Home / Metal cutting / Tool materials

The edge: material, geometry, and what speed it will take

Two tool materials, five ISO 513 workpiece groups, and a factor of ten between the slowest and fastest combination. Then geometry, which decides everything the speed ranges cannot.

Cutting speed range by workpiece group and tool material
ISO 513 group	Carbide, SFM	Carbide, m/min	HSS, SFM	HSS, m/min
P Steel	200 – 600	61 – 183	50 – 140	15 – 43
M Stainless	150 – 400	46 – 122	40 – 100	12 – 30
K Cast iron	250 – 450	76 – 137	50 – 90	15 – 27
N Aluminium	250 – 1500	76 – 457	70 – 600	21 – 183
S Heat resistant	50 – 250	15 – 76	10 – 50	3 – 15

Ranges, not recommendations. Where you sit inside one depends on the grade, the coating, the depth of cut and how rigid the setup is — which is what the calculators work out. The width of each band is itself information: aluminium spans six to one because the limit is usually the machine rather than the tool, while heat resistant alloys barely move because the limit is the edge.

Choosing between them

Not a close contest for most production work, but the exceptions are real and they are not the ones people expect.

Carbide

Harder, holds an edge at cutting-zone temperatures, and runs at three to five times the speed of HSS across every material group. It is the default for virtually all production turning today, and the reason a modern machine earns its cost.

What it asks for in return is rigidity. Carbide is brittle relative to steel, so a weak setup, a long overhang or a shaky machine will chip the edge long before it wears out. It also wants to stay in the cut — repeated entry shock is what it handles worst.

What tool manufacturer shock is what it handles worst.

HSS

Tougher and far more shock resistant, at a fraction of the speed. That trade is worth making in three situations: heavily interrupted work, manual or older machines that cannot hold carbide's rigidity requirements, and small or intricate tooling where a brittle edge is a liability.

It is also sharper. HSS takes a keener edge than carbide, which is why it cuts a thinner chip before it starts rubbing — a real advantage on light finishing passes and on materials that smear rather than shear.

ISO 513 classifies carbide, not HSS. The P / M / K / N / S letter and the grade numbers that go with it are a cemented carbide classification. The workpiece groups apply to any tool, but there is no equivalent grade system for HSS, so nothing here stretches one over the other.

Geometry decides the chip

The grade decides how long the edge survives. The geometry decides what the cut actually does. They are chosen separately, and only one of them belongs in a speeds and feeds calculation. Geometry has an important machining effect: Cutting forces. Therefore, it controls wasted heat. The point that you must have in mind is every Cutting tools study must compare the conditions on the same tool, including nose radius to include the effect on the machining system as a whole.

One detail, five consequences

Chip formation comes first: the rake face and the chipbreaker decide whether the chip curls, breaks or comes off as a continuous ribbon. Everything else follows from that.

Evacuation is next — a chip that will not break wraps the tool, the part or the turret, and a stalled chip is how a good setup turns into scrap in one revolution. Then cutting forces, because the same feed on a sharp positive geometry and a strong negative one produces different loads in different directions. Then vibration, since the direction of those forces is what a marginal setup either tolerates or resonates with. And finally surface finish, which is where all four of the previous ones arrive.

It is in the designation

Insert codes carry the geometry alongside the shape and the size. A KNUX turning insert names a 55 degree parallelogram at zero clearance, and then a chipbreaker code — R12, L12, R13 — which is the part doing the work described above. Same carbide, different code, different cut.

The direction of the industry says the same thing. Read current turning insert patents and they are almost entirely about the top face: protrusions, chip breaker walls, how chip control holds up at small depths of cut. The substrate is settled. Geometry is where inserts are still being invented.

The calculators take lead angle, the nose radius in turning, and a rake class. Nothing else. No chipbreaker, no edge preparation. That is deliberate rather than unfinished: those choices act on chip control, and chip control is decided from your supplier’s chipbreaker chart against the material and depth of cut you are running — not from a formula. Rake is the exception because it acts on force, and force is arithmetic: the correction is applied to specific cutting force and therefore to power, and to nothing else. Speed and feed do not move.

Rake, and why it is a class rather than an angle

Rake changes specific cutting force by roughly 1.5% per degree. Across the useful range that is a swing of about a fifth in the power a cut draws, which on a power-limited machine decides whether it runs at all.

The angle is not a published number

An insert with a chipbreaker does not have a rake angle. The rake face is a moulded form, so the angle varies across it and the part of it doing the work shifts with feed and depth of cut. The holder then tilts the insert, so what the workpiece meets is the insert geometry plus the holder inclination.

What manufacturers publish instead is the chipbreaker's application window in feed and depth. That is the honest form of the same information, and it is not a number you can put in an equation.

So the input is the family

Negative basic, neutral or positive basic — which you know without looking anything up, because the clearance letter in the ISO 1832 designation tells you the family the insert belongs to. Each class carries a coarse correction, and the field will take a published angle directly if you have one.

The default is negative basic, because that is the reference the specific cutting force constants were determined at. Leave it alone and the numbers are what they always were — the assumption was there before, it was simply invisible.

The correction touches force and power only. It never moves cutting speed or feed, so the chain from the specified finish down to the feed stays exactly as it was. A rake class is a coarse instrument and it is labelled as one — it will not tell you what a specific chipbreaker does at your depth of cut.

What that fifth of the power actually bought

Positive geometry is why small machines can cut at all. A shop with a modest spindle, a worn machine, a long overhang or thin-wall work is not choosing a positive insert for the finish — it is choosing it because a negative edge generates force the setup cannot absorb, and the cut simply stalls. Twenty percent is the difference between a job that runs on the machine you own and one that needs the machine you do not. Enter your available spindle power in either calculator and it will say so: when a cut exceeds what the machine has, it points at the rake class first, because switching insert geometry costs nothing in removal rate while reducing depth of cut costs it directly.

Taylor exponents, and why they are not in the calculation

The exponent n in V × Tⁿ = C decides how sharply tool life falls as speed rises. Typical ranges by tool material are well established.

Tool material	Typical n	What it means
HSS	0.08 – 0.20	Tool life collapses very steeply with speed. A small increase costs a large fraction of the edge.
Carbide	0.20 – 0.40	More forgiving. Speed can be pushed further before life falls away, which is where the productivity comes from.

These numbers are on this page as a reference and a sanity check. They are deliberately not used anywhere in the cutting speed optimization.

The whole point of running the two-speed test is getting the actual exponent for your specific tool, material and machine. Feeding a class average into a calculation meant to be precise to the job would be false precision dressed up as an answer. The table’s only job is flagging a measured n that falls wildly outside what is physically plausible — which almost always means bad test data rather than an unusual material. Tool grade determines the service life of the cutting edge, whereas tool geometry governs the mechanics of chip formation and cutting forces. These parameters should be selected independently, and only tool grade should be incorporated into the speed selection. Therefore, comparative cutting tools studies should be conducted under equivalent conditions using identical tool geometries including the same nose radius, following design of experiments guide to change just one variable, cutting speed.

Run the two-speed test

Where to check this against the makers

Everything on this page is general: ranges, classes and exponents that hold across a group. The number you cut with comes from the catalogue for the tool in your hand. These are the primary sources — grade charts, chipbreaker tables, designation keys — and they are worth reading before trusting any calculator, including ours.

Tool manufacturers
Maker	What is worth reading there
Sandvik Coromant	Turning, milling, drilling and tooling systems. Grade charts, insert designation, and the application handbook.
Kennametal	Inserts, end mills and drills, with speed and feed data by material group.
ISCAR	Indexable tooling; the ISCAR World of Tools catalogue and its machining recommendations.
Seco Tools	Turning, milling and holemaking, with the Seco technical guides.
Walter	Walter, Walter Titex and Walter Prototyp: precision turning, drilling and threading.
Mitsubishi Materials	Cemented carbide tooling and the technical data section of the general catalogue.
Kyocera	Inserts and coated grades, including the MEGACOAT series.
Tungaloy	Carbide cutting tools and indexable inserts, with grade and chipbreaker tables.
Sumitomo Electric Hardmetal	Carbide and CBN tooling, with cutting data by workpiece group.
CERATIZIT	Hard material solutions: inserts, carbide rods and wear parts.

Reference sites and standards
Source	What it gives you
Machining Doctor	Calculators, machinability ratings for 200+ materials and machining datasheets for 700+. Useful for a second opinion on a cutting speed before you commit to a cut.
Machining Doctor — machinability chart	Ratings by material, with the method it used to get them.
Machining Doctor — calculators	Speeds, feeds, power, chip thinning, surface finish, hardness conversion.
ISO	The standards this page and the calculator speak: ISO 513 for the workpiece groups, ISO 1832 for insert designation, ISO 1302 for surface texture.

These are other people's sites and other people's data. Unrival Tools is not affiliated with any of them, the names are their trademarks, and nothing here is an endorsement of one over another — or of them over us. Where a maker's catalogue and this page disagree, the catalogue wins: it knows the grade, the coating and the chipbreaker, and this page does not.