Process guide

CNC Metal Cutting Techniques for Clean Edges and Tight Tolerances

This guide covers the CNC metal cutting techniques we use on aluminum, stainless, steel, titanium and copper parts. It is written for design engineers and buyers who need to judge a process before releasing a drawing. Read it and you can pick a cutter, set a starting feed, and know when a job should move to a five-axis machine.

Get Instant Quote Talk to an Engineer

±0.005 mm toleranceRa 0.8–1.6 μm as standard127 CNC machinesNo minimum order quantity

CNC metal cutting techniques and techniques on a machined metal part

On this page

Key takeaways

Match the cutter to the material firstA geometry that works in 6061 will chatter in 316L. Pick helix and coating before you touch the feed override.

Roughing and finishing are separate operationsLeave 0.3–0.5 mm radial stock for the finisher. One-pass cutting rarely holds ±0.005 mm.

Heat is the main cause of scrapChip load, not spindle speed, carries heat away. Too light a feed rubs the edge and work-hardens stainless.

Thin walls need support, not slower speedsReduce radial engagement and add tabs or sacrificial stock instead of dropping the feed to near zero.

Section 1

What CNC metal cutting techniques actually control

Cutting metal on a CNC machine comes down to four variables you can change at the panel: surface speed, feed per tooth, radial engagement and coolant delivery. Everything else, tool coating, helix angle, fixture rigidity, is chosen once and then lives with the job. When a part comes out undersized or the edge tears, the cause is almost always one of those four numbers, not the machine.

Surface speed is how fast the cutting edge travels through the material, measured in m/min. It is set by spindle rpm and cutter diameter. Aluminum 6061 runs happily at 300–500 m/min with carbide. 316L stainless wants 80–120 m/min. Titanium TC4 sits lower still, around 40–60 m/min, because it holds heat at the edge instead of sending it into the chip.

Feed per tooth is the thickness of material each flute removes. It is the number that keeps the tool cool. If you halve the feed but keep the same rpm, you do not cut more gently, you rub. Rubbing creates heat, work-hardens stainless and dulls the cutter faster than a heavy cut would.

Radial engagement is how much of the cutter diameter is buried in the material. Full-width slotting at 100 percent engagement is the hardest cut you can ask a tool to make. Dropping to 30–40 percent engagement lets you raise feed per tooth and remove metal faster while the tool stays cool. That trade is the basis of high-efficiency milling.

Coolant does two jobs: it removes heat from the cutting zone and it flushes chips out of the pocket. On deep pockets, chip evacuation matters more than cooling. A recut chip grinds against the wall and leaves marks that no finishing pass will hide.

1
Four live variablesSpeed, feed per tooth, radial engagement, coolant.
2
One fixed setCoating, helix, fixture, tool holder.
3
Feed keeps the edge coolLight feed rubs instead of cutting.

Section 2

Tool geometry and material pairings that work

A three-flute cutter with a 45° helix and a polished surface is the default for aluminum. It clears chips well and can be pushed hard. For 6061 and 7075 we normally run uncoated or ZrN-coated carbide. Aluminum sticks to titanium-based coatings, so a TiAlN tool in aluminum will build up on the edge and start smearing the wall.

Stainless 304 and 316L behave the opposite way. They work-harden under the cut, so the tool must stay in the cut and take a real chip. Use four or five flutes, a 38–45° helix, and an AlTiN or AlCrN coating that survives 900 °C at the edge. Never dwell in stainless. A pause of half a second lets the surface harden and the next tooth rides over a skin that is harder than the cutter.

Titanium TC4 and Inconel need sharp, positive-rake edges and generous coolant. Titanium has low thermal conductivity, so heat goes into the tool. Keep surface speed low, keep the chip load up, and change the cutter at the first sign of edge rounding. Inconel is worse, and we usually plan extra tools into the job rather than trying to stretch one.

Copper and brass cut cleanly but grab. C101 and C110 want sharp edges and high rake. A dull tool on copper produces a raised burr that is hard to remove later. For beryllium copper, coolant and dust control are a safety matter, not a finish matter.

Plastic parts change the rules again. POM and PEEK cut well with two or three flutes and air blast. Coolant can stain some plastics, so we often run dry with high-pressure air instead.

1
Aluminum2–3 flutes, 45° helix, uncoated or ZrN.
2
Stainless4–5 flutes, AlTiN, never dwell in the cut.
3
Titanium and InconelPositive rake, low speed, plan for tool changes.
4
Copper alloysSharp edge, high rake, watch the burr.

Section 3

Setup decisions that decide whether you hold ±0.005 mm

Tolerance starts at the fixture, not at the cutter. A part that moves 0.02 mm under cutting load cannot be machined to ±0.005 mm no matter how good the program is. We check three things before the first chip: is the part fully seated, is the clamping force spread over enough area, and is there a hard stop the tool can push against.

Thin walls and floor sections are the usual failure point. The fix is not to slow down. It is to reduce radial engagement, add tabs that hold the wall to the parent stock, and finish the wall from both sides so the load balances. For a 1 mm wall on an aluminum housing, we often leave 2 mm of sacrificial stock and cut it away in a separate operation.

Workholding also decides how many setups the job needs. Every extra setup adds a re-datum and a stack of error. On a 4,000 mm maximum processing size part, one 5-axis setup with a Ø400 mm rotary table can replace three 3-axis setups and cut positional error from 0.05 mm to under 0.01 mm.

Thermal drift matters on long cycles. A machine that has been idle all night is not the same machine after three hours of cutting. On tight jobs we warm the spindle, cut a test feature, measure it, and only then run the batch.

Inspection closes the loop. Our standard is raw material check, in-process monitoring and a final inspection before shipment, with reports on request. If a feature is called at ±0.005 mm, it gets measured on the machine and again on the CMM.

1
Fixture firstA moving part cannot hold ±0.005 mm.
2
Support thin wallsTabs and sacrificial stock beat slower feeds.
3
Fewer setupsEach re-datum adds error to the stack.
4
Warm up the machineThermal drift shows up on long cycles.

How to

Step by step: cutting a bracket from bar stock

A worked sequence for a 6061-T6 bracket with a ±0.02 mm bore and a Ra 1.6 μm face.

1
Read the drawing for the tightest featureList every tolerance and finish callout. The tightest one sets the whole sequence. A ±0.005 mm bore means the boring operation goes last, after the part has stopped moving.
2
Pick stock and leave machining allowanceAdd 1–2 mm per side on faces that will be cut. On 6061-T6 plate, 1.5 mm allowance on each face is enough to clean up saw marks and still leave material for two finishing passes.
3
Face and square the first sideUse a 50 mm face mill, 4 inserts, at 350–500 m/min surface speed and 0.10–0.15 mm per tooth. Take 1 mm depth on the rough pass and 0.3 mm on the finish pass. Flip once and repeat, so the two faces are parallel within 0.02 mm.
4
Rough the profile with 30–40 percent radial engagementA 12 mm three-flute carbide cutter at 0.08 mm per tooth. Leave 0.3–0.5 mm radial stock on walls and 0.2 mm on the floor. Do not climb into a full-width slot if you can avoid it.
5
Drill and tap before the finishing passesSpot drill every hole to 0.5 mm depth, then drill. For M6 in 6061, run a 5.0 mm drill and tap at 300–500 rpm with a forming tap if the material allows it. Forming taps leave no chips to trap in a blind hole.
6
Finish the walls and floor in one continuous pathSame cutter, 0.3 mm radial stepover, 0.2 mm axial depth, full feed. Keep the tool moving. A pause on the wall shows up as a witness mark that no polishing will remove.
7
Bore the tight feature on the same setupBore or ream the ±0.005 mm bore without unclamping. Measure on the machine, adjust the offset once, and re-cut. This is the step where a second setup would cost you the tolerance.
8
Deburr, inspect and recordBreak edges with a 0.3 mm chamfer or a hand tool, then inspect the bore, the wall thickness and the face finish. Log the offsets you used so the next run starts from a known point.

Judge the job

Which cutting approach fits which part

Match the part geometry and tolerance to the process before quoting.

Part condition	Best approach	Typical starting point	Watch out for
Prismatic part, 3 faces, ±0.05 mm	3-axis milling	6,000–10,000 rpm, 0.08 mm/tooth	Re-datum error across setups
Five-sided part, ±0.02 mm	5-axis simultaneous	One setup, Ø400 mm table	Fixture access under the part
Long profile up to 4,000 mm	Large-travel mill	400 × 150 mm section	Thermal growth along the length
Thin wall under 1.5 mm	3-axis plus tabs	30% radial engagement	Chatter and wall deflection
Turned shaft with milled flats	Mill-turn center	Turn, then mill in the same setup	Concentricity after reclamping
Hardened tool steel, 50 HRC	3-axis with CBN or coated carbide	Low speed, small stepover	Edge wear after a few passes
Titanium TC4, ±0.01 mm	5-axis, high coolant	40–60 m/min surface speed	Heat into the tool
Inconel, tight pocket	3-axis, small tools	Plan extra cutters into the job	Tool life, not cycle time