Wire EDM vs CNC Milling: Corners, Slots and Hardened Steel

Two different ways of removing metal

Every other comparison on this site involves processes that cut. This one does not.

CNC milling removes material with a cutting edge. A rotating multi-tooth cutter is fed into the workpiece, the teeth shear off chips, and the shape is produced by moving the cutter along a programmed path. It is a mechanical process: force is applied, the material deforms and separates, and the tool wears.

Wire EDM removes material with electricity. A thin wire — usually brass, held under tension — passes through the workpiece while a controlled spark discharge jumps the gap between wire and work, melting and vaporising a tiny amount of material. The operation happens submerged in deionised water, which flushes the debris and controls the discharge. The wire never touches the part.

That difference in mechanism produces a set of consequences that no amount of process tuning can bridge.

	CNC milling	Wire EDM
Cutting mechanism	Mechanical shear	Thermal spark erosion
Tool contact	Yes	No
Internal corner radius	Tool radius — never zero	Essentially square
Hardened steel	Difficult; hard on tooling	Cuts as easily as soft
Cutting force on the part	Yes	None
Thin and delicate features	Deflect under load	No deflection
Material removal rate	High	Low
Bulk material removal	The right process	The wrong process
Materials	Any machinable material	Conductive materials only
Surface as cut	Machined	Recast layer; skim passes improve it
Start hole for internal profiles	Not required	Required
Accuracy	±0.01 mm on precision features	±0.01 mm, and tighter on a suitable profile
Machine rate	Lower	Higher
3D shapes and pockets	Routine	Not possible

The two rows that decide most specifications are the internal corner radius and the hardness. They are worth taking one at a time.

The internal corner: what only wire EDM can do

A milling cutter is a cylinder of finite diameter. When it cuts an internal corner, the tool sweeps a circle, and whatever the toolpath does, the corner it leaves is at least the radius of the cutter. A 6 mm end mill leaves a 3 mm radius. A 3 mm cutter leaves 1.5 mm. The radius can be made smaller by using a smaller tool, but it never reaches zero, and a smaller tool is slower, more fragile and limited in how deep it can reach.

That is a hard geometric limit, not a limitation of the machine or the operator. There is no milling strategy that produces a square internal corner.

A wire is a straight line of very small diameter, and it erodes along its own path. The corner it leaves is effectively square — the residual radius is on the order of the wire radius plus the spark gap, which is small enough that for most purposes the corner is sharp.

The practical significance is larger than it sounds, and it appears in a predictable set of applications:

• Dies and punches, where the profile of the cutting edge has to be sharp and the fit between punch and die depends on it
• Tooling and fixtures, where a component has to seat into a corner without a gap
• Keyways and splines with square internal corners
• Slots and narrow apertures where the width is close to the depth
• Parts that have to mate with a machined square feature

Where a drawing shows a square internal corner with no radius, the designer has specified a feature that only EDM can produce. If the corner has a tolerance on it, the specification is effectively naming the process. It is worth knowing that, because a shop quoting the part should either be using EDM or asking about the corner — a milled part will come back with a radius and be rejected, or worse, be accepted and not fit.

The converse is also worth stating: where a small radius is acceptable, milling is almost always the better process. Adding a corner radius to a drawing can move a part from the EDM machine to the mill, which changes the price and the lead time. That is one of the most useful single changes a designer can make, and it costs nothing functionally in most parts.

Hardness: cut the part after it is hard

Milling a hardened part is possible, but it is a poor experience for everyone. The material is abrasive, tool life collapses, cutting forces are high, and the part itself may move as internal stresses are released by the cut.

Wire EDM does not care. Because the material is removed thermally and the wire never contacts the surface, hardened steel machines at the same rate as soft steel. The hardness of the workpiece is irrelevant to the process.

That single fact reorganises the manufacturing route for a whole class of parts. The classic route for a die or a punch, or any part that has to be both accurate and hard, is:

1. Mill the shape in the soft condition, removing the bulk of the material while it is easy to cut
2. Heat treat the part to the required hardness
3. Wire EDM the critical profiles, corners, slots and apertures while the part is hard

This route gets the best of both processes. The bulk removal is done by the fast process on soft material. The accurate work is done by the process that is unaffected by hardness, after the heat treatment has finished moving the part — so the final dimensions are cut into the material in its final state, and the hardening distortion is already accounted for.

That last point is the one people miss. Hardening moves a part. Where a critical feature is machined before the heat treatment, the feature moves with the part and has to be corrected afterwards or accepted out of tolerance. Where it is wire EDM’d after hardening, it is cut to size on a part that has already finished moving. For a tight tolerance on a hardened component, that sequencing is worth more than the accuracy of either process on its own. The same logic governs the wider heat treatment route, which is covered on the heat treatment page.

No cutting force, and what that makes possible

Milling pushes on the workpiece. On a rigid block that is irrelevant. On a thin wall, a long slender feature or a delicate internal web, it is the dominant problem: the material deflects away from the cutter, the wall comes out tapered, chatter marks appear, and the dimensions are unreliable.

Wire EDM applies no mechanical force at all. The wire erodes the material across a small gap and never touches it, so there is nothing to push the part out of position. That makes it possible to cut:

• Very thin walls that would deflect or vibrate under a cutter
• Slender features with a high aspect ratio
• Delicate internal apertures where the remaining material is thin
• Small, close-together features where a cutter would not have room to work

This is the second reason wire EDM appears on parts that are not particularly hard. A thin-walled component with a precise profile is often a wire EDM job not because of hardness but because a cutter would push it around.

There is one further geometric capability worth knowing: a wire EDM machine with independent upper and lower wire guides can tilt the wire, which produces a tapered wall or a draft angle through the thickness. That extends the process beyond a straight 2D profile without turning it into a full 3D process.

The recast layer, and where it matters

EDM works by melting material, and melted material resolidifies. The surface left by the cut therefore carries a thin recast layer — sometimes called the white layer — which is harder and more brittle than the parent metal and may contain micro-cracks.

For most parts this is irrelevant. For two categories it is not:

• Fatigue-critical surfaces, where a brittle layer with micro-cracks is exactly the wrong thing to have at a highly stressed surface
• Surfaces that will be further processed, where the recast layer may affect a subsequent coating, plating or weld

The standard answer is skim passes. After the roughing pass, one or more finishing passes are run at lower power and with a smaller spark gap, which removes most or all of the recast layer and improves the surface finish considerably. A part cut with a rough pass and two skim passes has a very different surface from one cut with a rough pass alone.

Where the surface matters, that belongs on the drawing or in the enquiry. It is a specification decision rather than something the shop can infer from the geometry.

What the process needs before it can start

Two practical requirements that affect how a part is planned.

A start hole for internal profiles. The wire has to be threaded through the material to begin cutting an enclosed shape, so a small hole is drilled first — normally in the same setup that prepares the part. That hole is part of the process plan, and it has to exist before the EDM operation can run.

A conductive material. The process needs a circuit: wire, spark gap, workpiece, and the conductive path back. Steels, stainless, aluminium, copper alloys, titanium and conductive carbides all work. Plastics, ceramics and glass do not, because there is no conductive path. Where a part is made from a non-conductive material, milling is the process and the question does not arise.

For everything else, the EDM machining page covers the capability, and the grades we run are listed on the materials page.

Speed, cost and where each process actually wins

The cost comparison is not close in either direction — the two processes are good at different halves of the job.

Milling removes material fast. For bulk removal, pocketing, facing and 3D contouring, it is the only sensible process. Its rate is an order of magnitude above EDM’s in terms of material removed per hour, and where a part is mostly a shape cut out of a block, milling is the whole answer.

Wire EDM removes material slowly and at a higher machine rate. It is the most expensive way to remove a cubic centimetre of metal that exists. What it sells is not speed but capability: the square corner, the indifference to hardness, the absence of cutting force, and the accuracy on a profile.

So the practical routing is almost always a combination, and the question is which features go to which process:

• The bulk of the part — milled, in the soft condition
• The heat treatment — applied to the milled shape
• The critical profiles, corners, slots and apertures — wire EDM’d after hardening
• Any thin or delicate features — wire EDM’d, because a cutter would deflect them

Parts that are entirely wire EDM’d exist, but they are usually small, flat, profile-based components — a punch, a die insert, a precision flat part with an intricate outline — where there is no bulk to remove and the whole value is in the profile.

Where each process lives

CNC milling shows up as:

• Bulk material removal of any kind
• Pockets, faces, 3D contours and complex surfaces
• Holes, threads and tapped features
• Parts from non-conductive materials
• Anything where a corner radius is acceptable
• The soft-machining stage of a part that will be hardened

Wire EDM shows up as:

• Dies, punches and tooling where the profile has to be sharp — see fixtures and tooling
• Square internal corners, keyways and splines
• Narrow slots and intricate apertures
• Features on hardened parts, cut after heat treatment
• Thin-walled and delicate profiles that would deflect under a cutter
• Precision flat components where the profile is the whole part

The callout that belongs on the drawing

Instead of	Write
Square internal corner	State the corner radius, or state that it must be sharp
Internal corner, R0.5 acceptable	Say so — a radius may move the part to the mill and cut the cost
Hardened part, tight tolerance	Say that the critical features are to be cut after hardening
Slot, narrow and deep	State depth and width — the ratio decides the process
Thin wall, tight tolerance	Say so — a cutter will deflect it
Surface, fatigue-critical	Specify that the recast layer is to be removed by skim passes

The single most valuable line is the internal corner radius. Stating it — even to say it may be as large as R0.5 — can move a part from a slow thermal process to a fast mechanical one, and it is the single biggest cost lever on a profile-based component. Conversely, where a corner genuinely must be sharp, saying so tells the shop that EDM is required rather than leaving them to discover it after the first part is rejected.

Send the drawing with the material, the quantity and the corner requirements, and the quote comes back within 24 hours with DFM feedback — including a note where a radius change or a sequencing change would save cost without affecting function. Precision features are held to ±0.01 mm with ISO 2768-m as the general block — see tolerances we hold. Orders start at 50 pieces per style and material, samples from a single piece in 5–10 days, and every batch ships with a material certificate (MTR) tracing the grade to its mill heat plus pre-shipment photos.