CNC machining expert insights for design engineers

• 1
  What happens at the cutting edge
• 2
  How setup decisions limit what a machine can hold
• 3
  Why tolerance stack-up decides the real cost
• 4
  Material choice changes the whole process, not just the feed
• 5
  Finish selection: what the number means in practice
• 6
  Where CNC machining stops being the right answer
• 7
  Machining choice by part characteristic

Every CNC operation removes metal with a wedge-shaped tool pushed into the workpiece at a set feed per tooth. The chip carries away most of the heat. A chip that is too thin rubs instead of cutting, and the heat goes into the tool and the part. That is where chatter, work hardening and out-of-tolerance bores start.

Cutting speed is surface speed, not spindle rpm. A Ø10 mm carbide end mill in 6061 aluminium runs happily at 300–500 m/min, while the same tool in 316 stainless drops to 60–120 m/min. The tool diameter sets the conversion: rpm = surface speed × 1000 ÷ (π × Ø). Double the tool diameter and you halve the rpm for the same surface speed.

Feed per tooth controls chip thickness and therefore tool life. For aluminium, 0.05–0.15 mm per tooth is normal. For stainless and titanium, 0.02–0.08 mm per tooth keeps the edge from rubbing. Depth of cut and radial engagement trade against each other: a light radial pass (5–10% of tool diameter) lets you go deeper axially and keeps deflection down on long tools.

• 1
  Heat follows the chipThin chips push heat into the part and cause warping.
• 2
  Surface speed is material-dependentAluminium 300–500 m/min, stainless 60–120 m/min.
• 3
  Engagement trades against depthLight radial cuts allow deeper axial passes.

A machine is only as accurate as the setup that holds the part. Every time a part is removed and re-clamped, position is re-established from a datum, and each re-clamp adds variation. On a three-axis machine with four setups, that is four chances for a 0.02 mm shift. On a five-axis machine with one setup, it is one.

Thin walls are the classic failure case. A 0.8 mm wall in aluminium will deflect under a 12 mm end mill no matter how good the program is. The fix is not a slower feed; it is support. Fill the pocket with fixturing wax, leave sacrificial ribs, or step down to a Ø3–6 mm tool with a light radial engagement. Wall height to thickness ratios above 20:1 usually need a support strategy.

Workholding also sets the size ceiling. Our largest travels are 4,000 × 400 × 150 mm for long parts, and 750 × 1,150 × 550 mm for plate work. A Ø400 mm rotary table handles round parts that would otherwise need a second operation. If a feature sits on a face that cannot be reached in the same setup, cost climbs quickly.

• 1
  Fewer setups, less stack-upEach re-clamp adds positional variation.
• 2
  Support thin wallsAbove 20:1 height-to-thickness, use wax or ribs.
• 3
  Check the travel envelope first4,000 × 400 × 150 mm is our longest envelope.

A single ±0.005 mm callout is achievable on a rigid part with a good setup. Ten stacked ±0.005 mm callouts on the same drawing are a different problem. Tolerances accumulate from the datum outward, and each feature adds its own variation to the assembly. The question is not whether the shop can hold one dimension, but whether the stack still works at the worst case.

An engineer should separate functional tolerances from cosmetic or convenience ones. Bearing bores, seal grooves and mating faces need tight control. A clearance hole for an M6 screw does not. Opening those non-critical dimensions to ±0.1 mm or ±0.2 mm removes inspection time, reduces scrap risk and can change the process from a slow finishing pass to a normal one.

GD&T helps when it matches function. A position tolerance at MMC (maximum material condition) can allow a bonus tolerance as the hole grows, which is generous in the right way. A flatness callout on a surface that only needs to look flat is not. Every geometric control adds a measurement step, so put them only where the assembly actually feels them.

We inspect 100% of parts before shipment: raw material check, in-process monitoring and final inspection, with reports on request. That is the point at which a tolerance plan meets reality. If the drawing asks for something the process cannot repeat, the report will show it, and it is cheaper to change the drawing than to sort parts.

• 1
  Stack, not single featuresTen tight callouts behave differently than one.
• 2
  Open non-functional dims±0.1 mm on clearance holes saves time.
• 3
  Use GD&T where it functionsPosition at MMC gives useful bonus tolerance.

Aluminium 6061-T6 is the default for prototypes and fixtures because it cuts fast and holds a good finish. 7075 machines to a better strength-to-weight ratio but is less forgiving of sharp corners and tends to stress-relieve after heavy stock removal. 2024 is strong but has poor corrosion resistance unless it is anodized or coated.

Stainless grades behave differently from each other. 303 is free-machining and gives a clean finish. 304 and 316 work-harden quickly, so a dwell or a rubbing pass makes the next cut harder rather than easier. 17-4PH (SUS630) machines well in the solution-treated state and is often chosen for shafts and valve parts that need strength plus corrosion resistance.

Titanium TC4 (Ti-6Al-4V) and Inconel sit at the difficult end. They conduct heat poorly, so the edge stays hot and tool life drops. Low surface speeds, generous coolant and rigid setups are mandatory. Plastic parts follow different rules: POM and PEEK machine cleanly, while ABS and PP can gum up if the tool rubs. Carbon fibre needs diamond-coated tooling to avoid rapid edge wear.

We machine aluminium 6061, 2024, 5052, 5083, 6063, 6082, 7075 and ADC12; stainless 303, 304, 316, 316L, 420, 430, 431, 440C and 17-4PH; steels 1018, 1045, 4130, 4140, 4340, A36 and tool steel; copper and brass C101, C110, C36000 and beryllium copper; plus titanium, Inconel and magnesium. Material availability and machinability both shape the quote.

• 1
  6061-T6 is the baselineFast to cut, stable, takes a good finish.
• 2
  Stainless work-hardensAvoid dwell; keep the edge cutting.
• 3
  Titanium and Inconel need low speedsPoor heat conduction shortens tool life.

Surface roughness Ra describes average deviation from the mean line, not the visual look. As-machined surfaces typically land around Ra 1.6–3.2 μm, which is fine for brackets, housings and internal parts. A high-finish pass brings it to Ra 0.8–1.6 μm, which is where sealing faces and sliding surfaces usually sit.

Fine finishing to Ra 0.2–0.8 μm needs more than a slower feed. It usually means a dedicated finishing tool, a small stepover, and a part that is rigid enough not to vibrate. Achieving it on a thin wall or a long unsupported shaft is not realistic, no matter how the program is written. Match the callout to the geometry.

Coating and plating change dimensions. Anodizing builds oxide on the surface, hardcoat more than clear. Electroless nickel and zinc plating add a measurable layer, so threads and bores that must fit after coating need pre-plate dimensions. Laser marking needs a minimum character height of 1.5 mm to stay legible; below that, the mark becomes a smudge.

Bead blasting, tumbling, brushing and polishing are mechanical finishes that also deburr. They are often the cheapest way to remove sharp edges from a batch. Powder coating and black oxide cover the surface rather than refine it, so they are chosen for appearance or corrosion protection, not for dimensional control.

• 1
  Ra is not glossIt measures deviation, not shine.
• 2
  Fine finishes need rigidityRa 0.2–0.8 μm on thin walls is unrealistic.
• 3
  Coatings add thicknessPlan pre-plate dimensions for threads and bores.

CNC machining wins on tight tolerances, complex geometry and low-to-medium volumes. It loses when the part is a thin shell with uniform wall thickness, when the annual volume is in the tens of thousands, or when the geometry is mostly internal cavities that a mold could form in one shot. Die casting, vacuum casting and 3D printing each own a different corner of that map.

Small deep holes are a common boundary. A hole with a depth-to-diameter ratio above 10:1 needs a long, slender tool that deflects, so the hole drifts. Peck drilling helps, but the practical limit for reliable work is often 8:1 to 12:1 depending on material and diameter. Beyond that, consider EDM or a redesign.

Sharp internal corners are another. A cutter has a radius, so an internal corner is never sharper than the tool. Drawing a 0.5 mm corner radius on a pocket that is 40 mm deep forces a tiny tool with a long reach, which means slow passes and chatter risk. Opening the corner to the tool radius, or adding a relief, often cuts cycle time noticeably.

Volume economics matter too. From one prototype to 10,000+ part runs, machining is competitive without tooling cost. Above that, the amortized cost of a mold can beat it. The crossover depends on geometry and material, and it is worth checking both before committing to a process.

• 1
  Deep holes driftAbove 10:1 depth-to-diameter, expect problems.
• 2
  Corners have a radiusThe tool sets the smallest internal radius.
• 3
  Volume changes the mathMolds can beat machining at high annual volume.