CNC Machining
CNC machining removes material from solid stock with a programmed cutting tool, producing accurate parts directly from a CAD model with no tooling.
- Part
- Cutting
- Revised
- 2026-08-11
At a glance
- Family
- Mechanical
- Typical tolerances
- ±0.005 in (±0.13 mm) standard shop practice, equivalent to ISO 2768-m; ±0.001 in (±0.025 mm) for precision work; ±0.0002 in (±0.005 mm) on ground and precision-turned features.
- Surface finish
- Ra 125 µin (3.2 µm) as machined by default; Ra 63 µin (1.6 µm) with a finishing pass and Ra 32 µin (0.8 µm) with light finish cuts. Below Ra 16 µin (0.4 µm) requires grinding, lapping, or polishing.
- Typical volumes
- 1–10,000 parts; unit cost drops steeply from 1 to about 10 pieces, then flattens
- Lead time
- 3–10 business days for typical prototype and low-volume work, with 1–3 day expedite widely available. Production runs are scheduled against machine capacity rather than tooling lead time.
- Materials
- Wood, Plastic, Composite, Metal
What it is
CNC machining removes material from a solid block or bar with programmed cutting tools, producing finished parts directly from a CAD model with no tooling of any kind. Standard shop practice holds ±0.005 in (±0.13 mm); precision work holds ±0.001 in (±0.025 mm), and ground or precision-turned features reach ±0.0002 in (±0.005 mm) — an order of magnitude tighter than any additive process.
It is the most material-agnostic process in manufacturing. Aluminum, stainless and tool steels, titanium, brass and copper, engineering plastics such as POM, PEEK, and PC, glass and carbon composites, and hardwood and sheet stock all machine on the same machines with different tooling and parameters. Crucially, the part has the full, certified properties of wrought stock — no layer boundaries, no porosity, no sintering shrinkage.
The economics are the mirror image of molding: no tooling cost, high per-part cost, and a unit price that falls with quantity only as programming and fixturing amortize. Typical range is 1 to 10,000 parts, delivered in 3–10 business days.
How it works
- CAM programming. The solid model is imported, stock and work offsets defined, and toolpaths generated for each operation. Programming is a fixed cost per part number, which is why the first piece is disproportionately expensive and the tenth is not.
- Workholding and setup. The part is clamped in a vise, on a fixture plate, or in a chuck. Every orientation the tool must approach from is a separate setup, and each setup adds labor plus a positional stack-up of roughly 0.002–0.005 in (0.05–0.13 mm) between features machined in different setups. This is why 5-axis machines earn their cost: they reach five faces in one setup.
- Roughing. Bulk material is removed at high feed and depth of cut, leaving 0.010–0.020 in (0.25–0.5 mm) of stock. Material removal rate here is what sets cycle time on any part with significant volume to clear.
- Semi-finishing and finishing. Light radial depths at higher surface speed produce the final geometry and surface. Cutting speed varies enormously by material — carbide in 6061 aluminum runs several times the surface speed usable in 304 stainless and roughly five to ten times that usable in Ti-6Al-4V — which is why material choice moves cycle time and price so much.
- Hole making. Drilling for clearance and pilot holes, then reaming or boring where a bore tolerance or finish is specified, then tapping or thread milling.
- Secondary setups. The part is re-fixtured to machine remaining faces, sometimes on soft jaws cut to match the first-operation geometry.
- Deburr and inspect. Edge breaks are a hand or tumbling operation. Dimensional inspection ranges from calipers on general tolerances to CMM reports on toleranced and geometrically controlled features.
Design guidelines
Internal corner radii
Every internal vertical corner takes the radius of the tool that cut it — there is no sharp internal corner in a milled pocket. Specify a radius of at least one third the pocket depth, and make it 15–20% larger than the nominal tool radius so the cutter sweeps an arc rather than engaging the full slot width, which chatters and burns tools.
Pocket depth
Stay within 4× tool diameter for standard tooling; reduced-neck and long-reach tools go to 6–10× at lower feeds and with visible taper. Depth and corner radius are linked — a 0.5 in (12 mm) deep pocket with a 0.125 in (3 mm) corner radius forces a long, thin cutter and costs several times what a 0.25 in (6 mm) radius would.
Wall thickness
0.031 in (0.8 mm) minimum in metal and 0.060 in (1.5 mm) in plastic. Watch aspect ratio too: a wall taller than about 10× its thickness deflects away from the cutter and finishes thin and wavy.
Holes and threads
Use standard drill diameters — see the drill size chart. Depth is limited to roughly 4× diameter with a standard drill and 10× with peck cycles; deeper needs gun drilling. A tapped depth of 1.5× thread diameter develops essentially full strength in similar materials, so deeper is wasted machine time. Use standard sizes from the thread size chart and pilots from the tap drill chart, and thread mill large, blind, or hard-material threads instead of tapping them.
Undercuts
Undercuts need T-slot, dovetail, or lollipop cutters. Design them to standard widths — retaining-ring grooves and O-ring glands are standardized for exactly this reason. Non-standard undercuts mean custom tooling.
Tolerances and datums
Put ISO 2768-m (or a blanket ±0.005 in) in the title block and call out only the features that genuinely need more; every tightened dimension adds inspection time and may add a grinding operation. Where a fit is involved, specify the fit class rather than a symmetric tolerance — the ISO 286 fits and tolerances chart gives the values, and the GD&T symbols chart covers the geometric controls that communicate function better than a bilateral tolerance.
Surface finish
Ra 125 µin (3.2 µm) is the default machined finish. Ra 63 µin (1.6 µm) costs a finishing pass, Ra 32 µin (0.8 µm) costs light cuts, and below Ra 16 µin (0.4 µm) means grinding, lapping, or polishing — see the surface finish chart. Specify a finer finish only where it does work: sealing faces, sliding surfaces, fatigue-critical fillets.
Non-metals
Abrasive materials — carbon and glass composites, MDF, filled plastics — consume carbide quickly and want diamond-coated or PCD tooling. Unfilled thermoplastics need sharp positive-rake geometry and good chip evacuation, because rubbing generates heat the polymer cannot conduct away and the chip re-welds to the surface.
| Feature | Recommended | Limit | Why |
|---|---|---|---|
| Internal corner radius | 1/3 of pocket depth | Tool radius + 15% | Full-radius engagement chatters |
| Pocket depth | 4× tool diameter | 10× with special tooling | Tool deflection and chatter |
| Wall thickness, metal | 0.060 in (1.5 mm) | 0.031 in (0.8 mm) | Deflection under cutting load |
| Wall thickness, plastic | 0.080 in (2 mm) | 0.060 in (1.5 mm) | Lower stiffness, heat build-up |
| Hole depth | 4× diameter | 10× with peck drilling | Chip evacuation |
| Tapped depth | 1.5× diameter | 3× diameter | No added strength beyond 1.5× |
| Text | Engraved 0.020 in (0.5 mm) wide | 0.012 in (0.3 mm) | Smallest practical engraving cutter |
| General tolerance | ±0.005 in (ISO 2768-m) | ±0.001 in precision | Every tightened dimension adds cost |
Cost drivers
Machining is billed in spindle hours plus setup labor plus material, and the three respond to different design decisions.
Cycle time follows material removal volume and machinability. Roughing away 80% of a billet costs real money; so does a material that must be cut slowly. Aluminum 6061 is the cheapest common metal to machine, stainless costs meaningfully more, and titanium and nickel superalloys more again — both from slow cutting speeds and from tool consumption.
Setups are the step change. Each new orientation adds fixturing and handling labor and introduces a tolerance stack between setups. A part that can be finished in two setups on a 3-axis mill is dramatically cheaper than one needing five, which is the entire economic argument for 5-axis work.
Tolerance and finish multiply both. A blanket ±0.001 in can double the price of a part where only two features needed it.
Volume breakpoints: unit cost falls steeply from 1 to about 10 parts as programming and fixturing amortize, then flattens — going from 100 to 1,000 pieces changes the price far less than going from 1 to 10. Against injection molding, machining loses somewhere between 100 and 1,000 parts for small plastic components. Against investment casting or die casting, the crossover is typically a few hundred to a few thousand.
- Loosen every tolerance that does not do work, and call out the few that do.
- Design so the part can be finished in as few setups as possible.
- Increase internal corner radii — it lets the shop use a larger, stiffer, faster tool.
- Use standard drill, tap, and stock sizes; non-standard means special tooling or extra operations.
- Choose 6061 over 7075 and either over stainless unless the property is genuinely required.
Questions
6 questionsWhat tolerance can CNC machining hold?
±0.005 in (±0.13 mm) is standard shop practice and equivalent to ISO 2768-m. Precision work reaches ±0.001 in (±0.025 mm), and ground or precision-turned features get to ±0.0002 in (±0.005 mm). Cost rises sharply below ±0.001 in, so tighten only the features that need it.
Why do CNC pockets have rounded internal corners?
Because a rotating cutter cannot produce a sharp internal vertical corner — the corner takes the radius of the tool. Specify a radius of at least one third the pocket depth, and make it 15–20% larger than the nominal tool radius so the cutter sweeps an arc rather than engaging the full slot width.
How deep can a CNC pocket be?
About 4× the cutting tool diameter with standard tooling. Reduced-neck and long-reach tools extend that to 6–10× at lower feeds and with more chatter and taper. Depth and corner radius are linked: a deep pocket with a small corner radius forces a long, thin, expensive tool.
How deep should a tapped hole be?
1.5× the thread diameter develops essentially full thread strength when the fastener and part are similar materials. Deeper adds machine time and tap breakage risk without adding strength. In soft materials such as aluminum with a steel fastener, 2× diameter is a reasonable allowance.
Why does the number of setups matter so much?
Each setup is a re-fixturing operation with its own labor, and features machined in different setups carry a positional stack-up of roughly 0.002–0.005 in (0.05–0.13 mm) between them. Reducing setups cuts both cost and tolerance stack, which is why 5-axis machining is worth its higher hourly rate on complex parts.
When is CNC machining cheaper than injection molding?
Below roughly 100–1,000 parts for small plastic components, depending on complexity and mold cost. Machining has no tooling charge but a high per-part cost that flattens rather than falls with quantity, while molding has the opposite profile.