Quick Answer: Machining processes are manufacturing methods that remove material from a workpiece to produce a finished part at a specified geometry, tolerance, and surface finish. The main types are: CNC turning (cylindrical parts, concentricity ≤0.010–0.020 mm), CNC milling (prismatic and complex 3D geometry, ±0.020–0.050 mm general), drilling (hole creation, ±0.050–0.100 mm), grinding (ultra-high precision, ±0.001–0.005 mm, Ra <0.4 µm), broaching (internal profiles — keyways, splines — in a single pass), EDM (hardened materials above HRC 50 and sharp internal corners), and laser machining (thin-section profiles and sheet metal). No single process is optimal for all requirements. The governing selection logic is: geometry determines the primary process (rotating parts → turning; multi-face parts → milling); tolerance tightens the process (below ±0.005 mm → grinding or EDM); and material condition constrains the options (hardened steel above HRC 50 → EDM because cutting tools wear rapidly). Mismatching process to part geometry typically adds 20–50% to machining cost.
Why Different Machining Processes Exist
The variety of machining processes reflects the variety of engineering requirements that no single cutting method can satisfy simultaneously. Each process is optimized for a specific combination of geometry, material behavior, and accuracy level.
Geometry drives the primary selection: A shaft that must be concentric to ±0.010 mm across three bearing journals is not efficiently produced by milling, which would require the part to be repositioned three times with accumulated fixturing error at each step. The same shaft produced by CNC turning, where all three journals rotate on the same spindle axis, inherits the spindle’s concentricity naturally. Conversely, a bracket with flat mounting faces, threaded holes at multiple angles, and a pocket with an internal radius cannot be produced by turning — there is no sensible rotation axis for that geometry.
Material condition limits tool-based processes: Conventional machining processes — turning, milling, drilling, grinding — require a cutting tool harder than the workpiece. When steel is hardened to HRC 50–60 (tensile strength approximately 1,800–2,000 MPa), carbide cutting tools can still cut but at very low speeds with rapid wear. At HRC 60+, some hardened steels and ceramics become impractical for conventional cutting. EDM removes material by electrical spark erosion — the process has no cutting force and is independent of workpiece hardness. This is why mold and die cavities are roughed by milling (before hardening) and finished by EDM (after hardening).
Tolerance requirements add secondary constraints: Turning and milling produce tolerances of ±0.010–0.050 mm as production standards. For precision bearings, hydraulic sealing surfaces, and gauge applications requiring ±0.001–0.005 mm, cylindrical grinding, surface grinding, or jig grinding are used as finishing operations after turning or milling establish the basic geometry.
The Main Types of Machining Processes
CNC Turning
CNC turning rotates the workpiece on a spindle while a stationary cutting insert removes material from the OD, ID, or face. Because all features cut in one setup share the same rotation axis as their geometric reference, CNC turning naturally produces concentricity between diameters of 0.005–0.020 mm TIR — a level that milling cannot match without complex fixturing.
Best for: Shafts, pins, bushings, hydraulic fittings, fasteners, connectors — any component where the primary features are diameters along a central axis, and where concentricity between those features is functionally important.
Typical capability: Diameter tolerance ±0.010–0.025 mm in production; surface finish Ra 0.8–1.6 µm on finish turning passes; concentricity 0.005–0.020 mm TIR between features in the same setup.
Live tooling: Turning centers with live tooling (rotating mill/drill tools in the turret) can add keyways, cross-drilled holes, and flats to a turned part without re-fixturing, combining turning and milling in a single setup.
CNC Milling
CNC milling moves a rotating multi-flute cutting tool across the workpiece surface in the X, Y, and Z axes (3-axis), with additional rotary axes in 4-axis and 5-axis configurations. The tool’s ability to approach the workpiece from any direction makes milling the process of choice for prismatic parts with multiple faces, pockets, angular features, and complex 3D contours.
Best for: Housings, brackets, plates, mold cores and cavities (pre-hardening), structural aerospace components with complex contours, and any part where the primary features are flat surfaces, pockets, and multi-directional holes.
Typical capability: ±0.025–0.050 mm in general production; ±0.010–0.025 mm with careful setup and verification on critical features; surface finish Ra 0.8–3.2 µm depending on operation and tooling; angular features to within ±0.010–0.025 mm.
5-axis advantage: 5-axis machining allows the tool to tilt relative to the workpiece, enabling complex angular and contoured surfaces in fewer setups. This is particularly valuable for aerospace components with compound angles, impellers, turbine blades, and mold cavities with deep features requiring short, rigid tools at non-vertical angles.
Drilling
Drilling creates holes by advancing a rotating drill bit along its axis into the workpiece. It is the fastest method for hole creation but produces the lowest hole quality of the standard processes: diameter tolerance typically ±0.025–0.075 mm, surface finish Ra 3.2–6.3 µm, and potential departure from circularity of 0.025–0.075 mm.
Role in the production sequence: Drilling’s primary function is to create a hole that provides a starting condition for finishing operations (reaming to achieve ±0.010–0.025 mm tolerance and Ra 0.8–1.6 µm, or boring to achieve similar results with better positional control), or to create clearance holes and tap drill holes that do not require precision finishing.
Grinding
Grinding removes material using abrasive grains bonded in a wheel, with each grain acting as a miniature cutting tool removing an extremely thin chip. Because each grinding pass removes very little material (0.005–0.025 mm depth per pass is typical), the process can achieve dimensional accuracy and surface finish that cutting tools cannot match.
Typical capability: Cylindrical grinding achieves ±0.001–0.005 mm on diameter, roundness within 0.001–0.002 mm, and surface finish Ra 0.1–0.4 µm. Surface grinding produces flatness within 0.002–0.005 mm and finish Ra 0.2–0.8 µm. These figures represent an order of magnitude improvement over turning and milling.
Production sequence position: Grinding is used as a finishing operation after turning or milling has established the basic geometry and brought the part to within approximately 0.05–0.20 mm of final size. Grinding to final dimension from rough stock is economically impractical because the material removal rate is too low.
Common applications: Bearing seats on shafts (H7/g6 or H6/j5 fits requiring ±0.002–0.008 mm), hardened tool steel surfaces, precision gauge references, lapping and superfinishing of sealing surfaces, and any application requiring Ra below 0.4 µm.
Broaching
Broaching uses a multi-tooth cutting tool (broach) with progressively deeper teeth that each remove a small chip as the broach is pulled or pushed through the workpiece in a single linear stroke. The final broach tooth defines the finished geometry — all teeth in the tool cut in one pass.
Best for: Internal profiles that cannot be produced efficiently by rotary tools: keyways in hubs and bores, internal splines for power transmission components, non-circular bores, and surface broaching of flat faces on production volumes where cycle time matters.
Typical capability: Keyway width tolerance ±0.010–0.025 mm; internal spline tooth spacing ±0.010–0.020 mm; surface finish Ra 0.4–1.6 µm depending on broach condition. Broaching is a high-speed operation (a complete keyway produced in 2–5 seconds in production) but requires dedicated, expensive tooling that is not economical for small batches.
EDM (Electrical Discharge Machining)
EDM removes material by precisely controlled electrical discharge (spark) between the tool electrode and the workpiece — there is no mechanical cutting force, and the process is entirely independent of workpiece hardness. Material is removed as micro-droplets ejected by the spark, leaving a characteristic textured surface (the “spark eroded” finish) with fine, uniform texture.
Wire EDM cuts two-dimensional profiles through the workpiece by a continuously fed wire electrode (typically 0.20–0.30 mm diameter brass or coated wire), producing positional accuracy of ±0.002–0.005 mm on profile location. Sinker (Ram) EDM uses a shaped electrode machined to the negative of the desired cavity geometry, eroding the workpiece to the electrode shape with dimensional accuracy of ±0.003–0.010 mm.
Best for: Hardened tool steel mold cavities and die inserts (roughing by milling before hardening, finishing by EDM after hardening); internal profiles with sharp corners that milling cannot achieve (milling always leaves a radius equal to the tool radius at internal corners; EDM can produce corners approaching 90°); thin-wall features in hard materials where cutting force would deflect or break the part.
Limitation: EDM material removal rate is much slower than milling — typical EDM removal rates are 0.1–5 cm³/hour compared to 50–500 cm³/hour for milling in steel. EDM is economical only when conventional processes cannot meet the geometric or material requirements, or when the surface quality specific to EDM (fine uniform texture) is functionally required.
Laser Machining
Laser machining uses a focused, high-intensity laser beam to melt, vaporize, or ablate material from the workpiece surface. For 2D profile cutting of sheet metal and thin plate, laser cutting competes directly with plasma cutting and waterjet cutting in the 1–25 mm thickness range.
Best for: Complex 2D profiles in sheet metal (1–20 mm thickness for CO₂ and fiber lasers); precision profiling where heat-affected zone must be minimized; non-contact cutting of hard, brittle, or heat-sensitive materials; and marking, engraving, and ablation operations where very small features are needed without mechanical contact.
Limitation: Laser cutting is a 2D process for sheet stock — it cannot produce the 3D features that milling and turning create. The heat-affected zone (HAZ) around the cut edge affects material properties and surface hardness in metals, requiring post-processing in applications where edge metallurgy is critical.
Conventional vs Non-Conventional Machining
The distinction between conventional and non-conventional machining is mechanistic: conventional processes remove material through mechanical cutting action (tool edge harder than workpiece); non-conventional processes remove material through energy input (electrical, chemical, thermal, or acoustic) without relying on mechanical cutting.
| Factor | Conventional Machining | Non-Conventional Machining |
|---|---|---|
| Material removal mechanism | Mechanical cutting by tool | Spark, laser, electrochemical, ultrasonic |
| Tool-workpiece contact | Direct contact | Minimal or no contact |
| Applicability to hard materials | Limited above HRC 60 | Independent of workpiece hardness (EDM) |
| Material removal rate | High (50–500 cm³/hr for milling) | Low (0.1–5 cm³/hr for EDM) |
| Cutting force | Present; causes deflection in thin parts | None (EDM, laser); may cause cracking (ultrasonic) |
| Sharp internal corners | Not achievable (always leaves tool radius) | Achievable approaching 0° (EDM) |
| Typical cost | Lower | Higher (slow, specialized equipment) |
The selection principle: Use conventional machining unless there is a specific technical reason it cannot meet requirements. The technical reasons to switch to non-conventional are: (1) material hardness above HRC 50–55 where conventional tools wear rapidly; (2) geometry including sharp internal corners (below the minimum tool radius achievable); (3) thin walls or delicate features where cutting force would cause deflection or fracture; (4) materials that are unsuitable for cutting (ceramics, composites, some heat-treated alloys).
Process Selection by Tolerance and Surface Finish Requirement
| Process | Typical Diameter/Profile Tolerance | Surface Finish (Ra) | Typical Application |
|---|---|---|---|
| Drilling | ±0.025–0.075 mm | Ra 3.2–6.3 µm | Through holes, clearance holes, tap drill |
| CNC Turning (general) | ±0.025–0.050 mm | Ra 1.6–3.2 µm | Roughing and semi-finishing passes |
| CNC Turning (finish) | ±0.010–0.025 mm | Ra 0.8–1.6 µm | Bearing journals, precision fits |
| CNC Milling | ±0.020–0.050 mm | Ra 0.8–3.2 µm | Housings, brackets, prismatic parts |
| Reaming | ±0.010–0.025 mm | Ra 0.8–1.6 µm | Precision bore finishing |
| Grinding (cylindrical) | ±0.001–0.005 mm | Ra 0.1–0.4 µm | Bearing seats, precision shafts |
| Wire EDM | ±0.002–0.005 mm | Ra 0.4–1.6 µm | Profile cutting in hardened materials |
| Sinker EDM | ±0.003–0.010 mm | Ra 0.4–3.2 µm | Mold cavities, die inserts |
| Broaching | ±0.010–0.025 mm | Ra 0.4–1.6 µm | Internal profiles (keyways, splines) |
The cost of tighter tolerances: Each step tighter in tolerance requires additional process steps, slower material removal, and longer inspection time. Moving from ±0.050 mm (general milling) to ±0.010 mm (precision turning or milling) typically increases machining cost by 30–80%. Moving from ±0.010 mm to ±0.002 mm (cylindrical grinding) may double cost again. The engineering discipline is to specify the loosest tolerance that the application function genuinely requires, applying tight tolerance callouts only to features where fit, alignment, or sealing depends on that precision.
Common Process Combinations for Real Parts
Shaft (automotive transmission or machine tool): CNC turning for all diameters, shoulders, threads, and grooves → cylindrical grinding of bearing seat diameters to ±0.002–0.005 mm.
Hydraulic valve body: CNC milling for external geometry, bores, and fluid passages → drilling for all holes → reaming for precision bore seats (±0.010–0.020 mm) → surface grinding of sealing faces.
Injection mold insert: CNC milling for roughing and semi-finishing the cavity geometry before heat treatment → sinker EDM for final cavity details, sharp corners, and textured surfaces after hardening → hand polishing or surface finishing to Ra specification.
Gear hub with internal spline: Turning for external geometry → broaching for internal spline (2–5 second cycle time in production) → grinding of external diameter if bearing fit required.
Aerospace aluminum structural bracket: 5-axis CNC milling for complete external and internal geometry in a single setup → reaming for bushing and fastener holes → anodizing.
DFM Considerations for Process Selection
Design for the correct primary process: Parts that are predominantly cylindrical should have their design finalized to allow CNC turning as the primary operation. Adding asymmetric features (flats, offset holes, complex pockets) to what would otherwise be a turned part significantly increases cost by requiring live tooling, secondary milling, or multiple machine transfers. If the function of the part requires cylindrical features (bearing journals, threads) plus non-rotational features (bolt flanges, mounting brackets), evaluate whether the part can be manufactured as a turning-based part with live tooling or whether it should be redesigned as two parts.
Internal corners: CNC milling always leaves a radius at internal corners equal to the tool radius. For mold cavities, gear pockets, and dies where sharp internal corners are required, the CAD geometry must either accept the minimum radius achievable by the smallest practical end mill (typically R0.5–1.0 mm), or the design must be modified to use a dog-bone relief at corners, or EDM must be specified for corner finishing. Specifying sharp internal corners without a manufacturing method capable of producing them creates an unresolvable manufacturing conflict.
Tolerance allocation between processes: When a production sequence uses multiple processes in series (e.g., turning + grinding), the tolerances allocated to each step must account for the subsequent process’s capability. The rough turning stock allowance for subsequent grinding is typically 0.050–0.200 mm per side. If the rough turning tolerance is ±0.050 mm, the grinding must accommodate parts at the lower end of the allowance (less material to remove) and the upper end (more material), while still achieving the ±0.002–0.005 mm final tolerance. This must be analyzed in the process plan, not just in the final drawing callout.
Key Takeaways
- Geometry is the primary filter for process selection: rotating/cylindrical parts belong on CNC turning; prismatic/multi-face parts belong on CNC milling; the assignment of the wrong process to the geometry adds 20–50% to machining cost without improving quality.
- Tolerance is the secondary filter: turning and milling cover ±0.010–0.050 mm in production; grinding extends capability to ±0.001–0.005 mm; EDM achieves ±0.002–0.010 mm and is independent of workpiece hardness.
- Material hardness constrains the process above HRC 50: conventional cutting tools wear rapidly in materials above HRC 50–55; EDM is the primary alternative for hardened mold steel, die steel, and hardened precision components.
- Most real parts require a combination of processes: a shaft requires turning + grinding; a mold insert requires milling + EDM; a hydraulic valve body requires milling + drilling + reaming. Process selection should be done at the assembly/component level, not just for individual features.
- Over-specifying tolerances is the most common cost driver: applying ±0.005 mm tolerances to non-functional features forces grinding steps where turning or milling would be adequate, adding 50–100% to machining cost for no functional benefit.
- Non-conventional processes (EDM, laser, ECM) are specialty tools, not general upgrades: they solve specific constraints (hardness, sharp corners, no cutting force) at substantially higher cost per unit volume removed. Using EDM for a part that conventional milling could produce adds cost and lead time without performance benefit.
- For OEM procurement teams: the most valuable information to provide to a machining supplier is not just the final tolerance, but also the functional reason for each tight tolerance — bearing fit, hydraulic seal, locating pin clearance. This context allows the supplier to select the appropriate process and optimize the process sequence, rather than applying the tightest available process uniformly to meet uncontextualized tolerance callouts.
Frequently Asked Questions
What are the main types of machining processes?
The main machining processes used in industrial manufacturing are: CNC turning (rotating workpiece, stationary tool — for shafts, pins, bushings, and cylindrical components); CNC milling (rotating tool, moving workpiece — for housings, brackets, and prismatic components); drilling (axial hole creation); grinding (abrasive finishing for ±0.001–0.005 mm precision); broaching (single-pass internal profile cutting for keyways and splines); EDM (spark erosion for hardened materials and sharp internal corners); and laser machining (2D profile cutting of thin materials). Each process has a geometry and accuracy envelope within which it performs efficiently. Selecting the wrong process for the geometry increases cost without improving quality.
How do I choose between CNC turning and CNC milling?
The decision is driven by part geometry. CNC turning is correct when the part’s primary features — the ones that determine function — are diameters, shoulders, threads, and grooves along a central axis, and when concentricity between features is a functional requirement. CNC milling is correct when the primary features are flat surfaces, pockets, multi-directional holes, and complex 3D contours. The production cost consequence of the wrong choice: machining a cylindrical shaft on a milling center (instead of a lathe) requires multiple setups, accumulates concentricity error between setups, and takes 2–3× longer than turning. Machining a complex housing on a lathe is not feasible. For parts that are primarily cylindrical but include secondary milled features (keyways, flats, cross-holes), a turning center with live tooling produces both in a single setup.
What tolerances can each machining process achieve?
The practical production tolerance ranges are: drilling ±0.025–0.075 mm on diameter; CNC turning (finish) ±0.010–0.025 mm; CNC milling ±0.020–0.050 mm; reaming ±0.010–0.025 mm; cylindrical grinding ±0.001–0.005 mm on diameter; wire EDM ±0.002–0.005 mm on profile position; sinker EDM ±0.003–0.010 mm. These figures represent typical production capability with appropriate tooling and process controls — they are achievable consistently in a production environment, not just on individual test parts. Tighter tolerances are possible but require additional process steps, temperature-controlled environments, and more intensive inspection, increasing cost substantially.
When is EDM necessary instead of conventional machining?
EDM is necessary — not just beneficial — in three situations: (1) The workpiece has been hardened above approximately HRC 50–55, where conventional cutting tools wear rapidly and produce inconsistent results. This is the standard case for finishing injection mold cavities, die inserts, and precision tooling components, which are always machined to rough geometry before hardening and then finished by EDM after hardening. (2) The geometry requires sharp internal corners that conventional end mills cannot produce — milling always leaves a radius at least equal to the tool radius. EDM can approach 0° internal corners. (3) Thin walls, delicate features, or fragile parts where conventional cutting forces would cause deflection or fracture. EDM has no cutting force, producing these features without mechanical loading. For parts that do not meet one of these three criteria, conventional machining is almost always more economical.
What is the difference between conventional and non-conventional machining?
Conventional machining (turning, milling, drilling, grinding) removes material through mechanical cutting — a tool harder than the workpiece shears chips from the surface. The process is limited by tool hardness relative to workpiece hardness, cutting force (which causes deflection in thin parts), and the inherent radius that a rotating tool leaves at internal corners. Non-conventional machining (EDM, ECM, laser, ultrasonic) removes material through energy input — electrical spark, electrochemical reaction, photon energy, or acoustic energy — without relying on mechanical cutting. The key practical advantages: EDM and ECM are independent of workpiece hardness; EDM produces no cutting force; laser and EDM can produce features inaccessible to rotating tools. The key limitations: non-conventional processes remove material far more slowly than cutting (EDM at 0.1–5 cm³/hour vs milling at 50–500 cm³/hour) and cost more per unit of material removed. They are used selectively where conventional methods cannot meet the requirement, not as general replacements.
Written by the CMS engineering team with 15+ years of precision CNC machining experience producing components by turning, milling, grinding, EDM, drilling, and broaching for aerospace, automotive, medical device, industrial automation, and tooling OEM manufacturing programs. Technical references: Kalpakjian S. and Schmid S.R. — Manufacturing Engineering and Technology (Machining Processes chapters), Machinery’s Handbook (Cutting Speeds, Feeds, and Tool Life), ASM Handbook Vol. 16 (Machining — Process Selection), SME Tool and Manufacturing Engineers Handbook Vol. 1 (Machining).
Sourcing Precision CNC Machined Components Across Multiple Processes?
At CMS, we provide CNC turning, milling, drilling, reaming, and surface treatment in integrated production programs — with process selection guidance at the quoting stage, DFM review for geometry-process matching, and CMM first-article inspection.
[Request a process selection review and machining quote →]
