Learn About CNC Processing: A Beginner's Guide

• 1
  Learn about CNC processing: what happens inside the machine
• 2
  Milling, turning, and when each one fits
• 3
  How tolerance and surface finish are set
• 4
  What the shop needs before cutting starts
• 5
  Where CNC processing stops making sense
• 6
  Step by step: from CAD file to shipped part
• 7
  Which cutting process fits your part

A CNC machine is a cutting tool mounted on a frame that moves along commanded axes. The controller reads G-code, a list of coordinates, feed rates and spindle speeds, and drives servo motors to those positions. Every part starts as a CAD model. CAM software turns that model into toolpaths: the exact path each cutter takes, how deep it bites, and how fast it travels. Change the model, and the toolpath changes with it. Nothing is carved by hand.

The cutting itself is simple mechanics. A rotating tool presses into metal and shears away chips. Heat leaves with the chip, which is why feed rate matters more than spindle speed for tool life. Cut too slowly and the tool rubs instead of cutting, work-hardening stainless and burning edges. Cut too fast and the tool breaks. On 6061 aluminium we run roughing passes at 2,000–4,000 mm/min with carbide cutters; on 316 stainless the same cutter drops to 300–600 mm/min.

Axis count defines what the machine can reach. A 3-axis mill moves X, Y and Z only, so the part must be re-fixtured for each new face. A 4-axis machine adds rotation around one axis, which suits shafts and cylindrical features. A 5-axis machine tilts the tool or the table in two directions at once, so it can cut an angled face, a deep pocket wall or an undercut in one setup. Fewer setups means tighter positional tolerance.

That last point is the engineering payoff. Every time you unclamp and re-fixture a part, you add a small positional error, typically 0.02–0.05 mm, and you add labor time. On a part with six faces, 3-axis machining may need five setups. The same part on a 5-axis center needs one or two. For a bracket with tight hole-to-hole location, the difference decides whether the print holds.

Milling uses a rotating multi-point cutter against a stationary workpiece. It removes material from flat faces, pockets, slots, profiles and complex 3D surfaces. If your part is prismatic, has pockets, or needs holes on multiple faces, milling is the default. GreatLight runs 27 three-axis machines, 12 four-axis mills and 16 simultaneous 5-axis machining centers, so the axis count follows the geometry rather than the other way around.

Turning spins the workpiece against a single-point tool. It is the fast, cheap way to make anything round: shafts, bushings, spacers, connectors, valve bodies. A turned part holds diameter tolerance easily because the tool never leaves the cut. For parts that are mostly round with some flats or cross-holes, a mill-turn center does both in one setup. We run 16 mill-turn centers for exactly this mix.

Pick wrong and the cost shows up twice. Milling a simple round bushing wastes cycle time and leaves a scalloped surface that needs finishing. Turning a blocky housing means multiple fixtures and slow material removal. The rule we use: if more than 60 percent of the material removal is rotational, turn it. If the part is mostly flat faces and pockets, mill it. Mixed geometry goes to mill-turn.

Material changes the decision too. Aluminium 6061, 7075 and 2024 cut freely and hold fine finishes. Stainless 303 and 304 work-harden, so keep the cutter moving and never dwell. Titanium TC4 (Ti-6Al-4V) and Inconel generate heat at the edge and need lower speeds, rigid setups and sharp tooling. Plastics like POM and PEEK cut cleanly but melt if feed is too low. On thin walls, support the part or it will chatter.

Tolerance is the allowed deviation from the drawing. It is not a single number for the whole part; it applies per dimension. A general block tolerance of ±0.1 mm is common on non-critical edges. A bearing bore or a locating hole may need ±0.005 mm. Mixing the two on one print is normal and is how you control cost. Tighten only the dimensions that matter.

Achievable tolerance depends on the machine, the material and the setup. Our general machining tolerance is ±0.005 mm (±0.0002 in) on critical features, but holding that on a 500 mm long aluminium part is harder than on a 50 mm steel pin. Thermal expansion alone moves aluminium about 0.023 mm per metre per degree Celsius. If a part is measured hot off the machine, the number will drift as it cools.

Surface finish is measured as Ra, the average roughness of the cut surface. As-machined finish from a standard end mill lands around Ra 1.6–3.2 μm. A finer finish, Ra 0.8–1.6 μm, comes from smaller stepovers, sharper tooling or a finishing pass. Mirror-level Ra 0.2–0.8 μm usually needs polishing or a dedicated finishing operation. Specify finish only where the part needs it: a sealing face, a sliding surface, a visible panel.

Finishing operations change the part after cutting. Anodizing adds a hard oxide layer on aluminium and can shift dimensions by a few micrometres. Electroless nickel and zinc plating add a thin uniform coat. Bead blasting gives a matte look and hides tool marks. Laser marking puts a part number or logo on the surface; the minimum character height we can mark clearly is 1.5 mm. Tell us the finish in the quote so tolerance and coating stack up correctly.

A clean 3D model and a 2D drawing are the two inputs. The STEP or IGES file carries the geometry. The drawing carries the tolerance, finish, material and any notes the model cannot express. If the drawing says nothing, we machine to a general tolerance and a standard as-machined finish. That is fine for many parts and wrong for a few. Send both when the fit matters.

DFM review happens before the first chip. We check wall thickness, tool reach, corner radii and datum strategy. A pocket with an internal corner sharper than the cutter radius cannot be machined without a separate EDM step, so we will ask whether that corner is functional. A hole with a depth-to-diameter ratio over 8 may need a pilot and a long drill. Catching these in the file saves a re-cut later.

Setup planning decides how many times the part is clamped. Fewer setups mean better positional accuracy and lower cost. For a one-off prototype we may accept an extra setup to avoid building a fixture. For a 10,000-part run we design a fixture that holds the part in one orientation and repeat it. The same drawing can be quoted two ways depending on volume.

Inspection closes the loop. We check raw material certificates on arrival, monitor dimensions during the run, and inspect the finished part before shipment. Reports are available on request. If a feature is critical, say so on the drawing and it gets measured and recorded rather than sampled.

CNC is subtractive. It removes material from a solid block, so cost tracks the volume you cut away, not the volume you keep. A part that starts as a 200 × 200 × 100 mm block and ends as a thin bracket wastes most of the stock. For a shape like that, die casting or sheet metal fabrication is cheaper per part once volume rises. We run both processes, so we will say when one beats the other.

Very high volume is the other limit. CNC is economical from one prototype to a few thousand parts. Beyond that, tooling for casting or molding spreads its cost across so many units that the per-part price drops below machining. The crossover depends on geometry and material. A complex part with tight tolerance may stay on CNC longer; a simple part crosses over sooner.

Some features are simply not millable. A sharp internal corner, a deep narrow slot, or a cross-drilled hole at a shallow angle can need electrical discharge machining or a custom tool. We flag these in DFM rather than quote a feature we cannot hold. It is better to redesign a corner than to pay for a special process that doubles lead time.

Hardness matters too. Above roughly 45 HRC, carbide cutters wear fast and the process slows. Pre-hardened tool steel at 30–40 HRC machines well. Fully hardened parts usually get ground or EDM after heat treatment. If your part needs hardening, machine it soft, then treat, then finish the critical surfaces.