CNC Insert Type and Selection: A Practical Guide for Engineers

• 1
  Key takeaways
• 2
  CNC insert type and selection by task
• 3
  Reading the ISO code before you compare inserts
• 4
  Chipbreaker and rake angle: the part most buyers ignore
• 5
  Coating and substrate: what the P, M, K and H letters mean
• 6
  Edge preparation and how it changes tool life
• 7
  Matching insert type to the material on your drawing
• 8
  Seven-step insert selection workflow

Every turning insert carries a code such as CNMG 120408. The first letter is the shape: C is 80° rhombic, D is 55°, S is square, T is triangular, V is 35°, W is trigon. The second letter is the clearance angle: N is 0°, P is 11°, C is 7°. The third letter covers tolerance class and the fourth is the chipbreaker or hole style.

The four-digit number is the size. CNMG 120408 means a 12.7 mm inscribed circle, 4.76 mm thickness, and 0.8 mm corner radius. Changing the last two digits changes the corner radius, which changes feed rate and surface finish. A 0.4 mm radius suits finishing; a 1.2 mm radius suits roughing where you want edge strength.

Milling inserts use a different code family, often with a lead angle built into the cutter body. A 45° lead face mill spreads the cut across more edge length, which reduces shock. If you are comparing a square shoulder mill against a 45° face mill for the same part, the ISO code tells you which one can survive the depth of cut you need.

Get the code wrong and the holder may not clamp, the edge may not reach the feature, or the corner radius may be too small for the feed the machine can deliver. On our 127 CNC machines, mismatched insert codes are one of the most common causes of a stalled first cut.

• 1
  Shape letterC, D, S, T, V, W. Determines profile access and edge strength.
• 2
  Clearance letterN, P, C. Determines whether the insert is negative or positive.
• 3
  Size digitsIC, thickness, corner radius in millimeters.
• 4
  Breaker suffixControls chip form for a specific depth-of-cut range.

The chipbreaker is a groove molded into the insert face. It lifts and curls the chip so it breaks instead of wrapping around the tool. A breaker designed for 2–5 mm depth of cut will not break a 0.3 mm finishing chip. It will rub, generate heat, and leave a poor surface. Match the breaker range to the depth of cut on your drawing, not to the largest cut in the program.

Rake angle matters just as much. Positive rake (10–20°) cuts freely and reduces cutting force, which helps on slender parts, small bores, and low-rigidity setups. Negative rake (0° or negative) puts more material behind the edge and survives interrupted cuts and heavy roughing. The trade-off is higher cutting force and more heat into the part.

For stainless and high-temperature alloys, a sharp positive edge reduces work hardening. For cast iron and hard steel, a honed negative edge resists chipping. There is no single insert that does both well. If a job mixes materials, plan for two insert types rather than forcing one compromise.

On mill-turn centers and 5-axis work, the same logic applies but access is tighter. A 35° V insert reaches into a corner that an 80° C insert cannot. The weaker tip is the price you pay. Keep depths of cut below 0.5 mm and use a honed edge to protect it.

• 1
  Light cut, 0.2–0.5 mmSharp positive breaker. Watch for rubbing.
• 2
  Medium cut, 0.5–2 mmGeneral-purpose breaker. Most turning jobs land here.
• 3
  Heavy cut, 2–5 mmStrong negative breaker. Needs machine rigidity.

ISO grade colors are a starting point. P (blue) covers steel, M (yellow) covers stainless, K (red) covers cast iron, N (green) covers aluminium and non-ferrous, S (brown) covers titanium and superalloys, H (gray) covers hardened steel. The number after the letter tells you hardness versus toughness: P10 is harder and faster, P40 is tougher and slower.

CVD coatings are thick and wear-resistant. They suit continuous cuts in steel and cast iron at higher surface speeds. PVD coatings are thinner and keep a sharper edge. They suit stainless, titanium, and any job with interrupted cuts or a need for good surface finish.

Substrate grain size also matters. A fine-grain carbide substrate holds a sharper edge and resists chipping, which helps in small-diameter boring and threading. A coarser substrate is tougher and cheaper, which suits roughing where edge sharpness is less critical.

For aluminium, uncoated polished inserts with a high positive rake cut cleanly. Diamond-coated inserts last far longer but cost more. On 6061 and 7075 parts we often start with a polished uncoated insert, then move to diamond only when the run length justifies it.

• 1
  PVD TiAlNStainless, titanium, interrupted cuts.
• 2
  CVD TiCN/Al2O3Steel and cast iron, continuous cuts.
• 3
  Diamond or ZrNAluminium and non-ferrous, high speed.
• 4
  Fine-grain substrateSmall bores, threading, sharp edge needs.

A raw sintered edge is sharp but brittle. Edge preparation is a controlled honing or grinding step that removes micro-chipping and adds strength. A 0.02–0.05 mm hone is standard for general turning. A 0.05–0.10 mm hone suits roughing and interrupted cuts. A polished edge with no hone is used for aluminium and finishing where sharpness matters more than strength.

The wrong edge prep shows up fast. Too sharp on a hard scale forging and you get micro-chipping within minutes. Too honed on a finishing pass and you get rubbing, poor finish, and heat. If a tool fails early, check the edge prep before you blame the grade.

Tool life is not a fixed number. It depends on speed, feed, depth of cut, material condition, and rigidity. A conservative starting point is 70–80% of the maximum surface speed recommended for the grade. That usually gives a predictable wear pattern and enough warning before a catastrophic failure.

On our shop floor, we log flank wear after every trial run. If flank wear reaches 0.2 mm before the planned tool change, we adjust speed or feed. That simple check has kept our historical late-delivery probability below 2% and our qualification rate at 99.99%.

• 1
  Hone 0.02–0.05 mmGeneral turning and milling.
• 2
  Hone 0.05–0.10 mmRoughing and interrupted cuts.
• 3
  Polished, no honeAluminium and fine finishing.

Aluminium 6061 and 7075 cut easily but build up edge if the speed is too low. Use a polished positive insert, high rake, and surface speeds of 300–500 m/min. Keep the feed per tooth above 0.05 mm to avoid rubbing. A mist or high-pressure coolant helps clear chips from deep pockets.

Stainless 304 and 316 work-harden if the insert rubs. Use a sharp PVD-coated insert with a positive rake and keep the feed per tooth above 0.08 mm. Do not dwell. If the tool pauses in the cut, the surface hardens and the next pass will chip the edge. For 17-4PH, expect shorter tool life and plan for a mid-run insert change.

Titanium Ti-6Al-4V conducts heat poorly, so the cutting edge sees high temperature. Use a sharp PVD AlTiN insert, lower surface speed (40–60 m/min), and generous coolant. Inconel is worse: keep speeds low, use a positive edge, and accept that tool life will be measured in minutes, not hours.

For hardened tool steel above 45 HRC, use a CBN or ceramic insert if the geometry allows. Otherwise, a strong negative carbide insert with a honed edge and low speed will get the job done. The trade-off is cycle time.

• 1
  AluminiumPolished positive, 300–500 m/min, high feed.
• 2
  StainlessPVD sharp, feed above 0.08 mm/tooth, no dwell.
• 3
  TitaniumPVD AlTiN, 40–60 m/min, flood coolant.
• 4
  Hardened steelCBN, ceramic, or honed negative carbide.