CNC Milling: Precision Metal Cutting Explained

• 1
  What CNC milling precision metal cutting does at the edge
• 2
  Where the last 0.01 mm of precision metal cutting comes from
• 3
  How the workpiece metal changes the cut
• 4
  Features that decide whether milling is the right process
• 5
  Three-axis, four-axis, or five-axis milling

A CNC mill holds the workpiece and spins a multi-tooth cutter. Each flute takes a small bite, called chip load, and shears metal away. The control moves the tool along a programmed path, so the shape comes from motion rather than from a form tool. That is the core idea behind CNC milling precision metal cutting: the machine repeats a path, and the path decides geometry.

Chip load is the number that matters most. It is feed per tooth, not feed per revolution. A 10 mm three-flute carbide end mill running at 3,000 rpm and 900 mm/min feed takes 0.10 mm per tooth. Drop to 0.02 mm per tooth and the tool rubs instead of cutting. Heat goes into the edge, the edge wears, and the surface turns smeared.

Cutting speed is set by the material, not by the operator's mood. Aluminium 6061 runs fast, often 300–600 m/min surface speed with carbide. Stainless 316 and 17-4PH run far slower, commonly 60–120 m/min, because they work-harden at the cut. Titanium TC4 sits lower still. Spindle speed follows from surface speed divided by tool diameter.

Radial and axial depth of cut control how much of the flute is engaged. Full-width cuts in a slot load the tool heavily and push deflection up. Trochoidal paths take 5–10% radial engagement at higher feed, which keeps radial cutting forces low and lets the same cutter clear a deep pocket without chatter.

Climb milling is the default on modern machines. The cutter tooth enters at maximum chip thickness and exits at zero, which pushes the workpiece away from the tool and reduces rubbing. Conventional milling still has a place on rough castings with hard surface scale, where the entry shock would chip a carbide edge.

• 1
  Chip loadFeed per tooth. Too low rubs, too high breaks edges.
• 2
  Surface speedSet by material: aluminium fast, stainless and titanium slow.
• 3
  EngagementRadial and axial depth decide cutting force and chatter risk.
• 4
  Climb millingStandard for finish passes on clean stock.

Machine accuracy is only the starting point. A machine that positions to ±0.005 mm still produces a bad part if the setup moves. Thermal growth is the usual suspect. A spindle running for two hours grows, and a 100 mm aluminium part can shift several micrometres between the first and last cut. Shops that hold tight tolerances warm up spindles and cut in a temperature-controlled bay.

Tool deflection is the second cause. A long, thin end mill bends under side load. Deflection scales with the cube of length over diameter, so a cutter hanging 60 mm out of a 6 mm collet is roughly 1,000 times more flexible than the same cutter held short. Reach into a deep pocket and you buy reach with accuracy.

Clamping is the third. Vise jaws, soft jaws, and fixture plates all distort thin parts. A 3 mm wall clamped at 4,000 N will spring back when released, and the measured part no longer matches the cut part. Light clamping, support under the cut, and stress-relieved stock are the standard countermeasures.

Tolerance stack-up is the fourth. A ±0.05 mm position tolerance on a hole, a ±0.05 mm datum shift, and a ±0.02 mm perpendicularity error combine. The hole can sit 0.12 mm from nominal in the worst case. Engineers who specify each callout independently often find the assembly will not close even though every individual feature passed inspection.

• 1
  Thermal driftWarm up spindles and control the room temperature.
• 2
  Tool deflectionKeep length-to-diameter ratio low; use stub cutters.
• 3
  Clamping distortionThin walls spring back after the vise opens.
• 4
  Stack-upIndependent callouts can still miss the assembly.

Aluminium 6061 and 7075 cut freely and hold good finish. 7075 is stronger and machines almost as well, though it is more prone to distortion in thin sections. 2024 is tougher and more corrosion-sensitive, so it usually needs anodizing. Cast aluminium ADC12 machines well but can hide porosity that only shows after the skin is removed.

Stainless 303 is the free-machining grade and the easiest of the 300 series. 304 and 316 work-harden quickly. Light passes with a sharp edge and a steady feed keep the cut under the hardened layer. 17-4PH in the H900 condition is hard enough to demand carbide and rigid setups; in the annealed condition it cuts closer to 304.

Titanium TC4, also written Ti-6Al-4V, has low thermal conductivity. Heat stays at the edge instead of leaving with the chip. Cutting speeds drop to roughly 40–70 m/min, coolant flow has to be generous, and tool life becomes the cost driver. Inconel is worse on every axis and is priced accordingly.

Plastics behave differently again. POM and ABS cut cleanly with sharp two-flute cutters and high spindle speed. PEEK needs slower feeds to avoid melting. Carbon fibre is abrasive and wears carbide quickly, so diamond-coated tooling pays for itself on any real volume.

• 1
  Aluminium 6061/7075Fast, clean, low risk in thin walls.
• 2
  Stainless 304/316Work-hardens; light passes with steady feed.
• 3
  Titanium TC4Heat stays at the edge; tool life drives cost.
• 4
  Carbon fibreAbrasive; diamond coating extends tool life.

Milling wins on prismatic parts: flat faces, pockets, bosses, slots, drilled and tapped holes, and contoured surfaces. It handles one-off prototypes and 10,000-piece runs on the same machine, which is unusual among metal processes. Setup cost dominates at low volume; cycle time dominates at high volume.

A pocket depth over four times its width needs a long cutter, and long cutters deflect. Either the corner radius grows or the shop has to rough with a bigger tool and finish with a smaller one. Corner radii less than one third of the pocket depth are the single most common cost driver in a milling quote.

Thin walls below 0.8 mm are machinable but risky. Vibration, clamping spring-back, and heat all work against the wall. Adding a rib, thickening temporarily, or leaving stock for a finish pass all help. If the wall is functional at 0.5 mm, expect the shop to rough it thick and step down in small increments.

Sharp internal corners cannot be milled. Every cutter has a radius, so the corner inherits it. If the drawing calls a true sharp corner, the part goes to EDM or the design changes. Calling out the radius explicitly saves a round of questions.

Holes deeper than ten times the diameter are usually drilled rather than milled, then reamed or bored if the tolerance is tight. Milling a deep hole with a small end mill is slow and prone to taper.

• 1
  Pocket depthKeep under 4× the cutter width where possible.
• 2
  Corner radiusMatch it to a standard cutter; sharp corners need EDM.
• 3
  Thin wallsBelow 0.8 mm, add ribs or plan for multiple passes.
• 4
  Deep holesDrill first, then ream or bore to tolerance.