CNC Solutions for Mold & Die Making

Hard Milling: Cutting Steel at 50–65 HRC

Traditional mold making was simple: rough the cavity in soft steel, send it out for heat treatment, then finish with EDM. Hard milling has overturned this workflow. Modern CBN and nano-grain carbide end mills can cut fully hardened tool steel at 62 HRC — allowing heat treatment before final machining, which eliminates heat-treat distortion as a dimensional variable.

The physics of hard milling are fundamentally different from conventional machining. At 50+ HRC, the material is so hard that the chip formation mechanism changes from shear to adiabatic shear banding — the chip generates so much heat at the shear zone that it thermally softens locally, producing a red-hot, segmented chip. This is actually advantageous: the heat goes into the chip, not the workpiece or tool, keeping the mold dimensionally stable during machining.

Hard Milling Parameter Guidelines

Depth of Cut: Axial DOC = 0.2–0.5 × tool diameter. Radial DOC for finishing = 0.002–0.010" stepover.
Chip Thinning: At small radial engagement, effective chip thickness drops. You MUST compensate by increasing feed rate — otherwise the tool rubs instead of cuts. Use our Chip Load Calculator for thinning compensation.
Coolant: Air blast only for hardened steel. Flood coolant causes thermal shock cracking of CBN/carbide inserts. The chip should carry the heat away.
Corner Radius: Never use sharp corners on hard milling tools. Minimum 0.5mm corner radius for tool life. Ball nose end mills are the default for 3D surfaces.
Spindle Speed: 300–500 SFM for carbide, 500–1000 SFM for CBN. This translates to 15,000–40,000 RPM for the small-diameter tools used in mold finishing.

EDM vs. High-Speed Machining: The Decision Framework

The "EDM vs HSM" debate isn't binary — it's about understanding which features are better suited to which process, and where the crossover economics make sense. Modern mold shops use both, but the ratio has shifted dramatically toward HSM over the past decade.

Factor	EDM (Sinker)	High-Speed Milling	Recommendation
Sharp internal corners	✓ Any radius	Limited by tool radius	EDM for corners < 0.5mm
Deep ribs (> 10:1 L/D)	✓ No deflection	Tool deflection risk	EDM for L/D > 8:1
3D contour surfaces	Requires shaped electrode	✓ Direct from CAD	HSM preferred
Surface finish	VDI 1–12 textures	✓ 2–8 µin Ra (mirror)	HSM for polished surfaces
Lead time (single cavity)	4–6 hours + electrode	✓ 2–4 hours direct	HSM for speed
Heat-affected zone (HAZ)	Yes — recast layer	✓ No thermal damage	HSM for surface integrity

The trend in modern mold shops: use HSM for 80–90% of cavity machining, and reserve sinker EDM for sharp internal corners, deep ribs, and texture applications where it remains superior. Wire EDM remains essential for through-hole features and splitting inserts.

Graphite Electrode Machining

For mold shops that still rely on sinker EDM (or are transitioning toward more HSM), graphite electrode machining is a critical competency. Graphite machines differently from any metal — it doesn't produce chips but rather dust, which is abrasive, conductive, and a respiratory hazard.

Graphite Machining Requirements

Dust Collection: Sealed enclosure with dedicated vacuum system. Graphite dust is conductive — it will destroy exposed linear scales and ball screws if not contained.

Tool Material: Diamond-coated carbide or PCD. Uncoated carbide lasts 10× less in graphite due to abrasive wear. A $40 diamond-coated tool outlasts twenty $8 uncoated tools.

Spindle Speed: 24,000–60,000 RPM. Graphite allows extremely high SFM (800–2000) because there is no heat buildup — the material sublimates rather than melts.

Machine Protection: Sealed way covers, positive-pressure spindle bearing seals, and filtered coolant returns. Some shops dedicate a machine exclusively to graphite.

Mold Steel Selection and Machinability

The choice of mold steel directly affects both machining strategy and mold performance. Here's how common mold steels compare in machinability and application:

Steel Grade	Hardness	Application	Machinability Notes	Calculator
P20 (1.2311)	28–34 HRC	Medium-run injection molds	Good machinability, pre-hardened	Steel F&S
H13 (1.2344)	44–52 HRC	Die casting dies, hot work	Hard milling required post-HT	Steel F&S
S7 (1.2357)	54–58 HRC	High-impact dies, cold work	Requires CBN or advanced carbide	Steel F&S
D2 (1.2379)	58–62 HRC	Stamping dies, wear components	Chromium carbides cause chipping	Steel F&S
420 SS (1.2083)	50–52 HRC	Corrosion-resistant medical molds	Stringy chips, work hardening	Stainless F&S

Achieving Mirror Surface Finish (SPI A-1)

SPI A-1 ("mirror" finish, 0–1 µin Ra) is the highest surface finish grade in the plastic injection mold industry. Achieving it requires both machining strategy and post-machining polishing, but the less work the polisher has to do, the faster and more consistent the result.

The practical limit of direct CNC machining on hardened steel is approximately 2–4 µin Ra — achievable with ball nose end mills at 0.001–0.003" stepover, 40,000+ RPM, and light axial depth. From there, skilled hand polishing with diamond paste brings the surface to SPI A-1. Our Surface Finish Calculator predicts theoretical finish from tool geometry and feed rate.

Frequently Asked Questions

Do I need a dedicated high-speed machine for mold work?

For serious mold and die work, yes. A standard VMC with 8,000 RPM and 300 IPM rapids cannot perform effective hard milling. You need minimum 20,000 RPM (ideally 42,000+), 800+ IPM rapids, HSK-E or HSK-A spindle interface, and a control that can handle look-ahead block processing to maintain constant feed rate on complex contours. Entry-level HSM machines from Makino, Röders, or GF Machining start at $250,000–$350,000.

How much does EDM add to mold manufacturing cost?

Sinker EDM adds $2,000–$15,000 per cavity depending on complexity, because you must machine the graphite electrode (which is itself a precision part), then burn the feature, then clean up the recast layer. Each EDM operation you can eliminate through HSM typically saves 40–60% of the individual feature cost. However, some features (sharp internal corners, deep narrow ribs) are simply impractical to machine.

What spindle speed do I need for graphite electrodes?

Minimum 24,000 RPM, with 42,000–60,000 RPM preferred for fine-detail electrodes. The key constraint is tool diameter × SFM: a 0.5mm ball nose at 1500 SFM requires 36,000 RPM. Use our RPM & Cutting Speed Calculator to determine required spindle speed for your tool diameter and target SFM.

What surface finish can I achieve directly from the machine?

With proper HSM parameters, expect 4–8 µin Ra on hardened steel contour surfaces and 2–4 µin Ra on flat/ruled surfaces. This is SPI B-1 to A-2 grade — requiring only light polishing to reach SPI A-1 mirror finish. Without HSM (standard VMC), expect 32–63 µin Ra, requiring extensive manual polishing.