CNC Milling
Also: milling, 3-axis milling, vertical machining, VMC machining, CNC mill, machining center, HMC machining
CNC milling cuts pockets, holes, bosses and contours into plate and billet with rotating cutters on 3- and 4-axis machining centers, in any machinable material.
5,104 CNC machining companies in the Noramark directory
In milling the tool spins and the part stays put. The workpiece is clamped in a vise or on a fixture; the table moves in X and Y and the spindle in Z, and an automatic tool changer swaps between end mills, drills, taps, reamers and boring bars as the program calls for them. A fourth axis (rotary table or trunnion) indexes the part so several faces can be reached without re-clamping. Most job-shop milling runs on vertical machining centers (VMCs); horizontal machining centers with pallet changers take over for production, because chips fall clear and a rotary B-axis exposes four faces per load.
Milling is the workhorse for prismatic parts: plates, brackets, housings, manifolds, fixtures, enclosures and mold bases. Shops hold ±0.13 mm (±0.005") as a matter of course and ±0.025 mm (±0.001") on features the drawing calls out; reamed or bored holes hold ±0.013 mm (±0.0005"). Walls and floors come off at 1.6-3.2 µm Ra (63-125 µin), and a light finishing pass with a fresh tool brings that to 0.8 µm Ra (32 µin).
The limit is reach. A 3-axis mill cuts only what a vertical tool can see from above, so every additional face means another setup, and every setup adds handling and a tolerance stack. Internal corners carry the radius of the tool, deep pockets need long tools that chatter and taper, and thin floors and walls spring away from the cut. Parts with features on five faces, compound angles or contoured surfaces move to 5-axis machining; round parts belong on a lathe.
At a glance
| Typical tolerances | Standard ±0.13 mm (±0.005") on dimensions; ±0.025 mm (±0.001") with care on called-out features; reamed and bored holes to ±0.013 mm (±0.0005"). True position of ±0.05 mm (±0.002") between features cut in one setup and roughly double that across a flip. Flatness of 0.05 mm (0.002") over 300 mm on plates cut from stress-relieved or cast tooling plate; rolled 6061 plate moves when one face is milled away. |
|---|---|
| Size limits | A typical VMC has 760-1,000 mm (30-40") of X travel, 500 mm (20") of Y and 500 mm (20") of Z, with 500-1,000 kg on the table; large-format and bridge mills at fewer shops run to 3,000-6,000 mm (10-20 ft). End mills under 1 mm (0.040") exist but cut slowly and break easily; features under 0.5 mm (0.020") belong at a micro-machining shop. |
| Surface finish | As-milled 1.6-3.2 µm Ra (63-125 µin) on walls and floors; 0.8 µm Ra (32 µin) with a finishing pass and a fresh tool; face-milled tops reach 0.4-0.8 µm Ra (16-32 µin) with a wiper insert. Ball-nose finishing on contoured surfaces leaves cusps that show unless the stepover is small, which costs machine time; bead blasting, blending or polishing hides tool marks on visible surfaces. |
| Lead time | Prototypes in 3-7 business days, sometimes overnight for a simple aluminum plate; production in 2-5 weeks. Tooling plate and common bar are stocked; odd plate thicknesses in stainless or tool steel can add a week. |
Typical of U.S. job shops; confirm with the shop for your part.
Materials
Aluminum is the natural fit: 6061 and 7075 bar and plate, and MIC-6 cast tooling plate when flatness matters. Mild and alloy steel (1018, 4140, pre-hard 4140 at 28-32 HRC), stainless (303, 304, 316, 17-4 PH), pre-hardened tool steel up to about 45 HRC, brass and copper, and titanium all mill well with the right tooling and speeds. Hardened steel above 50 HRC is hard-milled with carbide or ceramic tools on small features and ground or EDM-cut for the rest. Engineering plastics (Delrin, nylon, PEEK, polycarbonate, UHMW) mill easily but move with heat and clamping pressure, so they need sharp tools, light clamping and looser tolerances.
What drives the cost
- Machine time: how much material comes off, how fast the material cuts, and the tool paths the geometry allows
- Number of setups: every face that needs a flip adds fixturing, handling and a tolerance stack
- Small internal radii, deep narrow pockets and thin floors that force small tools at low feed
- Tolerances below ±0.05 mm (±0.002") and finishes below 0.8 µm Ra, which add finishing passes and inspection time
- Quantity: programming and first-piece setup are amortized across the run
- Material: 7075 plate, stainless and pre-hard tool steel cost more to buy and more to cut than 6061
- Secondaries: deburring, anodizing, plating, heat treatment and inspection reports
When to use it
- Plates, brackets, housings, manifolds, fixtures and enclosures with features mainly on one or two faces
- Prototypes and production runs from one piece to a few thousand
- Flat, square and parallel datums and hole patterns held to ±0.05 mm (±0.002")
- Finishing the mounting faces and bores of castings, weldments and extrusions
- Pockets, slots and 2D profiles in aluminum and plastic plate
When not to
- Round, shaft-like parts: turning is faster and holds diameters better
- Parts with features on five or six faces, compound angles or contoured surfaces: 5-axis machining does them in one setup
- Thin sheet parts: laser cutting and bending waste far less material and time
- Volumes above a few thousand of a simple shape: die casting, stamping or molding will be cheaper per part
Design tips
- Give internal corners a radius larger than a third of the pocket depth and never smaller than 1 mm (0.040"), so a stiff standard end mill can cut them.
- Keep pocket depth under four times the tool diameter, and under three in hard materials; deeper pockets need long tools that chatter and leave taper.
- Expect a small radius where a wall meets a floor; ask for a sharp corner only where a mating part demands it.
- Put features on as few faces as possible and give the part a flat bottom and parallel sides: a vise is free fixturing.
- Use standard hole sizes and thread depths; a thread deeper than 1.5 times its diameter adds no strength and risks broken taps.
- Call out flatness and parallelism on plates explicitly, and specify MIC-6 or stress-relieved plate when they matter.
- Set datums to match how the part will be held, and tolerance across a flip more loosely than within one setup.
Frequently asked questions
- What is the difference between CNC milling and CNC machining?
- Machining is the umbrella term; milling is one of its operations. In milling the tool spins and the part is fixed, which suits prismatic parts. In turning the part spins, which suits round parts. When a shop says "milling" it usually means 3-axis work on a vertical machining center.
- What tolerances can CNC milling hold?
- Any competent shop holds ±0.13 mm (±0.005") without being asked, ±0.025 mm (±0.001") on called-out features and ±0.013 mm (±0.0005") on reamed or bored holes. Across a second setup expect the tolerance to roughly double unless the shop uses a qualified fixture.
- How deep can a CNC mill cut a pocket?
- Three to four times the tool diameter is comfortable. Long-reach tools go to eight or ten times at slower feeds and with a worse wall finish and some taper. Deeper narrow cavities are better made by sinker EDM or by splitting the part.
- 3-axis or 5-axis milling?
- 3-axis is cheaper per hour and accurate enough for parts with features on one or two faces. Move to 5-axis when features sit on three or more faces, at compound angles, or on contoured surfaces; a 3+2 positional setup gives most of the benefit at a modest premium.
