CNC line EDM cutting explained

• 1
  Key takeaways
• 2
  How CNC line EDM cutting removes metal
• 3
  Which materials the process suits, and which it does not
• 4
  Tolerance, surface finish and the number of passes
• 5
  Design rules that decide whether the part can be cut
• 6
  Where the process earns its cost in production
• 7
  Wire EDM compared with milling and die-sinking EDM

The cutting tool is a thin wire, usually brass or coated brass, held under tension between two guides. The workpiece sits in a tank of deionized water. A generator pulses voltage between wire and work, and each pulse breaks down the dielectric in a small gap. That spark vaporizes a tiny amount of metal and leaves a crater behind. Hundreds of thousands of pulses per second add up to a cut.

Nothing touches the part. There is no cutter pushing into the material, so thin walls and delicate ribs do not deflect. That is the main reason a shop reaches for this process on hardened tooling or on features that would chatter under an end mill.

The wire never touches the workpiece either. A gap of roughly 0.02–0.05 mm stays open during roughing, filled with flowing water that flushes debris out of the kerf. If flushing fails, the wire breaks.

The controller moves the XY table and often the upper guide independently. By tilting the wire, the machine cuts tapered walls and ruled surfaces in one pass. Taper angles up to about ±30° are common on small heights, less on tall parts.

• 1
  Wire diameter0.15–0.30 mm for roughing, 0.05–0.10 mm for fine detail.
• 2
  DielectricDeionized water, resistivity kept around 5–20 MΩ·cm.
• 3
  GapSpark gap plus wire radius sets the offset the controller applies.

Any conductive material can be cut. Hardened tool steel, carbide, Inconel, titanium and copper alloys all work, and hardness has almost no effect on cut speed. A 60 HRC die block cuts at roughly the same rate as the same block in the annealed state. That is why the process is standard for press tools and extrusion dies after heat treatment.

Aluminium cuts quickly but is rarely the best choice. The thermal damage layer is thin, yet the process is slow compared with milling, and aluminium parts with simple geometry are cheaper on a 3-axis mill. Reach for EDM when the aluminium part has a sharp internal corner, a deep narrow slot, or a feature that must be cut after anodizing is ruled out.

Non-conductive materials are out. Plastics, ceramics and most composites cannot be cut because there is no current path. Carbon fibre is conductive in one direction only, so results are inconsistent and we usually route it to abrasive waterjet or milling instead.

• 1
  Good fitHardened steel, carbide, Inconel, titanium, copper and brass.
• 2
  Possible but check costAluminium and mild steel with simple geometry.
• 3
  Wrong processPlastics, glass, ceramics, most composites.

A single roughing pass leaves a recast layer and a rough surface, often Ra 3.2 μm or worse. To reach a fine finish, the machine makes a series of skimming passes with decreasing offset and energy. Each pass removes a few micrometres and improves the wall.

With the right number of passes and a stable setup, a wire EDM cut can hold ±0.005 mm and reach Ra 0.8–1.6 μm on the cut wall. Tighter finishes down to Ra 0.2–0.8 μm are possible on dedicated fine-finish machines, but they cost time. Each extra skim pass can add minutes to hours per profile.

Accuracy also depends on the part, not just the machine. A tall, thin wall will move as internal stress releases when metal is removed. For parts above roughly 100 mm tall, we often recommend a stress-relief anneal before the final cut, or roughing on one setup and finishing after a pause.

• 1
  Rough onlyFast, Ra 1.6–3.2 μm, useful for clearance profiles.
• 2
  Two to three passesBalanced cost and finish, common for production dies.
• 3
  Four or more passesFine finish and tight tolerance, slower per part.

Every closed profile needs a start hole drilled through the material. The wire threads through that hole and then cuts the outline. If a cavity is blind, with no through path, the wire cannot reach it, so blind pockets must be milled or sunk with a die-sinking EDM electrode instead.

Internal corners cannot be perfectly sharp. The smallest radius the wire can leave equals the wire radius plus the spark gap, so a 0.25 mm wire gives a corner radius near 0.15 mm at best. If your drawing calls for a true sharp corner, either accept the radius or add a relief feature.

Slots and ribs should stay at least 1.2× the wire diameter wide, and taller than about 0.5 mm. Below that, flushing is poor and wire breakage rises. Tapered features need clearance at the bottom of the part so the tilted wire does not clip the fixture.

• 1
  Start holeRequired for every closed profile; drill it 0.3–0.5 mm oversize.
• 2
  Corner radiusWire radius plus gap; typically 0.10–0.20 mm.
• 3
  Minimum slotAbout 1.2× wire diameter, and not less than 0.5 mm deep.

The economics change with batch size. For one prototype bracket, milling wins on speed. For a hardened punch with a 0.2 mm internal radius and a ±0.005 mm fit to its die block, EDM is often the only route that holds the tolerance at all.

The process also shines when a feature has to be cut after heat treatment. Hardening distorts a part slightly, so any critical profile machined before the furnace will drift. Cutting the profile after hardening removes that variable entirely.

In our Dongguan plant, wire EDM runs alongside 127 high-precision CNC machines, including 16 simultaneous 5-axis centers. Parts up to 4,000 mm can be handled across the shop, and the EDM cells take the hardened tooling and thin-wall work that milling cannot hold. Every part is inspected before shipment, and reports are available on request.

• 1
  Best batch fitOne-off hardened tooling, small runs of complex profiles.
• 2
  Weak fitHigh-volume simple parts; milling is faster and cheaper.