CNC Machining Explains: How Metal Removal Actually Works
This page is for design engineers and buyers who need to judge a machined part before sending it out. It covers how a cutting edge removes material, how tolerance and finish are held, and which geometry belongs on a 3-axis, 4-axis, 5-axis or mill-turn machine.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
What CNC machining explains about material removal
CNC machining is subtractive. A rotating cutter is driven along programmed paths, and metal leaves the blank as chips. Nothing is added, nothing is cast into shape. The geometry you get is limited by what the tool can reach and how stiff the setup stays while it cuts.
Every cut has three numbers behind it: cutting speed, feed per tooth, and radial depth of cut. Change one and the other two move with it. Aluminum 6061 runs fast, often above 300 m/min surface speed. Ti-6Al-4V runs slow and hot, so cutters stay in the 40–60 m/min range with heavy coolant.
The chip carries the heat away. If your feature is narrow and deep, chips recut and the tool rubs instead of cutting. That is why deep slots and thin ribs end up as slow, expensive geometry even when the drawing looks simple.
Climb milling leaves a better surface on most materials. The cutter engages thick-to-thin, pushing the workpiece into the table instead of lifting it. On a light finishing pass this matters more than spindle speed.
Which machine setup fits which part
A 3-axis machine moves X, Y and Z only. The workpiece stays fixed. It handles plates, housings, brackets and anything you can reach from one, two or three faces. If a part needs holes on four sides, 3-axis means multiple setups, and each new setup adds a position error.
A 4-axis machine adds rotation around one horizontal axis, either a rotary table or an indexer. Shafts, long brackets and parts with features around a bore become one-setup work. This is the sweet spot for a lot of production hardware, and it is cheaper per part than 5-axis.
A 5-axis machine adds two rotary axes, so the tool can tilt relative to the surface. Undercuts, compound angles, ports and deep cavities open up. One setup replaces four or five, which removes the stacked error from re-clamping. Our shop runs 16 simultaneous 5-axis machining centers alongside 12 four-axis mills and 27 three-axis machines.
Mill-turn centers do turning and milling in the same cycle. A part that starts as bar stock, gets turned to diameter and then needs cross-drilled holes or milled flats belongs here. We run 16 mill-turn centers, which is often the fastest route for connector bodies, valve stems and bushings.
How tolerance and surface finish are held
Tolerance is a stack, not a single number. Machine positioning, tool wear, spindle thermal growth, fixture deflection and material springback all push the part around. A ±0.005 mm callout (±0.0002 in) is achievable, but it needs the right feature geometry and a stable setup.
Not every dimension deserves a tight callout. A mounting hole pattern might need ±0.02 mm. A clearance slot might not care at ±0.1 mm. Tightening tolerance on a feature that does not need it adds inspection time and scrap risk without adding function.
Surface finish follows the same logic. As-machined surfaces sit around Ra 1.6–3.2 μm. A controlled finishing pass gets Ra 0.8–1.6 μm. Fine finishes down at Ra 0.2–0.8 μm usually mean slower feeds, smaller stepovers and sometimes a second operation.
Thin walls are the usual failure point. Below about 0.8 mm in aluminum, cutting forces start to deflect the wall and chatter shows up in the finish. Adding a temporary support rib or machining the wall in two passes usually fixes it.
Features that machine well and features that fight back
Internal corners are cut with a round tool, so the smallest radius in a pocket sets the smallest cutter the shop can use. A 2 mm corner radius on a 40 mm deep pocket forces a long, thin tool that has to run slowly. Open the radius to 6 mm and the same pocket cuts three times faster.
Thread depth matters too. A tapped hole should be at least 1.5× nominal diameter deep for full thread engagement, and blind holes need extra depth for the tap lead. M2 tapped holes in stainless are a known trouble spot and often get replaced with a pressed insert.
Deep holes follow a rule of thumb: depth over 5× diameter needs peck drilling or gun drilling, and depth over 10× diameter may need a dedicated deep-hole process. The chip has to get out, and coolant has to get in.
For parts that have to sit flat, a thin floor under a pocket will bow after the clamps come off. Leave 1.5 mm minimum floor for aluminum, more for steel, or design a rib pattern into the back.
Why the same part costs different in different metals
Aluminum cuts quickly. 6061-T6 is the default for machined parts because it holds tolerance, welds, anodizes and runs at high spindle speeds. 7075 gives more strength but machines with a sharper edge and is harder to anodize cleanly.
Stainless 304 work-hardens at the cut. Light passes with a dull tool raise surface hardness and the next pass gets worse. 303 machines far better and is the usual choice when corrosion resistance and machinability both matter. 17-4PH adds strength after heat treatment.
Titanium and Inconel sit at the hard end. Ti-6Al-4V conducts heat poorly, so the heat stays in the cutting edge. Tool life drops and cycle time rises several times over aluminum. Inconel is worse again. Budget for both time and tooling.
Plastics behave differently. POM and ABS cut clean but melt if the feed is too slow. PEEK needs sharp tooling and generous coolant. Carbon fiber is abrasive and eats carbide, so diamond-coated tools are common.
How you know the part is right
A machined part is only as good as its inspection. Raw material certificates come first, because a wrong heat of steel ruins the whole run. In-process checks catch drift before a batch is finished. Final inspection confirms the drawing before anything ships.
We inspect 100% of parts before shipment and provide reports on request. For tight features that means CMM measurement, not calipers. Calipers read a diameter but they will not tell you whether a bore is round.
First article inspection on a new program is the cheapest insurance you can buy. It catches a programming error on part one instead of part two hundred. After that, sampling keeps the process honest.
Our historical qualification rate is 99.99%. That number comes from checking everything, not from sampling a few parts and hoping.
Setup choice against part geometry and cost
Use this to pick a route before asking for a quote.
| Setup | Fits this geometry | Main limit | Relative cost |
|---|---|---|---|
| 3-axis | Plates, brackets, open pockets | One face per setup | Lowest per part |
| 4-axis | Shafts, parts with radial holes | No compound angles | Moderate |
| 5-axis simultaneous | Ports, undercuts, compound angles | Programming and machine time | Highest hourly rate |
| 5-axis 3+2 | Angled faces, many sides | Still one tool direction per pass | Between 4 and 5-axis |
| Mill-turn | Bar stock plus cross features | Part must start from bar | Low for round parts |
| Wire EDM | Sharp internal corners, hardened steel | Slow, thin sections only | High per part |
When to choose which route
If the part fits in one or two setups on a plate, use 3-axis and spend the money on fixturing. If it has compound angles, deep ports or features on five faces, go 5-axis and accept the higher hourly rate to kill setup error. If it starts as bar and needs cross features, mill-turn is almost always the cheaper answer.
Questions engineers ask next
Can you machine a part to ±0.005 mm on every dimension?
±0.005 mm (±0.0002 in) is achievable on a stable setup with the right feature geometry. It is not realistic on every dimension of a large, thin part at the same time.
Send the drawing and we will tell you which callouts drive cost and which ones can be relaxed without losing function.
What is the smallest internal corner radius you can cut?
The corner radius equals the tool radius, so a 1 mm corner needs a 2 mm cutter. Long, thin cutters deflect, so deep pockets with small corners run slowly.
Opening a 1 mm corner to 3 mm often cuts cycle time significantly with no change in function.
Do I need 5-axis for a part with holes on four sides?
Not necessarily. A 4-axis machine with a rotary table reaches four sides in one setup. 5-axis becomes worth it when you also have compound angles or need to tilt the tool into a cavity.
We quote both routes when the geometry allows it so you can compare cost.
How does material choice change lead time?
Standard aluminum and stainless stock is usually on hand, so production can start within 24 hours of order release. Titanium, Inconel and some tool steels may need to be ordered in.
Quotation and free DFM analysis come back within 12 hours, and most parts ship in 3–5 days after that.
What do you need to quote a machined part?
A 3D model in STEP or IGES plus a 2D drawing with tolerance, finish and material callouts. Tell us the quantity and any inspection report you need.
Uploads are secure and confidential, and an NDA is available on request.
Can you hold a fine finish on a large part?
Yes, up to 4,000 mm maximum processing size. Large parts need more care because thermal drift over a long cycle moves the cut.
Finishing passes are kept light and the part is checked before the final operation.
Send the drawing and get a straight answer
Quotation and free DFM analysis within 12 hours, no minimum order quantity, from one prototype to 10,000+ part runs.
12-hour quote100% inspectionNDA on request
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
