KEY TAKEAWAYS

✓
CNC machining is faster and cheaper for most geometries — default to it unless your part has features that cutters physically cannot reach.

✓
EDM is the right tool for hardened materials, deep narrow slots, sharp internal corners, and complex through-cavities where mechanical cutting fails.

✓
Wire EDM holds tolerances down to 0.0001 inch and leaves no cutting forces — critical for thin walls and fragile features.

✓
EDM cycle times are slow; for high-volume production, it is rarely cost-effective unless the feature genuinely requires it.

✓
Hybrid approaches — rough with CNC, finish critical features with EDM — are common in aerospace and tooling and often represent the lowest total cost.

CNC machining is a subtractive process driven by mechanical cutting. Rotating or linearly moving cutting tools — end mills, drills, boring bars, inserts — shear material away through direct contact. The workpiece or tool moves along programmed axes (typically 3 to 5), and material removal rate is governed by spindle speed, feed rate, depth of cut, and tool geometry. It is fast, scalable, and well-understood across virtually every material class.
Electrical Discharge Machining (EDM) removes material through controlled electrical sparks, not mechanical cutting. A dielectric fluid floods the work zone, and rapid spark discharge between an electrode (or wire) and the workpiece erodes material in microscopic increments. Because no cutting force is applied, EDM can machine hardened steels, carbides, and exotic alloys that would destroy or deflect conventional tooling. The two primary variants are sinker EDM (ram EDM), which uses a shaped electrode pressed into the workpiece, and wire EDM, which uses a continuously fed brass or coated wire to cut 2D profiles through full material thickness. Both variants leave a characteristic recast layer on the machined surface — typically 0.0001 to 0.001 inch thick — which must be accounted for in fatigue-critical applications.

Rule of thumb: If your cutting tool can reach it and the material is not hardened beyond ~45 HRC, CNC is almost always faster and cheaper. EDM is a solution to a specific problem, not a general-purpose process.

CNC machining handles the broadest material range of any subtractive process. Aluminum, steel, stainless, titanium, brass, copper, PEEK, Delrin, nylon, and most engineering plastics are all routinely machined. Hardened steels up to approximately 45 HRC can be hard-milled with appropriate carbide tooling and coatings (TiAlN, etc.), though tool wear and cycle times increase significantly above 50 HRC. Above that threshold, EDM becomes the economically rational choice.
EDM’s defining advantage is material-agnostic cutting. Any electrically conductive material can be EDM’d — hardened D2, H13, M2 tool steels, tungsten carbide, Inconel, Hastelloy, titanium aluminide, and even polycrystalline diamond (PCD). The spark gap doesn’t care about hardness. This is why EDM dominates mold and die manufacturing, where cavities are roughed in the annealed state and then re-machined after heat treatment, or why aerospace turbine components in hardened nickel superalloys are finish-machined with EDM after CNC roughing.
One critical constraint: EDM requires electrical conductivity. Ceramics, most composites, and engineering plastics cannot be EDM’d at all. If your part is non-conductive, EDM is off the table regardless of geometry or hardness.

Warning: Do not specify EDM for non-conductive materials — it is physically impossible. Ceramics, PEEK, UHMW, and carbon fiber composites require alternative finishing strategies.

CNC machining routinely achieves tolerances of plus or minus 0.001 to 0.005 inch in production environments. With proper fixturing, tooling, and temperature-controlled environments, precision CNC reaches plus or minus 0.0002 inch on critical dimensions. Surface finish ranges from Ra 125 microinch in rough cuts down to Ra 8 to 16 microinch with fine finishing passes — and Ra 4 to 8 microinch with manual or vibratory post-processing. Five-axis CNC significantly expands reachable geometry by tilting the spindle relative to the workpiece, reducing the need for EDM on many complex forms.
Wire EDM tolerances of plus or minus 0.0001 inch are achievable and repeatable — it is one of the most dimensionally precise processes available for 2D profiles. Sinker EDM tolerances depend heavily on electrode accuracy and wear compensation algorithms, but plus or minus 0.0005 inch is standard for production sinker work. EDM surface finish in fine-spark finishing passes reaches Ra 4 to 8 microinch, and mirror finishes below Ra 2 microinch are possible with dedicated polishing spark conditions. Critically, EDM produces no burrs and applies zero cutting force — features that matter enormously for thin-wall sections, fragile geometries, and pre-hardened parts where distortion cannot be tolerated.
The geometric feature that most often drives EDM selection is the sharp internal corner. A CNC end mill always leaves a radius equal to its own radius. If your part requires a true 90-degree internal corner — common in mold cavities, keyways, and spline roots — sinker EDM with a sharp-cornered electrode is the only machining solution short of broaching.

Key insight: Wire EDM is frequently the most cost-effective way to cut hardened precision blanks, punches, and die sections to final dimension — eliminating post-heat-treat grinding in many cases.

CNC machining is fundamentally a high-material-removal-rate process. A 3-axis VMC roughing aluminum at aggressive parameters removes 10 to 50+ cubic inches per minute. Even hard milling of tool steel at conservative parameters vastly outpaces EDM. For prismatic parts, turned components, and most structural aerospace hardware, CNC is the cost-minimizing default. Setup time on a 4- or 5-axis machine can be significant for complex parts, but production amortizes that cost quickly.
EDM is slow by comparison. Wire EDM cutting speeds through 2-inch hardened steel range from roughly 10 to 30 square inches per hour depending on material, finish requirement, and machine capability. Sinker EDM is slower still — electrode wear, multiple electrode changes, and fine-spark finishing passes mean that machining a single mold cavity can take 8 to 40+ hours. This is acceptable when the feature cannot be made any other way, but it is economically punishing if used carelessly as a substitute for proper CNC programming.
Cost drivers for CNC are primarily machine time, tooling, and setup. Cost drivers for EDM are electrode fabrication (sinker), machine time, and dielectric consumables. For sinker EDM, electrode cost is often overlooked — a graphite or copper electrode must be precision-machined to create the negative of your cavity, which itself represents a CNC machining job. Complex multi-cavity sinker EDM jobs carry significant electrode budgets that must be quoted accurately.

There are geometries where CNC simply cannot produce the required feature, regardless of machine capability or programming sophistication. Recognizing these early in the design phase prevents costly redesigns and missed lead times.

• Sharp internal corners with no radius relief: Any CNC milled internal corner will carry a radius equal to the cutter radius. If the mating part, insert, or functional requirement demands a true sharp corner (zero radius), sinker EDM is required.
• Deep narrow slots and blind keyways: Aspect ratios beyond approximately 6:1 depth-to-width challenge or exceed rigid CNC tooling limits. EDM wire or a sinker electrode can follow the cavity without deflection concerns.
• Through-holes in hardened material: Drilling hardened tool steel or carbide is destructive to tooling. Wire EDM or EDM hole-popping completes these features efficiently post-hardening.
• Complex 3D cavity forms in hardened steels: Mold cores and cavities, die inserts, and forging dies are almost universally finished with sinker EDM after heat treatment.
• Micro-features below 0.010 inch: Micro-EDM and small-hole EDM drilling access feature sizes where carbide micro-end mills are fragile and prone to breakage.

If your part drawing contains any of these features, flag them in your DFM review before quoting. Missing them upstream is how prototype schedules blow up.

Warning: Specifying a sharp internal corner on a mold cavity or die insert without explicitly noting EDM in the process plan will result in a non-conforming part or a shop-floor deviation request. Communicate intent on the drawing.

In aerospace, defense, and precision tooling, the most common approach is not CNC or EDM — it is CNC then EDM. Parts are roughed and semi-finished in the annealed or lower-hardness state using CNC, leaving 0.010 to 0.030 inch of stock on critical surfaces. The part is then heat treated to final hardness, stress relieved, and re-fixtured for EDM finishing. This hybrid sequence takes advantage of CNC’s material removal speed while using EDM’s indifference to hardness for final dimensioning.
Wire EDM is particularly powerful as a finishing operation for precision blanks, punches, and die sections. A tool steel punch blank roughed on a CNC lathe or mill, hardened to 60 HRC, and then wire EDM’d to final profile tolerances of plus or minus 0.0002 inch is a standard production sequence in progressive die manufacturing. The wire EDM step replaces grinding in many cases, reduces cycle time, and handles complex profiles that surface grinders cannot follow.
When specifying a hybrid process flow, it is essential to account for heat treat distortion in your stock allowances. Through-hardened tool steels distort — how much depends on geometry, alloy, and quench method. Working with your manufacturing partner to establish distortion benchmarks on representative blanks before committing to tight pre-EDM stock is best practice. Nimble’s certified partner network and DFM review process flag these interactions before a job hits the floor.

Rule of thumb: Leave 0.015 to 0.030 inch of stock on EDM-finished surfaces after heat treatment for typical tool steel components. Undershooting this allowance risks scrapping a hardened part.

Both CNC machining and EDM appear extensively in aerospace and defense supply chains — often on the same part number. Turbine blades, fuel system components, structural fittings, and ordnance components all carry geometries that require one or both processes. For programs subject to ITAR (International Traffic in Arms Regulations), the manufacturing source and data handling must comply with strict export control requirements, regardless of which process is being used.
AS9100 Rev D certification adds a quality management layer specific to aviation, space, and defense — covering risk management, configuration control, and first article inspection requirements that ISO 9001 alone does not mandate. When sourcing EDM or CNC work for defense programs, verifying that your supplier holds both AS9100 and ITAR registration is non-negotiable. A shop that is ISO 9001 certified but not AS9100 cannot fulfill AS9100 flow-down requirements from prime contractors without exceptions.
CMM inspection with full ballooned FAI documentation is standard practice for aerospace machined components. For EDM-finished features in particular — where the recast layer and surface integrity affect fatigue life — non-destructive evaluation (NDE) requirements may apply. Nimble’s certified partner network is AS9100, ISO 9001, and ITAR-registered, with CMM inspection included on qualifying jobs, ensuring the documentation package meets prime contractor flow-down requirements without separate supplier qualification burden on your team.

Warning: Do not assume ISO 9001 certification satisfies AS9100 flow-down clauses. AS9100 Rev D includes aerospace-specific requirements that ISO 9001 does not cover — always verify the specific certification scope with your supplier.

The decision framework is straightforward once you have the geometry, material, tolerance, and quantity in front of you. Start with CNC as the default. Ask the following questions in sequence, and deviate to EDM only when a ‘yes’ answer makes it necessary.

• Is the material hardened above ~45 to 50 HRC? If yes, evaluate EDM for finishing operations.
• Does the feature require a zero-radius internal corner? If yes, sinker EDM is required unless a design change is acceptable.
• Is the feature geometry inaccessible to a rigid cutting tool? Deep narrow slots, blind cavities, and complex through-sections may require EDM.
• Is the wall section thin enough that cutting forces cause deflection or distortion? EDM’s zero cutting force may be the only path to a stable feature.
• Is the material non-conductive? If yes, EDM is eliminated regardless of other factors.

If none of these triggers apply, CNC is the right process. If one or more apply to specific features on an otherwise CNC-machinable part, a hybrid approach is almost always more cost-effective than routing the entire part to EDM. Submitting a complete 3D model and 2D drawing for DFM review — which Nimble provides free with every quote — surfaces these decisions before they become production problems. Getting the process call right upstream is the difference between a clean program and an expensive deviation.

Key insight: Most parts that ‘need EDM’ actually need EDM for one or two features only. Identify those features precisely, specify the process on the drawing, and machine everything else with CNC. Hybrid quoting is standard practice.

READY TO SOURCE?

Table of Contents

Related Services

Get a Quote in 24h

Upload your drawing and get a detailed quote with free DFM review.