CNC Milling Machining Guide

• 1
  How CNC milling removes metal
• 2
  Fixtures and workholding decide the tolerance
• 3
  Material behavior that changes the cut
• 4
  What tolerance is realistic on a mill
• 5
  Design details that keep milling cheap
• 6
  When milling is not the right process
• 7
  3-axis vs 4-axis vs 5-axis: when each wins

A milling cutter is a multi-tooth tool that spins while the workpiece feeds past it. Each insert or flute takes a small chip. Heat leaves with the chip, not into the part, which is why milling can run dry on many aluminum jobs. The geometry of the cut, not the spindle speed alone, decides whether the tool survives.

Cutting speed and feed per tooth set the chip load. On 6061 aluminum, a 12 mm carbide end mill often runs at 300–500 m/min surface speed with 0.05–0.15 mm per tooth. Drop to 30–60 m/min on 316 stainless and the same tool needs a smaller chip load and more coolant. Push either past the limit and you get chatter, not a good finish.

Radial and axial engagement matter more than most drawings suggest. A cutter taking 5% of its diameter radially can run much faster than one buried at 50%. The load per tooth stays stable; the arc of contact shrinks. Programmers exploit this with trochoidal paths and high-feed cutters, which spread the cut over a longer edge.

Climb milling is the default on modern machines. The cutter tooth enters at maximum chip thickness and exits at zero, which pushes the part into the fixture and leaves a cleaner wall. Conventional milling does the opposite and tends to rub, work-harden stainless, and lift thin parts. Only use it for rough castings with hard skin.

• 1
  Chip loadSet by feed per tooth; the real limit on tool life.
• 2
  EngagementLower radial depth lets you raise speed.
• 3
  Climb millingStandard choice; better finish and tool life.

The machine is rarely the weak link. A 3-axis mill with a good vise holds ±0.02 mm all day. The same machine with a part clamped on one corner will flex, vibrate, and drift. Workholding stiffness sits between the cutter and the part, so any movement shows up in the wall.

For thin walls, support the part from both sides or leave sacrificial ribs. A 1.5 mm aluminum wall will deflect under a 10 mm cutter even at light load. Rough with the wall at 3 mm, then finish to 1.5 mm with a smaller tool and a spring pass. The spring pass takes 0.05 mm with no feed change and removes the deflection left from the previous pass.

Soft jaws machined to the part profile beat a standard vise for anything with a curved or angled face. For a batch of 50 parts, soft jaws add setup time once and remove it fifty times. Vacuum plates work for flat, non-porous plates but lose grip on small features. Magnetic chucks hold steel well and do nothing for aluminum.

Five-axis machines reduce the number of setups. One rotary table with a Ø400 mm face lets a part be reached from five sides without unclamping. Each re-clamp adds position error of 0.01–0.03 mm. On a part with six tight bores, that error stacks. On a simple bracket, it does not matter.

• 1
  Soft jawsMachined to profile; worth it above 20 parts.
• 2
  Thin wallsRough thick, finish with light spring passes.
• 3
  Re-clampingEach setup adds 0.01–0.03 mm position error.

Aluminum 6061 machines fast and holds a good finish. 7075 is stronger but gummier; it needs sharper tools and more coolant to stop built-up edge. 2024 tends to warp after machining because of internal stress, so rough it, stress-relieve, then finish. On thin 2024 ribs, expect 0.05–0.1 mm of movement after unclamping.

Stainless 316 work-hardens the moment a tool rubs. Keep the cutter engaged, never dwell, and never let a dull tool skim. 17-4PH in the H900 condition cuts more like a tool steel than a stainless; use carbide with a coating and reduce surface speed to 40–60 m/min. 303 is the free-machining grade and is the right choice when corrosion demand allows it.

Titanium Ti-6Al-4V (TC4) has low thermal conductivity, so heat stays at the edge. Use high-pressure coolant, 30–50 m/min, and a sharp uncoated or AlTiN-coated carbide. Inconel is slower still: 20–30 m/min with ceramic inserts for roughing. Both materials punish any lack of rigidity.

Plastics behave differently. POM and PEEK cut cleanly with sharp two-flute tools and air blast; coolant can cause stress cracking in some grades. ABS and PC melt if the chip cannot clear. Carbon fiber is abrasive and needs diamond-coated tooling plus dust extraction. None of these are hard to mill once the tool and feed are matched.

• 1
  7075 aluminumHigher strength, gummier; watch built-up edge.
• 2
  316 stainlessNever rub; keep the cutter engaged.
• 3
  Ti-6Al-4VLow speed, high-pressure coolant, sharp edge.
• 4
  Carbon fiberDiamond coating and dust extraction.

The shop floor number to remember is ±0.005 mm. That is what a well-set 5-axis machine holds on a feature that is reachable and rigid. It is not a blanket tolerance for every dimension on the drawing. A 300 mm long aluminum part will move with temperature; 1 °C of change is about 0.007 mm over that length.

General machining tolerance is often ±0.05 mm. Tighten only the features that need it. Every tightened dimension adds inspection time, a possible gauge, and a chance of scrap. On a bracket with 40 dimensions, calling out five as ±0.01 mm and leaving the rest at ±0.1 mm keeps the part affordable.

Surface finish follows the same logic. As-machined is Ra 1.6–3.2 μm. A fine finish of Ra 0.2–0.8 μm needs a smaller stepover, a sharper tool, and sometimes a finishing pass with a ball nose. That adds cycle time. If the drawing only needs a sealing face to be smooth, say so on that face.

Position tolerance matters more than size tolerance for assemblies. A bolt hole at the right diameter but 0.1 mm off position will not fit. True position of 0.05 mm is routine on one setup. Across three setups, expect 0.1 mm or plan a reamed dowel hole to locate the part.

• 1
  Achievable±0.005 mm on rigid, reachable features.
• 2
  General±0.05 mm covers most non-critical work.
• 3
  Thermal driftAbout 0.007 mm per 300 mm per °C.

Cutters are round, so inside corners are round. A 6 mm end mill leaves a 3 mm corner radius. Drawing a sharp internal corner forces a smaller tool, more passes, and sometimes EDM. Set corner radii to at least one-third of the pocket depth and use a standard cutter size.

Deep pockets are where cost climbs. A pocket 5× deeper than its width needs a long, thin tool that deflects and chatters. If you can, open the pocket to the side or split it into two shallower features. A 40 mm deep, 8 mm wide slot in aluminum is a slow job on any machine.

Text and logos are fine as long as the character height is at least 1.5 mm. Below that, the tool cannot reach and the mark smears. Engrave on a flat face, not a curved one, unless you accept variable depth. Laser marking handles the same limit and leaves no burr.

Threads cut with a mill or a tap are both normal. A tapped M3 hole needs 2.5 mm of full thread engagement minimum. On a blind hole, leave a thread relief so the tap does not bottom and break. For threads larger than M12, milling the thread is often faster than tapping on a 3-axis machine.

• 1
  Corner radiiAt least 1/3 of pocket depth.
• 2
  Pocket depthKeep under 5× tool diameter where possible.
• 3
  Engraving1.5 mm minimum character height.

Milling is a subtractive process, so deep internal channels and complex cooling passages are hard to reach. A conformal cooling channel inside a mold insert usually goes to metal 3D printing or casting. If the channel is straight and open at both ends, a drilled hole works and costs far less.

Very high volumes favor casting or forging. A 10,000 piece run of a simple bracket is cheaper as a die casting with a finish pass on the critical faces. Milling the whole geometry wastes material and machine time. The break-even sits around a few hundred to a few thousand parts, depending on geometry.

Parts that are mostly flat and thin belong to sheet metal. A 1 mm steel panel with bent edges and punched holes is a stamping or laser job, not a milling job. Milling it would take many passes to remove material that was never needed.

Very large parts are possible up to 4,000 mm, but the machine envelope is 4,000 × 400 × 150 mm for the long-travel configuration. Check that your part fits the actual travel, not just the maximum size. A 3,900 mm part with a feature at each end may need two setups.

• 1
  Internal channelsUse additive or casting instead.
• 2
  High volumeCasting wins above a few thousand parts.
• 3
  Thin sheetSheet metal fabrication is faster and cheaper.