Internal corners are where CNC machining hits a hard physical limit: a rotating end mill cannot leave a perfectly sharp inside corner, because the cutter itself has a radius. When your design needs a true knife edge inside a pocket or slot — a seal seat, a mating shoulder, a thin web between features — that is when wire EDM enters the conversation. Knowing when it is worth the extra process step saves real money and lead time.
Why a mill always leaves a radius
A pocket corner milled with a 6 mm end mill leaves an internal radius of roughly 3 mm plus runout. Even small tools have limits: a 0.5 mm end mill is fragile, cuts slowly, and deflects, so "just use a smaller cutter" gets expensive fast below about R1.0 mm. The practical rule in most prototype shops: leave a corner radius at least 1–1.5× the end mill radius, and preferably design corners at R2–R3 mm so a standard 4–6 mm cutter can sweep through in one pass. Corner radii are one of those CNC machining details that quietly drive cost — every extra tool change to dig out small radii adds setup and machine time.
How wire EDM actually cuts a corner
Wire EDM erodes metal with a charged brass wire, typically 0.25 mm or 0.20 mm diameter (fine wires down to 0.10 mm exist for ultra-tight work). The smallest radius a wire can produce is its own radius plus a small spark gap — so a 0.25 mm wire leaves an internal corner radius around 0.15 mm. No cutting force touches the part, which matters as much as the geometry:
- Hardness is irrelevant. Hardened D2 at 60 HRC, carbide, or heat-treated die sections cut exactly like mild steel. That is why die casting mold inserts and punch dies go straight to wire EDM after heat treatment — no distortion, no re-machining.
- No burrs, thin walls OK. Because there is no mechanical load, delicate ribs and thin webs that would chatter or deflect under a mill come out clean.
- Deep is fine. Cutting a 100 mm deep narrow slot is routine for wire EDM and nearly impossible for a mill at tight tolerances.
Accuracy and surface finish compared
Modern wire EDM holds ±0.005 mm routinely, and a good skim pass gets closer to ±0.002 mm on critical dimensions. Surface finish after rough cutting is around Ra 1.6–2.0 µm; skimming (repeat passes at lower energy) reaches Ra 0.4–0.8 µm where needed. The trade-off nobody mentions early enough: the cut edge carries a thin recast layer — typically 5–15 µm of re-solidified material that is harder and can carry micro-cracks. For most structural parts it does not matter; for fatigue-critical or sealing edges, specify a skim pass or polish it off.
A milled surface, by contrast, is clean parent metal with cold-worked compression at the surface — often better fatigue behavior — but bounded by that corner-radius reality and a practical tolerance of ±0.01–0.02 mm in typical prototype work.
Cost and lead time: the honest numbers
Wire EDM is slow. Roughing moves at roughly 20–40 mm² per minute on common steels; a 20 mm thick pocket outline that a mill finishes in two minutes can take 40–90 minutes on the wire. Add skim passes and the cost scales accordingly. In practice:
- CNC milling: minutes per feature, setup-dominated, great for everything except sharp internal corners and hardened stock.
- Wire EDM: hours per feature in bad cases, but almost zero fixturing — the wire does not care how hard the part is or how thin the wall.
Wire EDM also requires the part (or a start hole) to be conductive and reachable by wire — no enclosed internal cavities, and taper is limited by the machine (typically up to ±15–30° depending on model).
A hybrid approach that usually wins
The most economical path for a part with a few critical sharp corners is almost never "all EDM" or "all milling." Rough and finish everything possible by CNC, then wire-EDM only the features that genuinely need it. Two practical tips make this smooth:
- Give the EDM shop start holes (2–3 mm drilled where the wire will thread) wherever the profile does not start from an edge. Drilled start holes cost seconds on the mill; cut from outside costs wire time and material.
- On your drawing, call out only the corners that must be sharp as R0.2 mm (or "sharp, per EDM"), and leave everything else at R1.0 mm or larger. Mixed callouts keep the expensive process in the small box where it belongs.
When to just change the design
Before sending a part to wire EDM, ask what the sharp corner is for. If it is a seal seat, a chamfered land or an inserted pin might do the same job and keep the whole part on the mill. If the corner exists only because the CAD file was exported from a casting draft, relax it to R2 mm and save a process step entirely. Many prototype reviews with an experienced shop start and end there — send the model, ask which corners actually carry function, and mill the rest.
