Introduction to a Super Hard Tool: How PCBN and PCD Cut Hardened Steel

• 1
  What Counts as a Super Hard Tool
• 2
  How a Super Hard Edge Removes Hardened Steel
• 3
  Cutting Parameters That Decide Tool Life
• 4
  Where a Super Hard Tool Does Not Fit
• 5
  Machine and Setup Requirements
• 6
  Super Hard Tool Grades vs Carbide and Ceramic

A super hard tool is a cutting tool whose edge material sits above carbide on the hardness scale. In practice that means polycrystalline cubic boron nitride (PCBN), polycrystalline diamond (PCD), and single-crystal diamond. Hardness lands around 4,000 to 9,000 HV, compared with roughly 1,500 to 2,000 HV for coated carbide.

That gap changes the failure mode. Carbide edges deform and wear quickly once the workpiece passes about 45 HRC, because the heat and pressure at the contact zone exceed what the cobalt binder can hold. A super hard tool keeps its shape because the abrasive grains barely yield at those temperatures.

Hardness alone is not enough to justify the cost. PCBN is chemically stable against ferrous alloys at 1,000 °C and above, while diamond graphitizes when it touches iron. That single fact decides which insert you buy for a hardened steel shaft versus an aluminum housing.

The tool body also differs. Most super hard inserts are brazed tips on a carbide shank, and the tip is only 0.5 to 1.5 mm thick. You are paying for a small area of expensive material bonded to a cheap support, which is why regrinding and indexing discipline drives the real cost per part.

• 1
  PCBNFerrous workpieces above 45 HRC: hardened steel, bearing steel, gray cast iron.
• 2
  PCDNon-ferrous and abrasive: aluminum alloys, copper, composites, graphite.
• 3
  Single-crystal diamondMirror finishing on non-ferrous optics and wear parts.
• 4
  Not a super hard toolCBN-coated carbide and ceramic inserts behave differently. Do not mix the data.

Hard turning with PCBN is not a light finishing pass over a soft part. The insert takes the full hardness of the material in one setup, usually after heat treatment. The edge is prepared with a chamfer or a hone, typically 0.1 to 0.2 mm wide at a 20° to 25° angle, so the tip does not chip on entry.

Cutting happens in a narrow zone. Depth of cut stays small, often 0.1 to 0.4 mm, and feed runs 0.05 to 0.2 mm per revolution. The chip is thin and comes off hot. Most of the heat leaves with the chip, which is why these tools tolerate dry cutting and why coolant is often unnecessary or even harmful on interrupted cuts.

The negative rake geometry found on most PCBN inserts pushes the material rather than slicing it. That raises cutting force but protects the edge. On a rigid machine with a short tool overhang, the result is a surface finish in the Ra 0.2–0.8 μm range straight from the tool, which can replace a grinding step.

Rigidity is the limit, not the insert. A lathe with worn spindle bearings or a part held far from the chuck will chatter no matter how hard the tool is. When you hear a high-pitched ring on the first pass, stop and fix the setup before you blame the grade.

• 1
  Edge chamfer0.1–0.2 mm at 20°–25°, protects against chipping on entry.
• 2
  Depth of cut0.1–0.4 mm per pass on hardened steel.
• 3
  Feed0.05–0.2 mm/rev; too low rubs and work-hardens the surface.
• 4
  CoolantOften dry. Flood coolant on interrupted cuts can cause thermal cracking.

Speed is the first lever. On PCBN turning 60 HRC bearing steel, a starting point of 100 to 140 m/min usually gives a stable wear pattern. Push past 200 m/min and the edge wears fast; drop below 60 m/min and you generate built-up edge and poor finish.

Feed must stay above a floor. Below roughly 0.05 mm/rev the edge rubs instead of cutting. The workpiece surface work-hardens, the next pass cuts into a harder skin, and tool life collapses. If your finish requirement forces a very light feed, choose a grade with finer grain rather than slowing the feed further.

Depth of cut should be as constant as possible. On a hardened shaft with a keyway or a shoulder, an interrupted cut puts impact load on a brittle tip. A high-CBN-content grade with a stronger chamfer survives that better than a low-content finishing grade.

Measure wear at fixed intervals: flank wear land, notch wear at the depth line, and crater wear on the rake face. Log the numbers per part. After two or three jobs you will know your own tool life curve, which beats any catalog recommendation.

• 1
  Watch flank wear0.2 mm is a common replacement limit for finishing passes.
• 2
  Watch notch wearGrows at the depth-of-cut line on cast skins and forged surfaces.
• 3
  Keep depth constantVarying depth is the fastest way to chip a brazed tip.

Low-carbon and soft steels are a poor match. Below about 45 HRC, carbide is cheaper, tougher, and easier to replace. Using PCBN on soft material just burns money, because the hardness advantage does nothing and the brittle edge chips more easily.

Diamond is the wrong choice for any iron-bearing alloy. At cutting temperature the carbon diffuses into the steel, the edge wears at a rate you can see between parts, and the finish degrades within a few minutes of cutting.

Thin-wall and long slender parts rarely suit hard turning at all. The cutting force on a negative rake edge deflects the part, and you end up chasing chatter with speed changes. On those parts, grind or use a supported setup instead.

Small internal features are limited too. A super hard boring bar with enough stiffness to avoid chatter is hard to find below about 8 mm bore diameter. If the feature is smaller, plan a different process from the start.

• 1
  Skip PCBN below 45 HRCCarbide wins on cost and edge toughness.
• 2
  Never run PCD on steelDiamond reacts with iron and wears out fast.
• 3
  Small boresBelow roughly 8 mm, bar stiffness becomes the limiting factor.

A super hard tool needs a machine that can hold position under load. Spindle runout under 5 μm, a rigid turret, and a tool holder with minimal overhang are the baseline. On a worn lathe, no insert grade will give you a consistent Ra value across a batch.

Balance and chip evacuation matter more than most shops expect. Dry chips are hot and abrasive, and if they recirculate they scratch the finished surface. Air blast or a directed coolant stream aimed at the chip, not the edge, solves most of this.

For milling hardened pockets, the same rules apply but the entry is worse. A helical ramp at 2° to 3° with a small radial engagement keeps the load steady. Plunging straight down with a PCBN end mill will chip the corner on the first tooth.

At GreatLight we run hard-turning and hard-milling work on 16 simultaneous 5-axis machining centers and 27 three-axis machines, with tolerances held to ±0.005 mm and finishes from Ra 0.2–0.8 μm. Inspection is 100% before shipment, with reports on request.

• 1
  Spindle runoutUnder 5 μm for consistent finish across a batch.
• 2
  Chip controlAir blast aimed at the chip, not the insert edge.
• 3
  Helical entry2°–3° ramp for hardened pockets, small radial engagement.