How-to guide

Understanding CNC Machining: A Step-by-step Guide

This guide walks through the order of decisions that actually set part quality: drawing review, workholding, zero point, speeds and feeds, toolpath, in-process checks, and final inspection. Written for design engineers and buyers who need to judge whether a feature can be cut as drawn, and what to change when it cannot.

Get Instant Quote Talk to an Engineer

±0.005 mm toleranceRa 0.2–0.8 μm finish16 five-axis centers3–5 day shipping

Understanding CNC machining shown on a 5-axis machined engine part

On this page

Key takeaways

Tolerance drives everything±0.005 mm is reachable, but only when workholding and thermal drift are controlled first.

Order mattersZero point and stock allowance decide more than spindle speed ever will.

Speeds and feeds are a starting pointUse surface speed and chip load, then correct by chip shape and sound.

Inspection is part of the processMeasure at the machine between operations, not only at final inspection.

Some features should not be machinedDeep narrow slots and sharp internal corners are cheaper redesigned than cut.

Start here

Understanding CNC Machining Before You Cut Metal

Understanding CNC machining starts with one question: what does the drawing actually demand? A block with three Ø6 mm holes at ±0.1 mm and a flat face at Ra 3.2 μm is a different job from the same block with a 0.05 mm wall and a true position callout of 0.02 mm. The first runs on a three-axis mill in one setup. The second may need five-axis access, a soft-jaw fixture, and a temperature-stable room.

Read the drawing in layers. First find the datum scheme, because every tolerance that follows is measured from it. Then find the tightest single feature, since that one feature usually controls the machine choice, the workholding, and the number of setups. Then scan for features that cannot be reached from a single direction: undercuts, side holes, and pockets with a depth-to-width ratio above 4:1.

The third pass is material. Aluminium 6061-T6 cuts fast and moves little, so a ±0.005 mm band is realistic on a controlled machine. Stainless 316 and Inconel work-harden at the cut, generate more heat, and spring back after the tool passes. Titanium TC4 (Ti-6Al-4V) adds another constraint: low thermal conductivity means heat leaves with the chip, not the part, so coolant strategy matters as much as the feed rate.

A useful habit is to write down, before quoting, the answer to three things: the tightest tolerance, the smallest internal radius, and the largest dimension. Those three numbers predict more about cost and lead time than the part volume does. If any of them is outside what the process can hold comfortably, fix it at the design stage rather than at the machine.

1
Datum firstTolerances stacked on a vague datum cannot be inspected repeatably.
2
Tightest feature sets the machineOne 0.02 mm true position can push a part from three-axis to five-axis.
3
Depth-to-width above 4:1 needs a planLong reach tools deflect; expect a separate roughing and finishing pass.

Setup

Workholding, Zero Point, and Stock Allowance

Workholding decides the result more often than the cutting data does. A vise with 0.02 mm jaw lift will move a thin plate when the cutter loads it. For plates below 6 mm thick, use a fixture plate with support under the whole footprint, or clamp on a sacrificial tab and cut the tab off in a second operation. For rings and bushings, a Ø400 mm rotary table with a three-jaw chuck gives better roundness than clamping on the outside diameter in a vise.

Zero point selection is the next decision. Set the zero where the drawing datums are, not where it is convenient to touch off. If the drawing calls out datum A as a face and datum B as a bore, zero the machine on that face and bore, then record the offsets. This keeps the setup aligned with inspection later. On five-axis work, the rotary center becomes part of the zero chain, so verify it with a test bar before the first cut.

Stock allowance should be planned per surface, not as a single number. A typical plan leaves 0.5–1.0 mm on faces that will be finish-machined later, and 0.3 mm on bores that will be bored rather than drilled. Leave too little and the finishing pass cannot clean up the roughing marks. Leave too much and the finishing tool takes a heavy load on a light pass, which pushes the part away from the cutter.

For parts that will be heat treated or anodized, add allowance for the process, not just for machining. Anodizing builds roughly 5–25 μm per surface depending on the coating type, which matters on a Ø8 H7 bore. Hardcoat anodizing is thicker and can change a sliding fit into an interference fit. Tell the machinist which surfaces are functional and which are cosmetic before the first cut.

1
Support the whole partThin plates need backing, not just clamping force.
2
Zero on the datumsMachine offsets and inspection reports then speak the same language.
3
Plan stock per surface0.5–1.0 mm on finish faces, 0.3 mm on bores to be bored.
4
Budget for coating thicknessAnodizing changes fits; mask or compensate before machining.

Cutting data

Speeds, Feeds, and What the Chip Tells You

Speeds and feeds come from two numbers: surface speed at the cutting edge and chip load per tooth. Surface speed is set by the tool material and the workpiece. Uncoated carbide in aluminium 6061 runs comfortably around 300–500 m/min. The same tool in 304 stainless drops to roughly 80–120 m/min. Inconel and titanium sit lower still, often 30–60 m/min, because the heat has nowhere to go.

Chip load is the feed per tooth, and it is where most setups go wrong. A Ø10 mm four-flute carbide end mill in aluminium wants roughly 0.05–0.10 mm per tooth in a full-width roughing pass. Drop that to 0.01 mm per tooth and the tool rubs instead of cutting, which work-hardens stainless and burns the edge. Feed rate is then spindle speed multiplied by number of teeth multiplied by chip load.

Read the chip. Aluminium should throw short, curled, silver chips. Long stringy chips mean the feed is too low for the speed, or the flute count is wrong for the material. Blue or straw-colored chips on steel mean the heat is high but the chip is carrying it away, which is fine in moderation. Fine gray powder means the tool is rubbing and the edge is about to fail.

Coolant and air blast are part of the same decision. Flood coolant carries heat away and clears chips on deep pockets. Through-spindle coolant helps above 5:1 depth-to-diameter, where chips otherwise pack at the bottom. On titanium and Inconel, high-pressure coolant is often the difference between a tool lasting 20 minutes and one lasting 2. On plastics and some magnesium alloys, air blast is safer than flood.

1
Aluminium 6061300–500 m/min surface speed, 0.05–0.10 mm per tooth on a Ø10 mm cutter.
2
Stainless 30480–120 m/min; keep chip load high enough to avoid work hardening.
3
Titanium and Inconel30–60 m/min with high-pressure coolant and rigid setups.
4
Read the chip color and shapePowder means rubbing; long strings mean feed too low.

Execution

Understanding CNC Machining in 7 Steps

Follow the order; skipping a step shows up as scrap later.

1
1. Review the drawing and release the DFMMark datums, the tightest tolerance, and the smallest internal radius. Flag any pocket deeper than 4× its width and any corner radius smaller than the cutter you plan to use. Our DFM analysis comes back with the quotation, usually within 12 hours.
2
2. Choose the machine and the number of setupsThree-axis for prismatic parts with features reachable from one or two directions. Four-axis when a part needs work on multiple sides of a cylinder. Five-axis when undercuts, compound angles, or a single-setup tolerance stack demand it. Fewer setups means fewer datum shifts.
3
3. Design the workholdingMatch the fixture to the cutting force, not to the part shape alone. Use soft jaws bored to the part diameter for round work, a fixture plate with support for thin plates, and tabs for parts that will be cut free. Check that the part cannot lift under the roughest pass.
4
4. Set zero and verify the rotary centerTouch off on the drawing datums. On five-axis work, indicate the rotary table with a test bar to within 0.005 mm before cutting. Record offsets in the setup sheet so the second operation repeats the first.
5
5. Rough with a planned stock allowanceLeave 0.5–1.0 mm on finish faces and 0.3 mm on bores. Use a larger cutter for bulk removal to reduce tool wear. Keep radial engagement moderate on long-reach tools; deflection grows with the cube of the length-to-diameter ratio.
6
6. Finish and inspect at the machineTake light finishing passes with fresh edges. Check critical dimensions with a micrometer or bore gauge before unclamping, because clamping stress can mask a size error. Adjust the offset and re-cut rather than re-fixturing the part.
7
7. Run final inspection and document itMeasure all drawing dimensions, record the results, and compare against the tolerance band. We inspect 100% of parts before shipment and can supply reports on request. If a dimension is borderline, decide before the part leaves the machine, not after.

Judgement

Which Machining Route Fits the Part

Pick the row that matches the feature, not the part category.

Part situation	Route	Typical tolerance	When it does not fit
Prismatic block, features from 1–2 sides	3-axis mill	±0.02 mm	Undercuts or side holes
Round part, multiple sides	4-axis mill	±0.01 mm	Compound angles
Undercuts, compound angles, one setup	5-axis center	±0.005 mm	Simple flat plates
Shaft with threads and diameters	Mill-turn center	±0.01 mm	Large prismatic bodies
Thin plate under 6 mm	3-axis + fixture plate	±0.02 mm	No flat backing available
Deep pocket above 4:1	3-axis + long-reach tool	±0.02 mm	Corner radius below tool size
Prototype, 1–20 pieces	3-axis or 5-axis, no tooling	±0.01 mm	Hard tooling already paid for
Production 10,000+ pieces	Die casting + machining	±0.05 mm	Tight flatness on large faces

FAQs

Common questions

How tight a tolerance can CNC machining hold in production?

On a controlled machine with stable temperature and proper workholding, ±0.005 mm is achievable on critical features, especially on aluminium and brass. Stainless and titanium are harder because of springback and heat.

The number that matters is the tolerance on the tightest feature, not the general note on the drawing. A part with a ±0.05 mm general tolerance and one 0.01 mm bore is quoted and inspected as a 0.01 mm part.

When should a design change instead of being machined?

Sharp internal corners, slots narrower than 2 mm and deeper than 8 mm, and threads under M2 are usually cheaper redesigned. Adding a corner radius equal to the cutter radius costs nothing and removes a finishing operation.

Deep narrow features also need long-reach tools, which deflect and force slower feeds. Widening a slot from 2 mm to 3 mm can cut cycle time noticeably.

What surface finish is realistic as-machined?

As-machined faces typically land at Ra 1.6–3.2 μm. A controlled finishing pass reaches Ra 0.8–1.6 μm, and fine finishing or polishing reaches Ra 0.2–0.8 μm on suitable materials.

Tighter finish usually means a separate finishing tool and a lighter pass, so it adds time. Specify finish only where the function needs it, such as sealing faces and bearing bores.

How does material choice affect the process?

Aluminium grades such as 6061-T6, 7075 and 6082 cut quickly and hold size well. Stainless 303 machines more freely than 304 or 316 because of its sulfur content, but it is less corrosion resistant.

Titanium TC4 and Inconel need lower surface speeds and high-pressure coolant. They are machined when the application demands the strength or heat resistance, not because they are easy.

What should be in the file sent for quotation?

Send a STEP or native CAD file plus a 2D drawing with datums, tolerances and finish callouts. Note the material grade, the quantity, and any surface treatment.

If a feature is functionally critical, mark it. That single mark tells the machinist where to spend setup time and where a general tolerance is enough.

Does a prototype run require different planning than production?

Prototypes skip hard tooling and often skip dedicated fixtures, so the setup is adjusted rather than built. Production runs justify fixtures that cut cycle time and improve repeatability.

We run from one prototype to 10,000+ part runs with no minimum order quantity, so the same drawing can move from prototype to production without a redesign.

Put the Steps to Work on Your Part

Send a STEP file and drawing and we will return a quotation with free DFM analysis, usually within 12 hours. Uploads stay confidential and an NDA is available on request.

12-hour quote100% inspectionNo minimum orderNDA on request

Get Instant Quote Talk to an Engineer