Precision Metal Cutting: Basics of CNC
This page covers the basics of CNC as they apply to precision metal cutting: what the controller actually controls, how material is removed, where the process holds ±0.005 mm and where it does not. Written for design engineers and buyers who need to judge whether a part belongs on a CNC machine or somewhere else.
What the basics of CNC actually control
A CNC machine does not cut a drawing. It cuts a toolpath. Between the two sits a chain you can measure: CAD model, CAM toolpath, post-processed G-code, controller interpolation, servo motion, spindle, tool, workpiece. Every tolerance you see on a print is the sum of errors in that chain. Understanding the basics of CNC means knowing which link is limiting you.
The controller reads G-code as a list of blocks. Each block tells the machine where to go, how fast, and which tool is turning. Linear moves (G01) interpolate along a straight line; arcs (G02/G03) follow a radius; rapid moves (G00) reposition without cutting. The controller does not see a cylinder or a pocket. It sees coordinates and feed rates, thousands of times per second.
Feed rate is usually written in mm per minute, spindle speed in rpm. The product of feed per tooth, number of teeth and rpm gives table feed. Get that relationship wrong and you get chatter or burned edges, not a dimension error. This is the first thing to check when a surface finish drifts.
Positioning accuracy and repeatability are different claims. Accuracy is how close the machine gets to commanded position. Repeatability is how consistently it returns to the same point. A machine with ±0.005 mm repeatability can still produce a part 0.03 mm off if the toolpath or the setup is wrong. Good shops control both.
- 1ControllerInterprets G-code and closes the position loop
- 2Servo and ball screwTurn commands into motion within microns
- 3Spindle and toolDefine surface speed, chip load and finish
- 4FixtureHolds the part rigid; a weak setup shows up as chatter
How metal is actually removed
Every cut is a controlled fracture. The tool edge presses into the material, the metal deforms plastically, a chip forms and slides up the rake face. Heat leaves with the chip, not with the part, which is why chip evacuation matters more than coolant volume. If chips recut, you lose finish and tool life at the same time.
Cutting speed depends on the material and the tool coating. Aluminum 6061 runs fast, often 300–600 m/min surface speed with uncoated or ZrN carbide. 316 stainless runs slow, roughly 120–180 m/min, because it work-hardens and holds heat at the edge. Titanium Ti-6Al-4V is slower still and needs high-pressure coolant. These are starting points, not laws.
Depth of cut and stepover set the cutting force. Roughing removes material quickly with a large axial depth and moderate stepover. Finishing takes light passes at high spindle speed to hit Ra 0.8–1.6 μm, and a spring pass can reach Ra 0.2–0.8 μm on a rigid setup. Skip the semi-finish pass and the finish pass inherits the roughing marks.
Tool deflection scales with the cube of the length-to-diameter ratio. A Ø6 mm end mill sticking 60 mm out of the holder will deflect roughly ten times more than the same tool at 20 mm. If a feature keeps coming out tapered, shorten the tool or change the approach before you blame the machine.
- 1Aluminum 6061300–600 m/min, easy chip evacuation
- 2316 stainless120–180 m/min, watch work hardening
- 3Ti-6Al-4V40–60 m/min, high-pressure coolant
- 4Tool steel80–120 m/min, rigid setup required
Three-axis, four-axis and five-axis: what each adds
A three-axis machine moves the tool in X, Y and Z while the part stays fixed. It handles plates, brackets, housings and most prismatic parts well. Its limit is access: any feature on a side face, or a hole that is not parallel to the spindle, needs a second setup. Each additional setup adds a datum transfer and its own error.
A four-axis machine adds rotation about one axis, usually A, on a rotary table. That lets you cut around a cylindrical part in one setup: shafts, flanges, cam profiles, parts with holes on multiple faces around an axis. The Ø400 mm rotary table we run covers most of that work.
A five-axis machine adds a second rotation, so the tool can approach the part from nearly any direction. This is what makes undercut walls, deep pockets with drafted sides, impellers and medical bone plates machinable in one setup. The gain is not only geometric freedom. Fewer setups mean fewer datum errors, and a single setup usually holds a tighter true position on related features.
Five-axis is not automatically more accurate. Simultaneous motion introduces rotary axis errors that a three-axis machine never sees. A three-axis machine with a good fixture can beat a five-axis machine with a sloppy one. Match the machine to the part, not to the spec sheet.
- 1Three-axisPrismatic parts, flat datums, one or two faces
- 2Four-axisCylindrical and multi-face parts around one axis
- 3Five-axisUndercuts, contoured surfaces, one-setup complex parts
- 4Mill-turnTurned features plus milling without re-chucking
Workholding, datums and the setup error nobody counts
The part is only as stable as the fixture holding it. A vise with a 0.02 mm jaw lift will tilt a thin plate. A three-point support on a casting that rocks will spring under cutting load. Engineers who specify ±0.005 mm on a part with a 0.5 mm wall should expect the fixture to be the binding constraint, not the machine.
Datums should be chosen so the critical dimensions are measured from the same face used to locate the part. On a five-axis job, that usually means a machined face plus two dowel holes. On a three-axis job, it means a clean corner and a flat bottom. If the print calls a datum that cannot be touched in the first setup, the shop has to invent one, and the tolerance stack grows.
Thin walls deflect under clamping force. A 1 mm aluminum wall clamped at 2 kN will move. The usual fix is to leave stock for a finishing pass after unclamping, or to support the wall with a soft jaw or low-melt fixturing. For parts under 2 mm wall thickness, plan for a flip operation.
Thermal drift is the slow error. A spindle running for hours grows a few tens of microns; a shop without temperature control sees dimensions walk through the day. We check first-off and mid-run parts against the print, because a machine that was correct at 08:00 is not guaranteed correct at 16:00.
- 1Three-point supportUse on castings and rough stock, not on finished faces
- 2Datum transferEach extra setup adds stack-up error
- 3Soft jawsMachine them in place for thin-wall parts
- 4Thermal checkRe-measure after long spindle runs
Choosing the process for a metal part
Pick by geometry, tolerance and quantity, not by habit.
| Process | Best fit | Typical tolerance | When it does not fit |
|---|---|---|---|
| 3-axis CNC | Prismatic parts, plates, brackets | ±0.005 mm on a rigid setup | Undercut features, deep side access |
| 4-axis CNC | Shafts, flanges, multi-face holes | ±0.005 mm, rotary repeatable | Free-form surfaces, compound angles |
| 5-axis CNC | Impellers, contoured pockets, medical plates | ±0.005 mm, one setup | Simple flat parts, cost not justified |
| Mill-turn | Turned body with milled flats and holes | ±0.005 mm, fewer setups | Very long parts beyond travel |
| CNC turning | Cylindrical parts, threads, bores | ±0.005 mm on diameter | Large prismatic blocks |
| Sheet metal | Enclosures, brackets under 6 mm | ±0.1 mm typical | Thick sections, tight bores |
| Die casting | High-volume housings, 1,000+ parts | ±0.05 mm plus machining | One-offs, tight tolerances as-cast |
| 3D printing | Prototypes, internal channels | ±0.1 mm typical | Load-bearing metal parts |
When CNC is the right call
If the part is metal, needs ±0.005 mm on more than one feature, and the geometry has undercuts or compound angles, choose five-axis CNC and design for one setup. If the part is flat, prismatic and under 200 pieces, a three-axis machine with a good fixture will hit the same tolerance for less money. Use casting only when volumes pass 1,000 and the as-cast tolerance is loose enough to machine.
Questions engineers ask about CNC cutting
What tolerance can a CNC machine hold on a typical metal part?
On a rigid setup with a stable material, ±0.005 mm is achievable on critical features. That figure is not automatic for every dimension on the print. Thin walls, long tool overhangs and deep bores widen the realistic window.
Send the full drawing with datums and we will tell you which features are genuinely held at ±0.005 mm and which need a looser callout or a design change.
How do I know if my part needs five-axis machining?
Look for three signs: features that cannot be reached from one spindle direction, compound angles that would need multiple fixtures, and related features whose true position matters across several faces.
If none of those apply, three-axis or four-axis is usually the better choice. Five-axis adds cost through programming and cycle time, and it only pays back when it removes setups or enables geometry you cannot make otherwise.
Which metals are easy and which are hard on a CNC machine?
Aluminum 6061, 7075, brass C36000 and mild steel 1018 cut cleanly and hold tight tolerances. Stainless 316 and 17-4PH work-harden, so light passes and constant feed matter. Titanium Ti-6Al-4V and Inconel hold heat at the edge and need high-pressure coolant and slower speeds.
We machine all of these. The material choice affects cycle time, tool life and the surface finish you can expect off the machine.
Can CNC hit a mirror finish straight off the tool?
Ra 0.2–0.8 μm is reachable with a fine finishing pass, a sharp tool and a rigid setup. Below that, you are in polishing or lapping territory.
As-machined parts typically sit at Ra 1.6–3.2 μm, and a standard finish pass reaches Ra 0.8–1.6 μm. Tell us the finish callout and we will match the toolpath to it.
How does workholding affect the tolerance I get?
More than most engineers expect. Clamping force bends thin parts, jaw lift tilts plates, and an unstable support lets the part move under load. Any of these can consume the whole tolerance budget before the cutter touches metal.
Good shops design the fixture around the part. If your part has walls under 2 mm or free-form surfaces, mention it at quote time so the setup is planned for it.
What file formats and information should I send for a quote?
STEP or IGES for 3D geometry, a 2D PDF with datums and tolerances, plus material, finish and quantity. Note any critical features explicitly rather than relying on general block tolerances.
We return a quotation and a free DFM analysis within 12 hours, and production can start within 24 hours of approval. Uploads stay confidential and we sign an NDA on request.
Send the drawing, get a real answer
Upload your STEP file and print. We will review the geometry, flag features that fight the tolerance, and quote within 12 hours.
12-hour quoteFree DFM analysisNDA on request100% inspection
Follow GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
