CNC Mill Guide: How Milling Actually Cuts Metal

• 1
  Key takeaways
• 2
  What Happens Where the Tool Meets the Part
• 3
  Axis Count: What Each Configuration Buys You
• 4
  Spindle, Toolholding and Workholding Limits
• 5
  Tolerance, Finish and What Drives Cost
• 6
  Matching the Part to the Process

A CNC mill removes material with a rotating multi-flute tool while the workpiece stays clamped to a bed. The tool moves in X, Y and Z, and the table or the head carries the feed. Every flute takes a chip, releases it, and re-enters. That interrupted contact is the defining trait of milling. It shapes everything downstream: tool life, surface finish, chatter risk and how much stock you can leave for a finishing pass.

Chip thickness is set by feed per tooth, not by spindle speed alone. If you double the speed but keep the same feed per tooth, the cutter is still taking the same chip, so the load on the edge stays similar while heat per minute goes up. This is why feed and speed are always quoted as a pair. A 12 mm 3-flute carbide end mill in 6061-T6 might run at 0.05 mm per tooth and 6,000 rpm, while the same cutter in 316 stainless drops to roughly 0.03 mm per tooth and half the speed.

Climb milling, where the cutter engages the thickest part of the chip first, is the default on machines with ball screws and low backlash. It pulls the work into the cutter and leaves a cleaner wall. Conventional milling still has a place on older machines with worn lead screws, on castings with hard surface scale, and on finishing passes where you want to avoid rubbing. The choice shows up directly in the wall finish and in how long the insert lasts.

Built-up edge is the failure mode most people misread. In soft aluminum and low-carbon steel, material welds onto the cutting edge and then breaks away, taking tool coating with it. The finish looks smeared and the dimensions drift. Raising surface speed, adding a lubricating coolant, or switching to a sharper polished insert usually clears it. If the smearing returns on every part, the problem is more likely the tool geometry than the cutting data.

• 1
  Interrupted cutEach flute loads and unloads once per revolution, so impact resistance matters.
• 2
  Feed per toothChip thickness is set by feed and tooth count, not rpm alone.
• 3
  Climb millingDefault on low-backlash machines; better wall finish and tool life.
• 4
  Built-up edgeWelded material smears the finish; fix speed or geometry, not just coolant.

A 3-axis mill moves the tool in X, Y and Z. The part sits in one orientation and the operator re-fixtures it for any face that is not reachable from the top. That is not a flaw, it is a cost model. For a flat bracket with holes on one face plus a couple of edges, 3-axis work on a machine with 750 × 1,150 × 550 mm travel is often the cheapest path, because setup time is short and the tooling is simple.

A 4-axis mill adds rotation around one axis, usually the X or Y. The common case is a part with features on four sides of a prismatic block: the rotary table indexes 90 degrees between operations and one setup covers all four faces. Positional 4-axis work holds true position well because the part never leaves the fixture. What it does not do is machine a compound angle while cutting.

A 5-axis mill adds a second rotary axis, and the two rotaries let the tool approach the part from an arbitrary direction. There are two families. Table-table machines tilt and rotate the workpiece; head-head machines move the spindle. In both cases the payoff is the same: undercut regions, deep pockets with drafted walls, and port geometries that would need three or four separate fixtures on a 3-axis machine. The trade is that programming and verification take longer, and the machine needs a rigid setup to hold position at the extremes of travel.

GreatLight runs 16 simultaneous 5-axis machining centers, 12 four-axis mills, 27 three-axis machines and 16 mill-turn centers, with 4,000 mm maximum processing size. That mix matters when quoting. We place a part on the machine that finishes it in the fewest setups, not on the largest machine available. A part that fits a 500 × 500 × 450 mm envelope rarely benefits from being moved to a large-travel machine, and the fixture cost tells you so quickly.

• 1
  3-axisOne orientation per setup; lowest fixture cost for prismatic parts.
• 2
  4-axisIndexing around one axis; four faces in a single setup.
• 3
  5-axisContinuous multi-directional cutting; undercuts and drafted pockets.
• 4
  Mill-turnRotational and prismatic features without re-chucking.

The spindle is the stiffest link or the weakest one, depending on how you use it. A CAT40 or HSK-A63 taper with a short gauge-length holder puts the cutting edge close to the bearings, where rigidity is highest. Add a 150 mm extension and you have built a tuning fork. Deep cavities and tall bosses usually force that extension, and the result is chatter that no feed override can fix. If a design needs a long reach, the pocket depth and corner radius should be chosen with that in mind.

Toolholding runout drives dimensional spread on hole features. A holder with 0.02 mm runout cuts a hole larger on one side, and a reamer follows the same error. For holes held to ±0.005 mm, we measure runout before the run and change holders rather than compensate in the program. That is a shop-floor decision, not a CAM setting.

Workholding is where most first-article problems start. A vise with 2 mm of parallel lift can tilt a plate enough to break a flatness callout. Thin plates need support underneath, not just clamping force from the side. Vacuum plates and fixture plates with drilled and tapped grids handle thin, flat parts far better than a two-jaw vise. For a part that will be machined on five faces, we often leave a tab or boss that the second operation removes.

Material behavior sets the practical limits. Aluminum 6061 and 7075 cut freely and hold thin walls reasonably well. Titanium Ti-6Al-4V and Inconel heat the edge instead of the chip, so speeds drop and tool life shortens. Plastics such as POM and PEEK need sharp, polished tools and generous coolant to stop melting and burring. Stainless 316L work-hardens under a rubbing cut, so a light pass with a dull tool is worse than a heavier pass with a fresh one.

• 1
  Keep it shortGauge length is the biggest single lever on rigidity.
• 2
  Measure runoutCheck holder TIR before hole-critical operations, not after.
• 3
  Support thin partsVacuum or fixture plates beat side clamping for flatness.
• 4
  Match materialTitanium and stainless punish the wrong speed far more than aluminum.

Tolerance is not a single number for a part. It is a set of feature-level requirements, and each one has a different cost. A bore held to ±0.005 mm may need a boring operation or a reamer after milling. A pocket floor at the same tolerance may need a finishing pass with a small stepover and a fresh insert. The part drawing that puts ±0.005 mm on everything is usually telling us the designer has not decided which features actually matter.

Surface finish follows the same logic. As-machined surfaces land around Ra 1.6–3.2 μm. A high-finish cut reaches Ra 0.8–1.6 μm. Fine finishing gets to Ra 0.2–0.8 μm, and at that level you are often better served by a secondary process. Bead blasting, tumbling or polishing can hit a cosmetic requirement faster and cheaper than chasing it on the machine.

Inspection closes the loop. We inspect 100% of parts before shipment, with raw material checks, in-process monitoring and a final inspection, and reports are available on request. For a first article, the report is what tells you whether the process is stable or whether it passed by luck. If a feature is borderline on the report, it will be borderline again on the next run.

The hidden cost driver is setups, not cycle time. Two extra fixtures can add more to a quote than doubling the spindle time on a simple part. When a design can be reached from fewer directions, or when a feature can be toleranced loosely without hurting function, the quote drops. Engineers who mark only the functional tolerances usually get the better price.

• 1
  Feature-level toleranceApply tight limits only where the assembly needs them.
• 2
  Finish choiceDecide whether the surface is functional or cosmetic.
• 3
  First-article reportRead it for margin, not just pass or fail.
• 4
  Setup countReducing directions of approach cuts cost fastest.