CNC Machining: Milling, Turning, Tolerances & Materials

CNC machining removes material from a solid blank using programmable cutting tools guided by computer numerical control. It is the default subtractive process for metal and rigid-plastic parts that need tight tolerances, repeatable geometry, and a surface finish close to the final dimension. The two base operations are milling, where a rotating multi-point cutter moves against a mostly stationary workpiece, and turning, where the workpiece itself rotates against a single-point tool.

Most CNC metal work is held to ISO 2768-1 fine class, roughly ±0.10mm (±0.004in) on a 6 to 30mm (0.24 to 1.18in) feature, with precision setups reaching ±0.025mm (±0.001in). Standard as-machined surface finish sits around Ra 3.2µm (125µin); a fine-finishing pass brings it to about Ra 0.8µm (32µin), and grinding reaches Ra 0.4µm (16µin) or better.

How CNC machining works

A CNC machine reads toolpath code, usually generated from a CAD model through CAM software, and drives the cutting tool along those paths with high positional accuracy. The machine frame, the spindle, and the feedback systems (linear scales or rotary encoders) together determine how tightly a feature can be held and how smooth a surface can be left. Rigid cast-iron or polymer-concrete frames damp vibration, which matters most when cutting hard alloys or holding single-micron tolerances.

Milling

In milling, the cutter spins and the workpiece is clamped to a table that moves it past the tool. End mills remove material from faces, pockets, and slots; face mills take wide, shallow cuts across flat surfaces; ball mills sculpt curved and contoured surfaces. Milling is the natural choice for prismatic parts, housing, brackets, molds, and any geometry defined mainly by flat or gently curved faces. Because the tool is round, every internal corner carries a fillet, and the size of that fillet is set by the smallest tool that can reach the corner.

Turning

In turning, the workpiece is held in a chuck or collet and spun on a spindle while a single-point tool feeds into it. Turning produces cylindrical features: diameters, tapers, threads, radii, and facing cuts. A CNC lathe can also drill and bore on the centerline, and a live-tool lathe (mill-turn) can add milled flats and cross-holes in the same setup. Turning is the right process for shafts, pins, bushings, fittings, and any part whose main geometry is rotationally symmetric.

Axes: 3, 4, and 5

A 3-axis machine moves the tool in X, Y, and Z. It handles the majority of prismatic work in one or two setups. A 4th axis adds rotation, usually for indexing parts between faces or cutting helical and cam features. A 5th axis adds a second rotary axis so the part can be tilted and rotated to present almost any face to the tool, which lets complex geometry and undercuts finish in a single setup. Five-axis work cuts setup error and improves access, but it costs more per hour and requires more programming skill. Whether a given shop offers 3, 4, or 5-axis work varies, so capability should be confirmed rather than assumed (see 5-axis CNC machining).

Tooling, workholding, and setup

The cutting tool and how the part is held matter as much as the machine itself. Most CNC metal cutting uses solid-carbide tools or indexable-carbide inserts; high-speed steel survives only on softer, lower-speed work. Coatings extend tool life on abrasive and work-hardening alloys: titanium aluminum nitride (TiAlN) is common for steel and stainless, while uncoated or polished tooling suits aluminum to reduce edge buildup. Feed per tooth, surface speed, and depth of cut are set from published speed-and-feed tables for each material, then refined on the shop floor by listening for chatter and watching chip color and shape. A blue chip on steel means too much heat; a thin, curled chip usually means a healthy cut.

Workholding sets the achievable tolerance, because a part that shifts under load cannot be held tightly. Vises, soft jaws, fixture plates, vacuum tables, and magnetic chucks each suit different geometries. The aim is to grip the part rigidly through every cut without distorting it, and to leave a reference datum that inspection can return to. Parts that need several operations run in a defined sequence of setups, and every added setup introduces a chance for cumulative error, which is why reducing setups is one of the largest tolerance and cost gains available.

The CAM workflow

A part moves from CAD to CAM to the machine. The CAM system generates toolpaths from the model, selecting tools, speeds, feeds, and the order of operations. The programmer simulates the paths to catch collisions and wasted air cuts, then posts the code in the dialect the control reads, commonly G-code. Thoughtful CAM work shortens cycle time, protects tooling, and is where most of the difference between an efficient and an inefficient setup is made. A well-programmed roughing strategy can remove the bulk of the material in a fraction of the time a default path would take.

Tolerances and surface finish

Tolerance tiers

For machined metals, ISO 2768-1 fine class is the working default: ±0.05mm for sizes from 0.5 to 3mm (±0.002in for 0.02 to 0.12in), ±0.10mm for 6 to 30mm (±0.004in for 0.24 to 1.18in), and ±0.15mm for 30 to 120mm (±0.006in for 1.18 to 4.72in). Medium class, roughly double those values, is the general default for non-critical features. Precision work targets ±0.05mm (±0.002in), high-precision work reaches ±0.025mm (±0.001in), and the tightest setups can hold ±0.013mm (±0.0005in) on suitably rigid machines with temperature control.

Geometric tolerances follow ISO 2768-2 grade K in common practice, with flatness, parallelism, and perpendicularity around 0.05mm (0.002in) for typical parts. Critical fits and datums are usually specified with GD&T per ASME Y14.5 or ISO 1101 so that inspection is repeatable across suppliers.

Surface finish

Surface finish is reported as Ra, the arithmetic average roughness. A standard as-machined milled or turned surface is about Ra 3.2µm (125µin). A finishing pass or a sharper tool with a smaller depth of cut brings that to Ra 1.6µm (63µin). Grinding reaches Ra 0.8µm (32µin) and below, and lapping or honing can produce mirror surfaces below Ra 0.2µm (8µin). Smoother finishes cost more because they need slower feeds, finer tooling, and added operations, so they are specified only where function or appearance requires them.

Materials

Aluminum

Aluminum 6061-T6 is the most common CNC alloy: it machines freely, holds ±0.025mm (±0.001in), and balances strength, corrosion resistance, and cost. Its tensile strength of 310MPa (45ksi) suits brackets, housings, and structural fittings. Aluminum 7075-T6 is far stronger, at 572MPa (83ksi), and is used for aerospace and high-stress structural parts, though it costs more and is not suitable for bending. Both alloys conduct heat well, which helps tool life, but they can build up on a cutting edge, so sharp tooling and flood coolant are standard.

Carbon steel and stainless

Carbon steel 1018 (about 70 percent of free-machining brass) and 1045 (closer to 60 percent) are general-purpose choices with good machinability and tensile strengths from 440 to 690MPa (65 to 100ksi). Stainless 304 and 316 are chosen for corrosion resistance; 316 adds 2 to 3 percent molybdenum for chloride and marine service and costs 15 to 30 percent more than 304. Both austenitic grades work-harden under dull tooling, so they need sharp tools, positive rake geometry, and adequate feed. Stainless machines at roughly 45 percent of the rate of free-machining brass, which is slower and costlier than carbon steel.

Titanium

Titanium Ti-6Al-4V is prized for its strength-to-weight ratio (tensile 895 to 1105MPa, or 130 to 160ksi, at about 60 percent of the density of steel) and corrosion resistance. It is also one of the harder CNC metals to cut. Its low thermal conductivity, about 6.7 W/m·K, concentrates heat in the cutting edge, and it work-hardens and tends to gall. Practical machining needs carbide tooling, low surface speed, high feed per tooth, generous flood coolant, and rigid setups. The result is longer cycle times and faster tool wear, which is reflected in part cost.

Brass and copper

Free-machining brass C360 is the benchmark for machinability, rated 100 percent on the brass scale, and it runs at high speed with excellent chip control. It is used for fittings, valves, electrical contacts, and decorative parts. Copper C110 has the highest electrical conductivity of common coppers (101 percent IACS) but is gummy and hard to machine cleanly; it is usually cut at lower speeds with sharp tooling. Copper is also highly reflective, so it is a poor fit for fiber laser cutting and is better parted by sawing or milling.

Engineering plastics

Rigid plastics machine on the same equipment at lower spindle loads. Acetal (POM) is the general-purpose choice for jigs, fixtures, and low-friction parts; it holds tolerance well and machines cleanly. PEEK serves high-temperature and chemical-resistant duties but costs many times more and needs care to avoid stress cracking. Glass-filled nylon and glass-filled PEEK are abrasive and call for carbide tooling to resist rapid wear. Plastics expand and contract with temperature far more than metals, so they are allowed to stabilize before final inspection and held to looser tolerances on long dimensions.

Milling vs turning: choosing the right process

The split between milling and turning comes down to the dominant geometry. If the part is defined by flat faces, pockets, slots, or complex 3D surfaces, it is a milling part. If it is defined by diameters, lengths, tapers, and threads around a centerline, it is a turning part. Many real parts combine both, which is why mill-turn centers and live-tool lathes exist: they turn the cylinder, then mill flats and drill cross-holes without a second setup.

Choose milling when

• The part is prismatic, with faces at right angles and features cut into flat or contoured surfaces.
• You need pockets, slots, gear teeth, or 3D-mold surfaces.
• Internal corners can accept a fillet and the part fits the machine’s travel.
• Example: an aluminum housing with a deep pocket, bolt holes, and a mating flange is a milling job, often 3-axis for the bulk and a 5-axis flip for an undercut.

Choose turning when

• The part is cylindrical or rotationally symmetric: shafts, bushings, pins, fittings, threads.
• You need close control of diameters and concentricity, which a lathe holds by spinning the part on its own axis.
• Example: a stainless shaft with stepped diameters, a sealing groove, and threaded ends is a turning job, finished in one chucking if the length-to-diameter ratio allows.

Design rules for CNC parts

Good CNC design works with the process rather than against it, and most of the savings come from a handful of rules applied early.

• Internal corners need a fillet. The radius cannot be smaller than the cutter that will reach it. A practical inside radius is 0.2 to 0.5mm (0.008 to 0.020in) for standard endmills; larger radii let the shop use a stiffer tool and run faster.
• Keep walls thick enough to stay rigid. Non-critical walls from 0.5 to 1.0mm (0.020 to 0.040in) are possible but deflect under cutting force; structural walls should be 1.5mm (0.060in) or more.
• Limit hole depth. Drilled holes lose accuracy beyond a 4:1 depth-to-diameter ratio; gun drilling reaches 10:1 and beyond. Deep holes also need chip-evacuation cycles.
• Tolerances cost money. Holding ±0.13mm (±0.005in) is routine. Tightening every feature to ±0.025mm (±0.001in) roughly doubles cost through slower feeds, extra setups, finer tooling, and added inspection. Specify tight tolerances only where function requires them.
• Avoid deep, narrow pockets and tall, thin features. They need long, slender tools that chatter and wear quickly. If a pocket must be deep, allow a larger corner radius and a wider floor.
• Standardize hole sizes and threads. Common drills and taps are cheaper to run and stock than specials.
• Plan for workholding. Leave a clamping surface or a tab the shop can grip, and avoid features that need a custom fixture for a single operation.

File format guidance

• A STEP file (.step or .stp) is the expected 3D format for CNC. It preserves geometry and tolerances and is the neutral exchange format CAM systems read most reliably.
• STL is for 3D printing, not CNC. It carries no tolerance data and approximates curves as facets, so it is not a machining input.
• Always state units in the file or filename. A file submitted without explicit units is read against a supplier default, and a millimeter-versus-inch mix produces parts at the wrong scale, a 25.4x error.
• Add a 2D drawing for critical dimensions, tolerances, thread calls, and surface-finish notes. The 3D model gives geometry; the drawing gives intent.
• For sheet metal, submit the flat unfolded shape rather than a bent 3D model so the flat pattern and bend allowances are unambiguous.

What drives CNC machining cost

Cost breaks down into material, setup, cycle time, tooling, and finishing. Understanding these levers helps a buyer design for economy rather than discover the cost too late.

The cost levers

• Material: the alloy and the stock form set the starting price. Titanium and stainless cost more per kilogram than aluminum or carbon steel, and hard-to-machine alloys add cycle time on top of their raw-material premium.
• Setup: every operation that needs a new fixture or re-orientation adds labor and a chance for error. Consolidating features into fewer setups is one of the largest savings available.
• Cycle time: driven by the volume of metal removed, the feeds and speeds the alloy allows, and the depth of pockets and holes. Removing a lot of material slowly is expensive.
• Tolerance and finish: tight tolerances and fine finishes demand slower feeds, finer tooling, added passes, and more inspection.
• Finishing and secondary operations: anodizing, powder coating, passivation, and assembly each add steps and cost downstream of machining.
• Volume: setup cost amortizes across the batch, so a second or tenth part costs far less than the first. This is why CNC suits low to mid volumes while injection molding or stamping wins at high volume.

For a sense of scale, a straightforward aluminum bracket is roughly an order of magnitude cheaper per part in bulk than as a one-off, almost entirely because the one-off carries the full setup and programming cost. The same logic is why engineers are encouraged to combine similar parts into a single order. See CNC machining quote for how these factors combine into a price.

Applications and industries

CNC machining serves almost every industry that needs precision metal or plastic parts. Aerospace work centers on aluminum and titanium structural brackets, fittings, and engine components held to tight tolerances with full material traceability. Medical parts span surgical instruments, implants, and device housings in biocompatible alloys, often produced on Swiss-type equipment. Automotive applications range from prototype fixtures and engine components to low-volume brackets and housings. Robotics, defense, optics, and consumer electronics all rely on CNC for housings, heat sinks, mounting plates, and precision linkage.

The common thread is a need for accuracy and repeatability that molding or cutting cannot deliver, at volumes from a single prototype to a few thousand units. Above that, dedicated tooling for molding, casting, or stamping usually wins on per-part cost.

When CNC machining is not the right choice

CNC is not economical for every part. Large, flat, or thin sheet parts are better cut by laser, waterjet, or plasma, which remove material without the cycle time of milling a wide area. High-volume simple parts are cheaper to mold, cast, or stamp once tooling amortizes. Very complex internal geometry that no cutter can reach may need EDM or additive manufacturing instead. And parts that need only loose tolerances and a simple shape may cost less as a casting or an extrusion. For an honest cost comparison, the deciding factors are the part geometry, the tolerance, the volume, and the material, and a good shop will flag when another process fits better.