---
type: process
name: "CNC Milling"
category: "Cutting"
subcategory: "Mechanical"
materials: ["Metal", "Plastic", "Wood", "Composite"]
tolerances: "±0.005 in (±0.13 mm) standard; ±0.001 in (±0.025 mm) precision; ±0.0005 in (±0.013 mm) on selected features"
volumes: "1–1,000 parts typical; economical to roughly 10,000 depending on cycle time"
lead_time: "3–10 business days for prototypes; 2–4 weeks for production quantities"
url: https://manufacturingprocesses.org/processes/cutting/cnc-milling
---

# CNC Milling

CNC milling removes material with a rotating multi-flute cutter moved along programmed paths, producing prismatic parts from solid stock.

- **Category**: [Cutting](https://manufacturingprocesses.org/processes/cutting.md)
- **Family**: Mechanical
- **Materials**: Metal, Plastic, Wood, Composite
- **Typical tolerances**: ±0.005 in (±0.13 mm) standard; ±0.001 in (±0.025 mm) precision; ±0.0005 in (±0.013 mm) on selected features
- **Surface finish**: 125 µin Ra (3.2 µm) as-machined; 63 µin (1.6 µm) with a finish pass; 32 µin (0.8 µm) fine; 16 µin (0.4 µm) achievable
- **Typical volumes**: 1–1,000 parts typical; economical to roughly 10,000 depending on cycle time
- **Lead time**: 3–10 business days for prototypes; 2–4 weeks for production quantities

## Overview

CNC milling removes material from solid stock with a rotating multi-flute cutter driven along programmed toolpaths, producing prismatic parts with flat faces, pockets, slots, holes and 3D contours. It is the default process for functional metal and plastic parts in quantities of one to a few thousand, and the only one that goes from CAD model to finished part in aluminum, steel, stainless, titanium or engineering plastics with no tooling at all.

A 3-axis machining center holds **±0.005 in (±0.13 mm)** as a routine shop standard and **±0.001 in (±0.025 mm)** where the drawing calls for it. Surfaces come off the machine near 125 µin Ra (3.2 µm) and can be finished to 32 µin (0.8 µm).

The constraints are geometric rather than material: every feature must be reachable by a rotating tool of finite diameter and finite length, which is why internal vertical corners are always radiused and deep narrow pockets cost more than shallow wide ones.

## How it works

1. **CAM programming.** The solid model is imported, stock defined, and toolpaths generated against a tool library, work offsets and cutting parameters. Programming is real cost on a one-off part and near zero amortized across a run.
2. **Workholding and setup.** The blank is clamped in a vise, on soft jaws, or in a dedicated fixture. Each face that must be machined is a *setup*, and every setup after the first re-establishes datums — budget roughly 0.002–0.005 in (0.05–0.13 mm) of positional stack-up between features cut in different setups.
3. **Zeroing.** An edge finder or touch probe sets the part origin and each tool's length offset is measured. On probed machines this takes seconds; done manually, minutes per tool.
4. **Roughing.** Bulk material comes off with adaptive or trochoidal paths using a small radial engagement — roughly 5–15% of cutter diameter — at full axial depth, keeping chip load constant and tool temperature down. Roughing leaves 0.010–0.020 in (0.25–0.50 mm) of stock on finished surfaces.
5. **Finish passes.** Radial depths of 0.002–0.010 in (0.05–0.25 mm) remove the roughing stock and set final tolerance and finish. This is where the tolerance on the drawing turns into cycle time.
6. **Hole making.** Drilling to standard sizes, peck cycles beyond about 4× diameter of depth, reaming or boring where the ID tolerance is tighter than a drill can hold, and tapping or thread milling.
7. **Deburring and inspection.** Brush or manual deburring, then calipers and gage pins for open tolerances and a CMM for GD&T callouts.

Typical carbide surface speeds show where the hours go: aluminum runs at 500–1,000 SFM (150–300 m/min), carbon and alloy steel at 250–450 SFM (75–140 m/min), 304/316 stainless at 150–300 SFM (45–90 m/min), and Ti-6Al-4V at 100–200 SFM (30–60 m/min). Titanium is not difficult to cut so much as slow to cut, and the machine bills by the hour.

## Design guidelines

### Internal corner radii
A rotating tool cannot cut a sharp internal vertical corner. Specify a corner radius of at least **1/3 the pocket depth**, and make it slightly larger than a standard tool radius — 0.135 in rather than 0.125 in for a 1/4 in cutter — because a corner matching the tool exactly wraps the cutter in full engagement and chatters.

### Pocket depth and tool reach
Keep pocket depth under **4× the diameter of the tool the geometry forces you to use**. Reduced-neck and long-reach tooling extends that to roughly 6–10× at lower feed rates, since deflection grows with the cube of overhang. Allow **0.020 in (0.5 mm)** of floor radius unless a sharp floor is functionally required.

### Wall thickness
Minimum **0.030 in (0.76 mm)** in metal and **0.060 in (1.5 mm)** in plastic; 0.060 in and 0.125 in (3 mm) respectively are the thicknesses that machine cleanly. Keep unsupported wall height under roughly 10× wall thickness.

### Holes and threads
Design around stocked drill sizes rather than arbitrary diameters ([drill size chart](/charts/drill-size-chart)). Standard hole depth is 4× diameter; deeper needs peck cycles or through-coolant tooling. Threads need only **1× diameter of full thread in steel and 1.5–2× in aluminum and plastics** — 3× adds tapping time and tap-breakage risk without adding strength ([tap drill chart](/charts/tap-drill-chart)).

### Tolerances and datums
Default the drawing to ISO 2768-m and tighten only the dimensions carrying a fit or an interface. Put bearing bores, dowel holes and shaft fits on an [ISO 286 fit class](/charts/iso-286-fits-tolerances), and express position and orientation with [GD&T callouts](/charts/gdt-symbols) rather than chained ± dimensions.

### Surface finish
125 µin Ra (3.2 µm) as-machined, 63 µin (1.6 µm) with a finish pass, 32 µin (0.8 µm) fine, and 16 µin (0.4 µm) achievable with light passes; smoother than that belongs to grinding ([surface finish chart](/charts/surface-finish-chart)).

| Material | Machinability | Watch for |
|---|---|---|
| 6061 / 7075 aluminum | Excellent | Highest removal rates, lowest cost per part |
| Brass C360 | Excellent | Free-cutting, holds fine detail |
| 1018 / 4140 steel | Good | Heavier cutting forces, slower than aluminum |
| 303 / 304 / 316 stainless | Moderate | Work hardens; constant feed, no dwelling |
| Ti-6Al-4V | Difficult | Low speed, high heat, flood coolant |
| Inconel 718 | Difficult | Rapid tool wear drives cost per part |
| Acetal, PEEK | Excellent | Dimensionally stable, clean chips |
| ABS / polycarbonate | Moderate | Melts and smears; single-flute tools, air blast |
| Carbon fiber / G10 | Abrasive | Diamond tooling and dust extraction |

| Feature | Recommended | Limit | Why |
|---|---|---|---|
| Internal corner radius | ≥ 1/3 pocket depth | Tool radius | Round tools cut round corners |
| Pocket depth | ≤ 4× tool diameter | ~10× long-reach | Deflection and chatter |
| Wall thickness, metal | 0.060 in (1.5 mm) | 0.030 in (0.76 mm) | Walls deflect under cutting load |
| Wall thickness, plastic | 0.125 in (3 mm) | 0.060 in (1.5 mm) | Low stiffness, heat softening |
| Hole depth | ≤ 4× diameter | ~10× with pecking | Chip evacuation |
| Thread depth | 1–2× diameter | 3× diameter | Extra engagement adds no strength |
| Engraved detail | ≥ 0.020 in (0.5 mm) | Smallest stocked cutter | Small tools break and run slowly |

## Cost drivers

Cost is machine hours plus setup plus material, and machine hours are set by how much metal comes off and how well finished the part must be when cutting stops.

**Setups dominate at low volume.** Each reorientation adds fixturing, offsets, programming and inspection. Going from three setups to two usually saves more than loosening a tolerance.

**Removed volume drives cycle time.** A part machined from a 4 × 4 × 2 in block that finishes at 15% of the blank weight spends most of its cycle roughing; buy stock close to the finished envelope.

**Tolerance and finish are multipliers.** Moving from ±0.005 in to ±0.001 in means slower finish passes, in-process probing, controlled inspection and higher scrap risk. Across twenty dimensions it can double the price.

**Tooling and volume.** Cutters under 1/8 in (3 mm), long-reach tools and custom form tools run slowly and break. Programming and first-article inspection are one-time charges — noise at 50 parts, most of the invoice at one.

Five ways to take cost out:

1. Use one internal corner radius throughout so a single cutter finishes the part.
2. Keep every pocket shallower than 4× the diameter of the tool it forces.
3. Pick holes and threads from the [drill size chart](/charts/drill-size-chart) and [tap drill chart](/charts/tap-drill-chart).
4. Leave the drawing at ISO 2768-m and tighten only the interfaces that matter.
5. If the part truly needs four or more machined faces, quote it as [5-axis](/processes/cutting/5-axis-cnc-machining) — one setup often beats three cheaper ones.

## FAQ

### What tolerance can CNC milling hold?

±0.005 in (±0.13 mm) is the routine shop standard and costs nothing extra, ±0.001 in (±0.025 mm) is normal work on selected features, and ±0.0005 in (±0.013 mm) is achievable with finish passes, probing and controlled inspection conditions. Allow an extra 0.002–0.005 in (0.05–0.13 mm) of stack-up between features cut in different setups.

### What is the minimum wall thickness for CNC milling?

0.030 in (0.76 mm) in metal and 0.060 in (1.5 mm) in plastic are workable minimums, but 0.060 in (1.5 mm) and 0.125 in (3 mm) machine cleanly without chatter. Keep unsupported wall height under about 10× the wall thickness — deflection under cutting load, not strength, is what limits thin walls.

### Why do CNC milled parts always have rounded internal corners?

The cutter is round, so the corner it leaves is round, with a radius equal to the tool radius. A tool small enough for a tiny radius is also short and slow. Specify a corner radius of at least one third of the pocket depth and reuse the same radius throughout so one tool can finish the part.

### How deep can a CNC milled pocket be?

About 4× the cutter diameter with standard tooling, extending to roughly 6–10× with reduced-neck and long-reach tools at reduced feed rates, because deflection grows with the cube of tool overhang. Deeper features are better handled by machining from both sides or by sinker EDM.

### What surface finish does CNC milling produce?

About 125 µin Ra (3.2 µm) as-machined. A dedicated finish pass reaches 63 µin (1.6 µm), fine finishing 32 µin (0.8 µm), and 16 µin (0.4 µm) is achievable with light passes and sharp tooling. Below that, grinding or polishing is the appropriate process.

### What materials can be CNC milled?

Aluminum, brass, copper, carbon and alloy steel, stainless, titanium, Inconel, magnesium and most engineering plastics. Machinability rather than possibility decides cost: aluminum runs at 500–1,000 SFM (150–300 m/min) while Ti-6Al-4V runs at 100–200 SFM (30–60 m/min), so the titanium version of the same part occupies the machine far longer.

## Alternative processes

- [Die Casting](https://manufacturingprocesses.org/processes/forming/die-casting.md): Die casting injects molten aluminum, zinc or magnesium into a hardened steel die under high pressure, producing thin-walled net-shape metal parts.
- [Investment Casting](https://manufacturingprocesses.org/processes/forming/investment-casting.md): Investment casting builds a ceramic shell around a wax pattern, melts the wax out and pours metal into the cavity, giving fine detail in almost any alloy.
- [Metal Injection Molding](https://manufacturingprocesses.org/processes/forming/metal-injection-molding.md): Metal injection molding molds a powder-and-binder feedstock exactly like a plastic, then debinds and sinters it into a dense small metal part.
- [Direct Metal Laser Sintering (DMLS)](https://manufacturingprocesses.org/processes/forming/direct-metal-laser-sintering-dmls.md): Direct metal laser sintering fuses metal powder layer by layer with a laser, building dense metal parts anchored to a supported build plate.
- [Sheet Metal Fabrication](https://manufacturingprocesses.org/processes/forming/sheet-metal-fabrication.md): Sheet metal fabrication cuts, bends and joins flat stock into a finished assembly, typically laser cutting followed by press braking, hardware and welding.

## Related processes

- [CNC Turning](https://manufacturingprocesses.org/processes/cutting/cnc-turning.md): CNC turning rotates the workpiece against a stationary tool, producing round parts with excellent concentricity and short cycle times.
- [5-Axis CNC Machining](https://manufacturingprocesses.org/processes/cutting/5-axis-cnc-machining.md): 5-axis CNC machining tilts and rotates the part or the head so the tool reaches every face and stays short and rigid on complex surfaces.
- [CNC Machining](https://manufacturingprocesses.org/processes/cutting/cnc-machining.md): CNC machining removes material from solid stock with a programmed cutting tool, producing accurate parts directly from a CAD model with no tooling.
- [Swiss Screw Machining](https://manufacturingprocesses.org/processes/cutting/swiss-screw-machining.md): Swiss screw machining feeds bar stock through a guide bushing so cutting happens right next to the support, holding tight tolerances on slender parts.
- [Electrical Discharge Machining](https://manufacturingprocesses.org/processes/cutting/electrical-discharge-machining.md): EDM erodes conductive metal with controlled electrical sparks across a dielectric gap, cutting hardened material and sharp internal corners.

---

*Source: [Manufacturing Processes](https://manufacturingprocesses.org/processes/cutting/cnc-milling)*

*Last updated: August 11, 2026*