Hard milling, grinding or wire EDM: picking the finishing route at 55-62 HRC
Once a part is above roughly 50 HRC, there are only three practical ways to take it to final size: mill it, grind it, or burn it with EDM. Shops pick between them every day, and the choice moves both the price and the lead time by a factor that dwarfs anything else on the quote.
Here is how the decision actually gets made.
What each process is good at
Hard milling removes material with a defined cutting edge — CBN or coated carbide — on a machining centre. It is the only one of the three that produces arbitrary 3D geometry in one setup. Cavities, blends, ribs, contoured faces: all of it comes off the same spindle.
Grinding uses an abrasive wheel. It wins on flatness, parallelism, roundness and the very best surface finishes. It is slow at removing volume, and it wants simple geometry — flat faces, cylinders, simple profiles.
Wire EDM erodes material with a spark, so hardness is irrelevant to it. It produces sharp internal corners that no rotating tool can reach, and it applies zero cutting force, which matters on thin or delicate sections. It only makes ruled surfaces, and it is slow.
Side by side
| Hard milling | Grinding | Wire EDM | |
|---|---|---|---|
| Geometry freedom | High — full 3D | Low — flat, cylindrical | Medium — ruled surfaces only |
| Realistic tolerance | ±0.01 mm, ±0.005 mm on called-out features | ±0.002 mm and better | ±0.005 mm |
| Realistic finish | Ra 0.4-0.8 | Ra 0.1-0.4 | Ra 0.8-1.6 as cut |
| Internal corner radius | Limited by tool radius | Limited by wheel | Down to wire radius (~0.1 mm) |
| Cutting force | Moderate | Low | None |
| Volume removal | Fast | Slow | Very slow |
| Setups | Usually one | Often several | One, plus a start hole |
The rules that decide it
Sharp internal corners force EDM. A 0.2 mm internal corner cannot be milled — there is no cutter that small with the rigidity to survive hardened steel. If the drawing has one, the feature is going on a wire machine, and the rest of the part gets planned around that.
Flatness and parallelism below about 0.01 mm force grinding. Hard milling holds size well but leaves a subtle cusp pattern and is sensitive to thermal growth. If the print calls for 0.005 mm flatness over 200 mm, that face gets ground, full stop.
3D contours force hard milling. A mould cavity with blended surfaces is not a grinding job and not an EDM job unless you are willing to sink an electrode — which means making the electrode first, which is its own machining job.
Volume forces hard milling. Grinding a 4 mm step off a hardened block is a way to burn the part and the wheel. Mill it close, then grind the last 0.05 mm if the finish demands it.
The hybrid route is usually the cheapest
The instinct to pick one process for the whole part is what inflates quotes. In practice the cheapest plan is almost always mixed:
- Hard mill everything to within 0.05 mm.
- Grind only the two or three faces that carry the critical tolerance.
- Wire EDM only the features no cutter can reach.
That takes the fast process for the bulk of the material, the accurate process for the small number of surfaces that need it, and the expensive process for the features with no alternative. A shop that quotes this way will usually beat a shop quoting “grind everything” by a wide margin on the same drawing — see hybrid routing for how to specify it.
What this changes on your drawing
Mark which faces carry the real tolerance. A blanket tolerance class across every dimension forces the shop to assume grinding everywhere, because that is the only way to guarantee it. Mark three faces and the rest opens up to milling.
Do the same with surface finish. Ra 0.4 on a sealing face is a specification; Ra 0.4 on all surfaces of a die block is a polishing operation you did not ask for and will pay for.
If you are unsure which route your part wants, send the drawing and say so — the answer is usually obvious to a shop that runs all three, and it costs nothing to ask.