Hard milling

Definition and typical parts

Hard milling is CNC milling of steel after heat treatment, typically at 48-62 HRC and up to about 65 HRC. The usual sequence is rough machine → harden and temper → hard mill to size. Heat treatment distortion is machined out in the last step.

The process became practical in the 1990s. 3 developments made it possible:

• Fine-grain carbide with heat-resistant coatings
• High-speed spindles
• CAM software that holds tool load constant

Typical parts:

• Mould cavities, cores and inserts
• Die inserts and forging dies
• Punch profiles and form tools
• Cavities that were once made with graphite or copper electrodes and sinker EDM

Cutting mechanism and machining stages

Hardened steel tolerates very little load per cutting edge before the edge chips. Hard milling uses light engagement and high cutting speed to keep the chip thin. The cutting zone heats and softens the steel locally, and the chip carries most of the heat away.

Flood coolant would quench the edge on every revolution and crack the coating. Most hard milling therefore runs dry, with an air blast or with minimum-quantity lubrication (MQL).

The work is split into stages, each with its own engagement:

Stage	Typical tool	Engagement	Purpose
Roughing (if done hard)	Bull-nose or high-feed end mill, 6-16 mm	Trochoidal: ap up to 1.5×D, ae 3-8% of D. High-feed: ap 0.2-0.5 mm, wide ae	Remove bulk stock at constant tool load
Rest machining	Smaller bull-nose or ball-nose	Same chip load as roughing	Clear corners the large tool could not reach
Semi-finish	Ball-nose or bull-nose	ae and ap 0.1-0.3 mm	Leave an even 0.05-0.10 mm everywhere
Finish	Ball-nose (3D), bull-nose or flat end mill (walls, floors)	ae 0.05-0.3 mm, ap 0.05-0.10 mm	Final size and surface

Constant-engagement toolpaths

A conventional offset toolpath raises the tool load 2-3 times at every inside corner. At 60 HRC that load spike breaks small tools.

Trochoidal and other constant-engagement paths keep the arc of contact the same along the whole path. Details are in trochoidal and dynamic toolpaths.

Rest machining and even stock

After a 10 mm tool roughs a cavity, the corners still hold material. Rest machining calculates that remaining stock and cuts only it, at the small tool’s own chip load.

The semi-finish pass leaves an even 0.05-0.10 mm for the finishing tool. Uneven stock makes the finishing tool deflect by different amounts, and the surface follows that deflection.

End mill types for hardened steel

Tool	Application	Notes
Coated carbide ball-nose	3D finishing of cavities and cores, 45-65 HRC	Fine-grain carbide with AlTiN, AlCrN or TiSiN-type coating. Most common tool
Coated carbide bull-nose (corner radius)	Roughing, rest machining, flat floors	Stronger corner than a sharp end mill
High-feed end mill	Roughing open areas	Shallow depth, high feed per tooth; force directed axially into the spindle
CBN ball-nose	Finishing small features above about 58 HRC	Diameters about 0.5-6 mm. Longer life, holds size over long paths. Finishing only
Necked long-reach ball-nose	Deep ribs and pockets	Short flute, relieved neck. Each extra diameter of reach lowers feed and finish

Spindle speed is set on the effective diameter, not the nominal one. A 6 mm ball-nose cutting 0.1 mm deep touches the work on a circle about 1.5 mm across. The spindle must turn about 4 times faster than the nominal diameter suggests, so small tools need 20,000 rpm or more.

Tool holding sets the limit for accuracy and tool life:

• Holder | shrink-fit or hydraulic
• Runout | under 0.005 mm at the tool tip
• Stickout | as short as the geometry allows, ideally under about 4×D

Stepover and cusp height

A ball-nose tool leaves a small ridge, or cusp, between neighbouring passes. Its height depends on the ball radius R and the stepover s:

h ≈ s² / 8R

Ball diameter	Stepover 0.1 mm	Stepover 0.2 mm	Stepover 0.3 mm
2 mm	1.25 µm	5.0 µm	11.3 µm
6 mm	0.42 µm	1.7 µm	3.8 µm
10 mm	0.25 µm	1.0 µm	2.3 µm

Halving the stepover cuts the cusp to 25% of its height and doubles the finishing time. The theoretical Ra of a cusp profile is about 25% of its height. A 1 µm cusp corresponds to roughly Ra 0.25 µm, before runout, deflection and tool wear add to it.

Shops finish with the largest ball the geometry allows. A small internal radius specified across a whole cavity forces a small ball and slows the finishing of every surface.

3-axis vs 5-axis hard milling

On a 3-axis machine the ball-nose tool stays vertical. On flat or gently sloping surfaces its centre point, where cutting speed is zero, ends up in the cut. The centre rubs instead of cutting, which degrades the finish and wears the tool tip.

A 5-axis machine tilts the tool, usually 10-20°, so the contact point moves onto the faster part of the ball. The tilt also lets a short holder reach into a deep cavity clear of the walls. Cantilever deflection grows with the cube of stickout, so halving the length reduces bending about 8 times.

Setup	Typical use
3-axis	Shallow open parts, flat-bottomed pockets, plates
3+2 positioning (tilt, lock, mill in 3 axes)	Most cavities and inserts
Simultaneous 5-axis	Deep ribs, steep walls, forms where the tilt must change continuously

Tolerances and surface finish

Figures for a warmed-up, thermally stable machining centre. Confirm per part and per drawing.

Characteristic	Typical	Best case
Size	±0.01 mm	±0.005 mm on a few called features, with on-machine probing
3D profile	0.02 mm	0.01 mm
Surface finish (Ra)	0.4-0.8 µm	0.2 µm on small areas with fine stepover
Internal corner radius	Equal to tool radius	0.25-0.5 mm with 0.5-1 mm tools at shallow depth

Heat and wear set these limits. The spindle grows as it warms up. A long finishing path wears the tool, so the end of the path comes out slightly oversize.

Shops manage this with warm-up cycles, by splitting long paths between tools and by using CBN on critical areas.

Below Ra 0.2 µm, bench polishing or lapping after milling usually costs less than finer milling.

Limits of hard milling

Deep, narrow features. Ribs and slots deeper than about 6-10 times their width need long tools. Those tools deflect and chatter. Sinker EDM handles these features with less risk.

Sharp internal corners. A milled corner can never be sharper than the tool radius. Through profiles with sharp inside corners go to wire EDM; blind ones go to sinker EDM.

Large flat faces to a few microns. Each pass leaves its own marks. Machine straightness also shows over 300 mm of travel. Flatness and parallelism of a few microns over a large plate belong to grinding.

Round parts. Diameters, bores and shoulders on a turned part are faster and more accurate by hard turning.

High-carbide grades at high hardness. D2 at 62 HRC and high-vanadium powder steels wear tools quickly. A large finishing surface may need several tools, each leaving a small step.

Hard milling vs sinker EDM vs grinding

Feature	Hard milling	Sinker EDM	Grinding
Open 3D cavity or core	First choice	Only where ribs or corners require it	Not applicable
Rib or slot deeper than 6-10× width	Slow, high risk	First choice	Not applicable
Sharp internal corner	Limited by tool radius	Yes, in blind cavities	Outside corners and open profiles only
Flat face, flatness under 0.005 mm	Marginal	Not applicable	First choice
Recast layer	None	Yes, polished off on critical surfaces	None
Lead time	Shortest; no electrodes	Electrodes add days	Separate setup per face

A common mould insert route: hard mill the cavity → sinker EDM 2-3 deep ribs → grind shut-off faces.

Drawing and RFQ requirements

• Hardness | as a band after heat treatment, e.g. 52-54 HRC or 58-62 HRC, not “hardened”.
• Grade | by standard designation. H13 at 48-52 HRC and D2 at 60 HRC are different jobs on the same geometry.
• Tight features | ±0.005 mm only on the features that need it; the rest at ±0.01 mm or ±0.02 mm.
• Internal corner radii | as large as the design allows. A larger radius allows a larger, stiffer tool and a wider stepover.
• Finish per surface | e.g. Ra 0.4 µm on the moulding surface and Ra 1.6 µm on clearance faces. State whether the cavity will be polished or textured.
• EDM acceptance | whether EDM is allowed on ribs and corners, and whether the recast layer must be removed.
• Blank condition | annealed for roughing first, or already hardened. Stock to leave before hardening is in the heat treat allowance table.