CNC Machining Processes: Which One Makes Your Part
The process is decided by the features on the drawing, and it decides which shops can quote. This page lays out what each CNC process makes, what it typically holds and what usually goes out to a specialist.
All tolerances and finishes below are typical ranges, not promises. The shop that quotes confirms what it holds on your geometry and material.
The processes, side by side
Ten processes cover almost every machined part. Most shops in Vietnam run the first four. The further down the table, the smaller the pool of shops that hold the machine in house.
| Process | What it makes | Typical tolerance | Typical Ra (µm) | What to know before you quote |
|---|---|---|---|---|
| 3 axis milling | Plates, brackets, housings, pockets and hole patterns reached from one side per setup | ±0.1 general, ±0.02 on fitted features | 1.6 to 3.2 | Every face reached from another side is another setup and another clamping error |
| 4 axis and 3+2 milling | Parts with features on several faces, hole patterns around a cylinder | ±0.05, ±0.02 on fitted features | 1.6 to 3.2 | A rotary table indexes the part, so four faces can come off in one clamping |
| 5 axis simultaneous milling | Contoured surfaces, impellers, compound angles, undercuts | ±0.02 to ±0.05 | 0.8 to 3.2 | Higher hourly rate, fewer setups. Worth it when the part would need four or more setups on 3 axis |
| CNC turning | Shafts, bushings, flanges, spacers, threaded ends | ±0.02 on diameters | 0.8 to 3.2 | Bar capacity through the spindle limits the diameter, not the chuck |
| Turn-mill (live tooling) | Turned parts with cross holes, flats, keyways or milled slots | ±0.02 on diameters, ±0.05 on milled features | 0.8 to 3.2 | Removes the second setup on a mill. Fewer machines than plain lathes |
| Swiss-type turning | Small, long or slender turned parts: pins, screws, connector bodies | ±0.005 to ±0.01 on diameters | 0.4 to 1.6 | Bar diameters typically up to about 20 or 32 mm. Economical from a few hundred pieces |
| Wire EDM | Punches, die openings, sharp internal corners, narrow slots, hardened parts | ±0.005 to ±0.01 | 0.4 to 1.6 with skim cuts | Conductive materials only. Slow per millimetre, so it is used where nothing else works |
| Sinker EDM | Blind cavities, ribs and sharp internal corners in mould and die steel | ±0.01 to ±0.02 | 0.8 to 3.2 | Needs a machined electrode first, which is a cost line of its own |
| Surface grinding | Flat faces with tight flatness or parallelism, hardened plates | ±0.005 | 0.2 to 0.8 | A separate operation after milling, often after heat treatment |
| Cylindrical grinding | Bearing seats, shaft journals, pins after hardening | ±0.005 or tighter on diameter | 0.2 to 0.8 | Specify it only on the diameters that need it, and leave the rest turned |
Tolerances are what a process typically holds on a well designed feature in aluminium or free machining steel. Hard materials, thin walls and long parts widen them. Fits are expressed in ISO 286 terms (engineering fits). The general tolerance classes are on the standards page.
Milling and turning carry most of the work
A milled part is held still and the cutter moves around it. A turned part spins and a stationary tool cuts it. Anything that is mostly round starts on a lathe, anything that is mostly prismatic starts on a mill, and a part that is both is where turn-mill machines and second setups come in.
The number of axes matters less than the number of setups. Each time a part is turned over and clamped again, the faces from the two setups are only as well aligned as the re-clamping. On a 4 or 5 axis machine the part stays clamped while the table turns, so faces line up better even at the same linear tolerance.
EDM and grinding finish what cutting cannot
Electrical discharge machining removes metal with sparks instead of a cutter, so it reaches sharp internal corners and hardened steel that a mill cannot. Wire EDM cuts through profiles like a band saw with a 0.1 to 0.3 mm wire. Sinker EDM burns a shaped electrode into a blind cavity.
Grinding is how a hardened part reaches a tight tolerance after heat treatment has moved it. A shaft that must run in a bearing is usually turned oversize, hardened, then ground to size on the journals only. If your drawing has both a hardness callout and a tolerance under ±0.01 mm on the same feature, expect a grinding line in the quote.
Which process each feature needs
Read your drawing feature by feature. The most demanding feature sets the process, and with it the shortlist of shops that can take the job.
| Part feature | Usual process | Watch for |
|---|---|---|
| Pocket with internal corners | Milling | The corner radius equals the cutter radius. A radius slightly larger than the cutter, and a depth up to about 4 times the width, keeps it cheap |
| Sharp internal corner | Wire or sinker EDM | If the corner does not need to be sharp, a relief cut (dog bone) lets a mill do it |
| Long slender shaft, length over 10 times diameter | Swiss-type turning or turning with a steady rest | Deflection under the cut. Tight runout on a long part is the expensive line |
| Cross hole or flat on a turned part | Turn-mill | Without live tooling it moves to a mill as a second setup |
| Bore to H7 | Reaming or boring | Standard reamer sizes are cheapest. An odd size is bored |
| Bore to H6 or tighter | Boring then honing, or grinding | Usually a separate operation and a separate machine |
| Internal thread | Tapping or thread milling | Thread depth of 1.5 times the diameter carries the load. Deeper adds cost and broken taps |
| Surface harder than about 45 HRC | Grinding or hard turning after heat treatment, or wire EDM | Heat treatment moves the part. Leave grinding stock on the features that matter |
| Thin wall under about 1 mm | Milling with care | Chatter and distortion. Fixturing and light cuts add time |
| Freeform or blended surface | 5 axis milling | Ask for the surface tolerance as a profile, not as linear dimensions |
Thread sizes and callouts are covered in the thread callout guide, and the question of when a part justifies a Swiss-type machine in the Swiss-type turning guide.
Design notes that change the process, and the price
Six drawing choices decide whether a part runs on a common machine in one or two setups or needs a special process. None of them change how the part works.
- Internal corner radiiGive every internal pocket corner a radius. A drawing with sharp internal corners either goes to EDM or comes back with a question.
- Hole and thread depthDrilled holes deeper than about 6 to 8 times the diameter need peck drilling or gun drilling. Threads beyond 1.5 to 2 times the diameter add little strength.
- Standard sizesStandard drill, reamer and thread sizes are tools the shop already has. An odd size is a special tool or a slower interpolated cut.
- Wall thicknessTypical practical minimums are around 0.8 mm in metal and 1.5 mm in plastic. Thinner walls are possible but are quoted as a risk.
- Number of setupsCount the directions a cutter must reach the part from. Each one is a setup, and each setup is a positional tolerance between faces.
- Tolerance where it fitsHold the fitted features tight and leave the rest to the general class. The process that holds ±0.005 mm is slower on every face it touches.
More examples with the cost effect of each change: design changes that cut machining cost. How tolerances map to price: tolerances explained.
Steps that usually go to a specialist
A machine shop machines. Heat treatment, coating and sometimes grinding are done by other companies down the road. That is normal and it is not a warning sign, but it adds days and a handover, and both belong in the plan.
When a quote comes back, ask which steps are in house and which are subcontracted, and who answers for the final dimensions after coating. The lead time guide shows where those days usually sit.
- Heat treatmentThrough hardening, case hardening and nitriding are usually done by a specialist furnace, not by the machine shop.
- Anodising and platingType II and hard anodise, zinc, nickel and chrome plating normally go to a finishing plant. Coating thickness changes fitted dimensions.
- PassivationSometimes in house for stainless work, often subcontracted. It removes free iron and adds no measurable thickness.
- Grinding and EDMIn house at some shops, subcontracted at others. Ask, because it decides who answers for the tolerance.
- Welding and assemblyWelded frames, press fits and sub assemblies are separate skills. Name them in the RFQ so they are quoted, not assumed.
How the process decides who we match
When an RFQ comes in we read the drawing first and work out which processes the part needs. That is the first filter: a part with a wire EDM profile goes only to shops that run wire EDM or name the shop that does it for them. A Swiss-type part goes to shops with sliding headstock lathes, not to a shop that would quote it on a conventional lathe at three times the cycle time.
Material and part size come next. The material side is on the materials page, and the sector side, with the paperwork each industry brings, is on the industries page.
What to state in the RFQ
- A 3D model (STEP) and a PDF drawing with tolerances
- Material grade and temper
- Any feature you know needs EDM, grinding or a special tool
- Hardness and when it applies, before or after machining
- Coating, with the faces to mask
- Quantity now and expected annual quantity
Questions about machining processes
Can one shop do milling, turning and EDM on the same part?
Some shops can, many cannot. A shop with mills and lathes is common, while wire EDM, sinker EDM and grinding are held by fewer shops or bought in from a neighbour. Name every process the part needs in the RFQ so we match shops that run all of them or that name their subcontractor up front.
Is 5 axis machining always more expensive than 3 axis?
The hourly rate is higher, but the part can be cheaper. A part that needs four or five setups on a 3 axis mill often costs less in one or two setups on a 5 axis machine, and the faces line up better because the part is not reclamped.
What tolerance should I expect from CNC turning?
Typically ±0.02 mm on diameters on a conventional CNC lathe and ±0.005 to ±0.01 mm on a Swiss-type machine for small parts. Tighter than that usually means grinding. These are typical ranges, and the shop that quotes confirms what it holds on your geometry.
Which operations are usually subcontracted?
Heat treatment, anodising, plating and powder coating are usually done by specialist plants. Grinding and EDM depend on the shop. A subcontracted step adds a few days and a transfer between two companies, so ask who carries responsibility for the final dimensions.
Know which processes your part needs?
Send the drawing and we match it with up to 3 shops in Vietnam that run those processes. You hear from us within 24 business hours.