tool takes a deep, narrow cut at high feed and moves smoothly.

Worked example: a 10 mm, 3-flute carbide mill in steel

At 100 m/min and f_z = 0.04 mm: n = 3 183 rpm and V_f = 382 mm/min at half-diameter width.
Conventional: a_e = 5 mm, a_p = 5 mm. MRR = 5 × 5 × 382 = 9 549 mm³/min.
Adaptive: a_e = 1 mm (10 %), a_p = 20 mm (two diameters). The chip-thinning factor is 10 ÷ (2 × √(10 × 1 − 1)) = 1.67, so V_f rises to 637 mm/min. MRR = 1 × 20 × 637 = 12 732 mm³/min, 1.3 times as much.
The adaptive cut spreads wear over 20 mm of flute, not 5 mm, so the tool lasts longer; the cost is spindle power and a rigid machine.
On a hobby machine the same idea is used with a smaller cut: a_e of 10 % and a_p of 1–2 × D in aluminum, at feeds the machine can reach.

Entering the cut

Lead-in arc to a wall, and the three ways of going down: plunge, ramp and helix.

Plunge straight down only with a center-cutting tool and a light feed; it loads the tool end-on and is hard on small mills.
Ramp in along a slope of 2–5° over a path of several diameters. At 3°, a 5 mm drop needs 95 mm of path.
Helix in with a spiral of a diameter 1.5–2 × the tool: smooth and effective for pockets and holes; the diameter must clear the tool’s center.
Pre-drill a hole in hard materials, then let the end mill start there.
Lead-in and lead-out arcs bring the tool onto the finished wall tangentially. They avoid the mark a straight plunge leaves at the start point, and they apply compensation smoothly.
Cut direction. Choose climb for most contours; use conventional for a rough skin or a machine with backlash.

Finishing and 3D surfaces

On a flat floor or a vertical wall the finish is set by the feed and the tool’s sharpness. On a 3D surface made with a ball cutter, the passes leave ridges called scallops between them, whose height depends on the ball radius R and the step-over s.

h = R − √(R² − (s ÷ 2)²)

Scallop height on a flat surface against stepover for three ball diameters.

Worked example: a 6 mm ball nose cutter (R = 3 mm)

1.0 mm step-over: h = 3 − √(9 − 0.25) = 42 µm.
0.6 mm: h = 15 µm. 0.3 mm: h = 3.8 µm.
For a 5 µm scallop the step-over is 2 × √(2 × 3 × 0.005 − 0.005²) = 0.35 mm. Halving the step-over quarters the scallop but doubles the time.
On a sloped surface the scallop is larger across the slope direction; CAM’s “scallop” strategy keeps it constant by adjusting the step-over.

Parallel (raster) finishing is simple and good on shallow surfaces; waterline (Z-level) suits steep walls; pencil cleans concave corners; scallop (constant step-over) follows the surface and gives an even finish.
Finishing pass. Leave 0.1–0.5 mm for it, use a sharp tool at a light depth, and cut the walls last (climb) so that any tool push-off is removed.
Ball nose tips do not cut at the center: tilt the tool or keep the contact off the tip on shallow surfaces.

Tolerance, arcs and stock to leave

CAM turns curves into many short straight segments. The toolpath tolerance sets how far the segments may stray from the true curve. Looser tolerances make smaller programs; tighter ones make smoother parts and larger files.

chord error e = R − √(R² − (L ÷ 2)²) segment length for an error e: L = 2 × √(2 R e − e²)

On a 10 mm radius, a tolerance of 0.01 mm allows segments up to 0.89 mm long. A 0.25 mm segment gives an error of only 3.1 µm.
Set the toolpath tolerance to about one-tenth of the part’s tolerance: 0.01 mm for a ±0.1 mm feature is ample. Smaller values slow the machine, because the controller cannot read tiny segments quickly.
Stock to leave (allowance). Roughing leaves 0.2–0.5 mm on walls and floors, so that the finishing pass cleans up with a constant, light cut. Roughing with no allowance leaves tool marks and any deflection error in the part.
Arc output. If the controller supports G2/G3, output arcs where the model has them; the program shrinks and the surface is smoother.
Corner rounding. A controller in a “smoothing” mode may cut corners; select exact-stop or constant-velocity mode as appropriate.

Nesting and sheet work

Nesting arranges parts on a sheet to waste the least material. Leave the width of the tool plus a margin between parts, and respect the grain on wood and the direction of printed material.
Tabs hold cut-out parts to the sheet. Make them small (3–5 mm wide, 1–2 mm tall), enough to resist the cutting force, and remove them with a chisel or sander afterwards. For the vacuum table, an onion-skin final layer of 0.2–0.5 mm is common.
Order of cutting. Cut inside holes and pockets first, then the outside, so the part stays held.
Tool compensation. An outside profile is cut on the outside of the line, an inside profile on the inside, so that the part is the right size. Fits made on a router need a test; see Designing for CNC Milling.
Spoilboard. Cut slightly into the spoilboard so the part separates cleanly, and skim the spoilboard flat occasionally.

Simulation and verification

Backplot shows the toolpath lines; material-removal simulation shows the stock being cut, including the tool holder. Use the second.
Check for: gouges into the finished surface, uncut material in corners, the holder or collet touching the wall or a clamp, rapid moves through the part, and wrong units.
Compare the simulation with the model using the software’s deviation tool when the surface matters.
Run the post-processed G-code in a viewer, as well as the CAM preview, so that you check what the machine will really get.
Air cut at a raised Z before the first real cut, in single-block mode with a reduced rapid override.

Post processors

The post processor is the translator between CAM’s generic toolpaths and the dialect of your controller. It decides how tool changes, coolant, arcs, work offsets, program numbers and the program’s start and end are written.

Use the right post. A wrong post can give an inch program on a metric machine, the wrong arc format, a missing tool change or an unsafe move.
Edit the header and footer to put your safe-start line (G21 G90 G17 G54 G40 G80), spindle commands, and retract sequence.
Test every new post with a short program and an air cut. Check the first moves, tool changes and arcs before cutting.
Keep the post with the job. When a program fails years later, you need to know which post and which settings produced it.
Arc format: some controllers (GRBL) want I and J; some accept R. Check this with a test circle.

CNC Machining: the overview of this guide.
G-code and Programming: reading and writing the programs CAM produces.
Milling: Operations and Tooling: tools, chip load and chip thinning.
Designing for CNC Milling: drawing parts that are easy to program.
CNC Feeds & Speeds Calculator.

FAQ

What is the best CAM software for a beginner?

A beginner-friendly program that includes a simulator and a basic post for your machine: Fusion (for personal use), Carbide Create, Estlcam, Vectric or FreeCAD Path. The best one is the one you will learn properly, and it matters less than learning the strategies.

Why does my machine slow down on a complex 3D toolpath?

The controller cannot read tiny line segments fast enough. Loosen the toolpath tolerance, output arcs, or use a smoother strategy; some controls have a look-ahead setting.

What is adaptive clearing and do I need it?

It is a roughing strategy with a constant, small engagement, deep cuts and fast feed. It is not essential, but it is gentle on the tool and removes metal quickly, and is worth using if your machine is rigid.

How much stock should I leave for finishing?

0.2–0.5 mm for metal, and 0.5–1 mm for woods that may move. Enough that the finishing tool cuts a uniform, light chip, not so much that it deflects.

Why is there a mark where the tool started the cut?

A straight plunge or a stop at the start leaves a mark. Use a tangent arc lead-in, ramp or helix, and finish the wall in one continuous pass.

References

CAM vendor documentation: Autodesk Fusion Manufacture, Vectric, FreeCAD Path workbench, Carbide Create (toolpath strategies, tolerance, tabs).
Oberg, E. et al., Machinery’s Handbook, 31st ed., Industrial Press: numerical control, milling.
Sandvik Coromant, Milling Handbook (circular interpolation, chip thickness and engagement).
Smid, P., CNC Programming Handbook, 3rd ed., Industrial Press.

Last reviewed: October 2026. Cutting data are starting points: machines, tools and materials differ, so test on scrap and follow the tool maker’s data.