Engineering · DFM
DFM best practices for Wire EDM.
Wire EDM does the things milling can’t — sharp internal corners, hardened materials, thin walls, and high-aspect features. The capability and design rules below.
01 · How it works
Spark-erosion, not cutting.
Wire EDM uses a thin metal wire (typically 0.010″ / 0.25 mm brass) flooded in dielectric fluid. Thousands of controlled electrical discharges per second erode material from the workpiece — without any mechanical cutting force. The wire never touches the part.
That single fact — no cutting force — is what gives EDM its unique capabilities: it doesn’t care if material is hardened, won’t deflect thin walls, and traces a path with no tool radius to leave behind.
02 · When to use
EDM beats milling when one of these is true.
Pick EDM when:
- Sharp internal corners requiredWire follows the geometry — no tool radius. Square pockets, sharp keyways, broached profiles done in one operation.
- Material is hardened post-cutEDM doesn't care about hardness. Tool steels at 60+ HRC and hardened stainless cut at essentially the same rate as soft material. Carbide cuts too, but slower — roughly 30% of the tool-steel rate.
- Thin walls or websNo cutting force = no deflection. Walls down to 0.005″ (0.13 mm) are routine.
- High aspect ratio features10:1, 15:1, even 20:1 wall heights are stable. Milling chatter limits these around 3–5:1.
- Profile tolerance is criticalTrue profile tolerance — no tool deflection or wear during the cut.
- Mating male/female pairsCut both halves from one master path with offsets. Fits perfectly the first time.
Pick milling when:
- Bulk material removalEDM is slow at removing volume. For pockets that mostly need to be empty space, mill first — EDM only the difficult features after.
- Cylindrical bores or threadsEDM cuts profiles, not bores. Use a lathe or boring head for round holes; tap or single-point for threads.
- 3D contoured surfacesWire EDM is essentially 2.5D — it cuts a profile that may taper. For 3D surfaces, you want a 5-axis mill.
- Cosmetic surfacesEDM leaves a recast layer. Cosmetic surfaces typically need a milled finish or post-EDM polish.
- Non-conductive materialPlastics, ceramics (without conductive coating), and most composites can't be EDM'd. They mill fine.
- Production volumePer-part time on EDM is rarely competitive at high volume unless EDM is the only way to make the feature.
03 · Corners & radii
Sharp corners are the headline feature.
The minimum internal corner radius is set by the wire radius plus the spark gap — it’s effectively half the kerf. With a standard 0.010″ wire, the smallest internal radius is about 0.006″ (0.15 mm). Smaller wires push that down to roughly 0.004″ (0.006″ wire) or 0.0025″ (0.004″ wire) if needed.
Compare that to milling, where the corner radius equals the cutter radius: ~0.030″+ is possible with small end mills, and 0.060″+ is the economical minimum. EDM’s sharp corners are 5–10× tighter than what an endmill can produce.
04 · Aspect ratio
Tall, narrow features are EDM territory.
Because there’s no cutting force, EDM holds tolerances on tall, thin features that milling can’t touch. A 0.020″ wide slot 0.500″ deep (25:1 aspect ratio) is routine. Milling that geometry would require a 0.020″ endmill — which has roughly 0.080″ of usable reach before chatter becomes inevitable.
05 · Surface finish
More passes = better finish (and more time).
A first cut (rough pass) leaves a Ra around 64 µin and a small recast layer. Each subsequent skim pass — done with reduced energy — improves the finish and removes recast. Going from rough to mirror requires a 4-pass skim cycle, each pass adding time.
For most aerospace and tooling work, a 1–2 skim cut is the sweet spot — Ra 8–16 µin with reasonable time. Mirror finishes (4 µin Ra) require a 4-pass skim cycle and are usually called out only on functional surfaces.
06 · Materials
Conductive only — but hardness doesn’t matter.
EDM-friendly materials
Anything electrically conductive. Hardness doesn’t affect cut speed.
- ·Tool steels (A2/D2/S7/H13)
- ·Hardened steels (any HRC)
- ·Stainless (300/400 series)
- ·Aluminum (all alloys)
- ·Titanium (any grade)
- ·Inconel & Hastelloy
- ·Carbide (tungsten)
- ·Copper / brass
- ·PCD inserts
- ·Beryllium copper
- ·Nimonic
- ·Permalloy / Mu-metal
Watch out
Conductivity matters; some "metals" cut poorly or risk wire breakage.
- Plastics & ceramics: Don’t conduct. Use mill or grind instead.
- Cast iron: Porosity and graphite inclusions can break the wire. Sand-cast worse than ductile.
- Sintered or PM parts: Density variations cause inconsistent cut and wire risk.
- Aluminum: Cuts fast but the recast layer is thicker. More skim passes needed for fatigue-critical parts.
- Heat-affected zone (HAZ): Every EDM cut leaves a 0.0005–0.002″ HAZ. Critical fatigue parts may need post-cut polish.
07 · Combined ops
EDM works best as part of a sequence.
Wire EDM is rarely the single operation that produces a finished part — it’s usually one step in a sequence. The most common patterns:
Mill bulk → EDM details
Mill the rough envelope and any easy features. EDM only the sharp corners, thin webs, or features the endmill can’t produce. Saves hours of EDM time.
Mill → harden → EDM
Mill near-net while soft, heat-treat to final hardness, then EDM the precision features. Eliminates post-heat-treat distortion in the critical features.
EDM master path
Cut the male and female halves of a mating pair from the same toolpath using offsets — 0.0001″ fits achievable in the same machine, same setup.
EDM start hole + path
For closed-contour interior cuts (cutouts inside a part), the workflow is: mill or drill a small start hole → thread the wire → cut the closed contour. Designed in early, free; added later, expensive.
Stack cutting
Multiple parts (often identical) clamped together and cut as a stack. Common for thin gaskets, laminations, or small lots of identical features.
Roughing pre-cut
For very deep features in expensive material, mill or drill a chip-clearing path first to reduce EDM time and wire consumption.
Cost shape
What drives EDM cost.
EDM is priced by machine-hour. The geometry, material, and finish requirements all roll up into time. The four levers that move per-part cost the most:
Stack height
Cut speed scales inversely with thickness. A 1″ stack takes 2× the time of a 0.5″ stack — same path.
Path length
Total wire travel (perimeter + skim passes). Long contours cost more than short ones.
Number of passes
Each added skim pass adds significant time — see the chart above (≈1.3× for one skim, 1.7× for two, 2.9× for a four-pass mirror finish). Don’t spec mirror finish unless required.
Setup complexity
Multi-position fixturing, start holes, custom wire angles — each adds setup overhead.
Also in DFM
Designing for CNC machining is a different conversation.
Tool reach, pocket geometry, drill standards, threading rules, and the patterns that drive milling and turning cost. The companion reference for CNC.
Have a part with sharp corners or hardened material?
Tell us about your part and we'll get back to you promptly. Aerospace, medical, defense, and semiconductor production work welcome.Email CAD models and drawings to sales@digitalmachine.com, including ITAR, EAR, CUI and AS9100 work. Keep controlled technical data out of web forms.
First articles through full production runs