Ways to Do CNC Machining: A Setup Guide for Engineers
There are many ways to do CNC machining, and the machine choice decides your tolerance, your fixturing and your cost. This guide walks through the five common setups, the parameters that matter, and the checks we run before a cutter touches metal.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
- 9
Key takeaways
Match the part geometry to the machine before you pick a cutting strategy
Most quoting arguments start with machines, not geometry. That is backwards. Start with the faces you must reach, the number of setups you can afford, and the tolerance that actually matters on the drawing. A bracket with one flat face and four holes does not need a 5-axis center. A housing with a compound-angle boss and an internal undercut usually does.
Write down three numbers before you open the CAM file: the tightest tolerance, the smallest internal radius, and the deepest pocket-to-diameter ratio. A pocket deeper than 4× the cutter diameter needs a long-reach tool, and long-reach tools deflect. If the drawing asks for ±0.005 mm at the bottom of that pocket, the process plan changes before the first tool is loaded.
There are many ways to do CNC machining, but the common ones fall into five setups: 3-axis, 4-axis, 5-axis, mill-turn, and dedicated turning. Each one trades reach against rigidity, and rigidity is what buys you surface finish and tool life.
One practical rule from the shop floor: if a part can be finished in two setups on a 3-axis machine, that plan usually beats a single-setup plan on a 5-axis machine for small quantities. Setup count is not the only cost. Programming time, fixture cost and inspection time all move together.
Cutting speed, feed and depth of cut: what each one does to the cut
Three variables control almost everything at the tool tip. Cutting speed drives temperature. Feed rate drives force and chip thickness. Depth of cut drives load on the insert and the spindle. Change one and the other two need a second look.
Cutting speed has the strongest effect on cutting temperature. In aluminium 6061, a 3-flute carbide end mill runs well between 200 and 350 m/min surface speed with good coolant flow. In 17-4PH stainless, drop to 40–70 m/min and expect shorter tool life at the top of that range.
Feed rate sets the chip load. Doubling the feed roughly doubles the cutting force, which is why a light finishing pass on a thin wall needs a smaller chip load, not a slower spindle. For a 10 mm carbide end mill in aluminium, 0.05–0.10 mm per tooth is a reasonable roughing range; drop to 0.02–0.05 mm per tooth for finishing.
Depth of cut is the least forgiving. Doubling the radial or axial engagement roughly doubles the cutting force and raises tool wear quickly. On a 27-machine 3-axis fleet, the safe roughing pattern is 50–70% radial engagement with axial depth matched to the flute length, then a finishing pass at 5–10% radial engagement.
- 1Cutting speed → temperatureHigher surface speed raises heat at the edge faster than any other change.
- 2Feed → forceFeed sets chip thickness; doubling it roughly doubles the cutting force.
- 3Depth of cut → loadEngagement controls spindle load and insert wear. Raise it last.
- 4Tool life → all threeSpeed, feed and engagement each shorten tool life when pushed.
Workholding choices decide whether your tolerance survives the cut
A part rarely fails because the machine was inaccurate. It fails because the part moved. Vise jaws, soft jaws, vacuum chucks and custom fixtures all behave differently under interrupted cuts.
For a first op on a rectangular block, a pair of hardened vise jaws with a 0.5–1 mm seat depth is enough for most aluminium work. For a thin plate under 3 mm, switch to a vacuum chuck or a sacrificial backing plate; vise pressure will bow the part and the finished thickness will vary across the face.
For a second op on a machined face, soft jaws bored to the part profile at the current spindle speed give the best repeatability. Bore them at the same speed you will run the job, because jaw runout changes with spindle speed.
The classic mistake is clamping on a finished surface with too much force. Aluminium 6061 marks easily. Use copper or nylon jaw liners, and torque the vise to a repeatable setting rather than by feel.
The five common setups and when each one is the right call
3-axis milling handles the majority of prismatic parts. Features on one face, or on two faces after a flip, cut cleanly with short rigid tools. If your part is a plate, a bracket or a manifold block with holes and slots, this is the cheapest and fastest route.
4-axis milling adds a rotary table, usually Ø400 mm on our machines. It suits parts with features on four sides of a rectangular block, like a valve body or a shaft with milled flats. It removes a second or third setup without adding the programming cost of full simultaneous motion.
5-axis machining covers two different jobs. Positional 5-axis indexes the part to an angle and then cuts with three axes, which is fast to program and rigid. Simultaneous 5-axis moves all axes at once, which is what you need for compound curves, deep undercuts and impeller blades.
Mill-turn centers combine a lathe spindle with milling capability. A part with a turned bore, a milled flat and cross-drilled holes finishes in one setup with a single datum. For hydraulic fittings and sensor housings, this removes the concentricity error that comes from moving the part between machines.
Dedicated turning remains the fastest way to make round parts. Shafts, bushings and spacers with a length-to-diameter ratio under 8 turn quickly with good surface finish. Past that ratio, add a steady rest or expect chatter.
Material behavior changes the way you cut, not just the speed
Aluminium is the easiest of the common metals. 6061-T6 machines freely, takes a good finish and holds ±0.005 mm on stable geometry. 7075 is stronger but more prone to chatter on thin sections, so reduce radial engagement and keep the tool short.
Stainless 304 and 316 work-harden. If the tool rubs instead of cutting, the surface hardens and the next pass is harder still. Keep the chip load up, never dwell, and use a fresh edge. 17-4PH in the H900 condition cuts cleanly at 40–70 m/min.
Titanium TC4 (Ti-6Al-4V) carries heat into the tool rather than the chip. Use low surface speed, high coolant pressure and a sharp uncoated or AlTiN-coated carbide tool. Expect shorter tool life than stainless and plan for it.
Plastics behave differently again. POM and PEEK cut cleanly with sharp two-flute tools and air blast. ABS and PC soften with heat, so reduce spindle speed and increase feed to keep the chip thick and the part cool.
How to verify the process before the batch runs
The cheapest inspection happens while the part is still on the machine. If your setup is correct, a single offset change fixes a dimension. If you pull the part and re-fixture it, you have lost the datum and the correction becomes a guess.
For a first article, measure the features the drawing marks as critical, plus one or two that reveal setup error. A wall thickness measured at three heights tells you whether the part is bowing. A bore measured at the top and bottom tells you whether the tool is deflecting.
For production runs, keep the same inspection method across the batch. Switching from calipers to a CMM mid-run introduces a measuring difference that looks like a process shift but is not.
We run raw material checks, in-process monitoring and a final inspection before shipment, with reports on request. A qualification rate of 99.99% comes from catching the first part, not from inspecting the last one.
Step by step: how to plan and run a CNC job
Follow this order from drawing to first article.
- 1Read the drawing and mark critical featuresMark the tightest tolerance, the datum faces and any surface finish callout. If a feature is called at ±0.005 mm while everything else is ±0.1 mm, that one feature drives the process.
- 2Pick the machine and count setupsChoose the smallest machine that reaches every feature. Target two setups or fewer for prismatic parts, and use a 4-axis or mill-turn setup only when it removes a flip. Every added setup adds alignment error.
- 3Choose stock and allow for distortionAdd 0.5–1 mm per side on machined faces for stress relief. On thin walls under 2 mm, rough, stress-relieve, then finish. Cutting both sides in one pass will bow the part.
- 4Design the fixture before the toolpathDecide the clamping points on non-critical surfaces. Keep clamp force off thin floors. For a second op, bore soft jaws at the job spindle speed for repeatable runout.
- 5Set cutting parameters from the materialAluminium 6061: 200–350 m/min, 0.05–0.10 mm per tooth roughing. Stainless 316: 60–90 m/min. Titanium TC4: 40–60 m/min. Start at the low end and watch chip color and sound.
- 6Run a first-article check before the full batchMeasure the critical features, not just the easy ones. Check wall thickness with a micrometer at three points. If the first article is in tolerance but near a limit, adjust the offset before running the rest.
- 7Control chips and coolant through the cycleAluminium needs high-volume flood coolant or through-spindle air to clear chips from deep pockets. Recutting a chip is the fastest way to break a small end mill.
- 8Deburr and inspect before the part leaves the machineBreak edges with a hand tool or a chamfer pass in the program. Then run the final inspection while the setup is still on the table, so any correction is a single offset change.
Which setup fits which part
Use this table to shortlist the machine before quoting.
| Setup | Best for | Typical tolerance | Watch out for |
|---|---|---|---|
| 3-axis milling | Plates, brackets, manifolds with features on 1–2 faces | ±0.01 mm | Multiple flips add alignment error |
| 4-axis milling | Blocks with features on four sides, shafts with flats | ±0.01 mm | Rotary table runout must be checked |
| 5-axis positional | Compound angles, angled holes, deep side access | ±0.005 mm | Long-reach tools deflect in deep pockets |
| 5-axis simultaneous | Impellers, blades, organic contours, undercuts | ±0.005 mm | Programming and simulation time is high |
| Mill-turn | Fittings, housings with bores and cross holes | ±0.005 mm | Bar size limits the part envelope |
| Turning | Shafts, bushings, spacers, round flanges | ±0.005 mm | Chatter above 8:1 length-to-diameter |
| Thin-wall milling | Housings with walls under 2 mm | ±0.01 mm | Clamping force bows the part |
Questions engineers ask before choosing a setup
How do I know if a part needs 5-axis machining?
Look at the reach, not the tolerance. If a feature sits behind another feature, at a compound angle, or at the bottom of a deep cavity that a straight tool cannot enter, you need 5-axis access.
If every feature can be reached from one of two perpendicular directions with a short rigid tool, 3-axis or 4-axis will usually be faster and cheaper.
What is a reasonable tolerance for a first prototype?
On stable geometry, ±0.005 mm is achievable on our machines and is the tightest we quote. On thin walls, long bores or unsupported sections, expect ±0.01 mm unless the process is split into roughing and finishing with a stress-relief step.
Tell us which features actually need the tight number. Applying ±0.005 mm to every dimension raises cost with no functional gain.
How does feed rate affect cutting force?
Cutting force scales roughly with chip cross-section, so doubling the feed doubles the force. That is why a finishing pass uses a smaller chip load rather than a slower spindle speed.
If a thin wall chatters, reduce radial engagement and feed per tooth together, and keep the tool as short as the geometry allows.
When should I use mill-turn instead of separate milling and turning?
Use mill-turn when concentricity between a turned bore and milled features matters. One setup means one datum, so the runout error from re-chucking disappears.
For simple round parts with no milled features, a dedicated lathe is faster and cheaper.
What causes a good first article to drift during a production run?
Tool wear is the usual cause, followed by thermal growth in the spindle and fixture. On long runs, check the critical dimension at fixed intervals and adjust the offset before the part drifts out of tolerance.
Chip buildup in deep pockets is another common cause. If the chip cannot leave, it gets recut and the load on the tool rises.
Do you machine from one prototype up to production quantities?
Yes. We have no minimum order quantity and run from a single prototype to 10,000+ part runs across 127 high-precision CNC machines, including 16 simultaneous 5-axis centers.
Quotation and free DFM analysis come back within 12 hours, and production can start within 24 hours.
Send your drawing and we will pick the setup
Upload a STEP file and we will return a quote, a DFM note and a recommended machine setup within 12 hours.
12-hour quoteFree DFM analysisNo MOQNDA on request
More process notes from GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
