Choosing a machining process for titanium, nickel and hardened alloys

Why the process matters more here than anywhere else

On a mild steel or aluminium part, three-axis milling, turning and drilling cover almost everything, and the choice between them is close to free. Difficult alloys remove that slack. Titanium sheds heat so slowly that a poorly chosen setup burns tools rather than cutting metal; hardened steel above about 50 HRC stops most carbide outright; Inconel work-hardens under a light cut and turns the next pass into a harder problem than the first.

The result is that on these materials, which process — not just which machine — decides whether a part is routine or a redo. Three questions settle most of it: what hardness is being removed, how many features are on how many faces, and what the surface actually needs to do once the part is in service.

Milling, turning or grinding — how the alloy decides

	Best suited to	Struggles with
Milling (3-axis)	Prismatic parts, soft-to-medium alloys, features on few faces	Hardness above ~45 HRC, features on many faces
Milling (5-axis)	Complex geometry, features on multiple faces in one setup, thin walls that cannot survive repeated re-fixturing	Simple prismatic parts, where it adds cost with no accuracy gain
Turning	Rotationally symmetric parts, any hardness with the right insert	Non-round features, which still need a second operation
Grinding	Hardened parts needing a fine finish or tight roundness, after heat treatment	Stock removal — it is a finishing process, not a shaping one
Wire/sinker EDM	Hardened material, internal corners a cutter cannot reach, conductive alloys regardless of hardness	Non-conductive materials, and anywhere a cut edge is acceptable

None of these replace the others; a hardened tool-steel part routinely passes through three of them in sequence — milled soft, heat treated, then ground or wire EDM’d to final size — because each process is doing the part of the job the others cannot.

When 5-axis actually earns its price

Five-axis machining is quoted far more often than it is needed, and the question that separates a genuine case from an upsell is narrow: does the part have features on more than one face that must hold a relationship to each other — a bore square to a face on the opposite side, a pocket positioned off a datum that a re-fixture would lose? If yes, a single 5-axis setup removes the stack-up error that multiple 3-axis operations would introduce, and on titanium it also removes the repeated clamping that thin-walled parts do not tolerate well.

If the part is prismatic with everything on two or three faces that a sub-plate and a tombstone can reach, 3-axis in multiple operations is usually cheaper and just as accurate. The tell on a drawing is a callout for “5-axis machining” instead of the tolerance relationship that actually requires it — that phrasing prices in a specific machine rather than a specific result, and narrows the pool of shops able to quote it for no accuracy gained.

EDM: the process nobody budgets for until they need it

Wire and sinker EDM cut by spark erosion rather than a cutting edge, so hardness is irrelevant to them — they cut hardened tool steel and annealed aluminium at comparable rates for a given geometry. That makes EDM the answer to two problems milling cannot solve at all: a sharp internal corner behind a cutter’s radius, and any feature that needs to be cut after heat treatment without softening it back down.

The trade-off is speed and finish. EDM is slow per cubic millimetre removed, so it is a finishing or feature-completion process, never a roughing one, and a recast layer forms on the cut surface that some fatigue-critical parts require removing afterwards. Specify EDM where a corner radius genuinely cannot be opened up on the drawing; where it can, milling with a slightly larger radius is faster and cheaper for an identical function.

Hard turning against grinding, revisited

The two processes both finish hardened parts and are frequently interchangeable, which is exactly why the choice is worth making deliberately rather than by habit. Hard turning removes stock faster and does it in one setup on rotationally symmetric geometry; grinding holds tighter roundness and a finer finish, particularly past about 50 HRC where a turned surface starts to show tool marks under inspection. A shaft with a running fit typically wants grinding on the bearing diameters and hard turning everywhere else on the same part — not one process for the whole piece.

The mistake that costs more than the wrong process

The single most expensive habit on a drawing is specifying the process instead of the requirement: “5-axis machining,” “wire EDM,” “ground finish” written as an instruction rather than a consequence of a tolerance or a geometry. Every shop that reads that drawing prices in that specific process even where a cheaper one would meet the same callout, and the pool of shops able to quote it narrows to whoever owns that machine.

State the relationship or the finish that matters — true position between two features, a corner radius, a surface roughness — and let the shop propose the process. A published supplier standard exists partly for this reason: it lets a drawing describe the result once, instead of a different process assumption per shop.

For titanium specifically, each of these processes is worked through on one page, with starting data, failure modes and drawing notes: titanium machining processes.

Reading in this guide