CNC Cutting Tool Selection Guide: The Right Tool and Cutting Parameters by Material

🇹🇷 Bu rehberi Türkçe okuyun

Introduction

When you sit down to machine a part, the first question is always the same: “Which tool should I use for this material?” Catalogs list hundreds of options — hardness, alloy, adhesion tendency, thermal resistance. If you don’t know what each is for, you either buy needlessly expensive tools or pick a cheap one and lose the tool within minutes.

This Mentor CNC guide shows which tool to use for each material group, the cutting-speed range and the tips to finish the job fast. It follows the ISO 513 cutting-tool classification; the values are a starting reference to adapt to your own machine.

Section 1: Steels (Group P)

Steels are the backbone of industrial production — automotive, machinery, energy and construction all work with steel. Hardness is usually expressed in Brinell (HB). Very different behaviors hide under the same word “steel.” Note: steels hardened above 45 HRC belong to a separate group, H (Section 6).

Cutting Parameters for Steel

• Turning: P1 → V_c 300, f 0.25, a_p 3–4 mm | P2–P3 → 200 / 0.18 / 2–3 | P4–P5 → 120 / 0.12 / 1–2.
• Boring: P1 → 250 / 0.20 (watch chatter on long bars) | P3 → 160 / 0.15.
• Threading: P1–P2 → 140 | P3 → 100–120 | P5 → 60–80 (coolant needed).
• Drilling: P1 → 180 / 0.20 | P3 → 120 / 0.15 (by diameter).

Golden Rules for Steel

• Lower speed as hardness rises: reduce cutting speed progressively as hardness increases.
• Raise speed to avoid adhesion (P1–P2): very low speed drops temperature and the material welds to the edge (BUE). Don’t run P1 below 200 m/min.
• Cold start on ceramics (P4–P5): halve the speed for the first 30 s, then ramp up; a sudden full speed breaks the edge.
• Coolant is a must (P3 and above): dry cutting cuts life by ≈ 40% in P3.
• Chip control: long/curled chips cause vibration and breakage; use a chip-breaker geometry.

Section 2: Stainless Steels (Group M)

The real value of stainless steel is its corrosion resistance (thanks to nickel/chromium). Medical instruments, food, petrochemical — anywhere corrosion is an issue. Upside: corrosion resistance. Downside: high adhesion tendency; the material sticks to the edge, performance drops and life shortens. The austenitic group is given in HB, the hardened martensitic group in HRC.

Cutting Parameters for Stainless

• Turning: M1–M2 → V_c 100 / f 0.15 / a_p 1–2 | M3 → 80 / 0.12 / 1–1.5 | M4 → 60 / 0.10 / 0.5–1.
• Boring: M1–M2 → 70 / 0.12 (reduce chatter risk).
• Threading: M1–M2 → 50–70 (intensive coolant) | M3–M4 → 40–60.
• Drilling: M1–M2 → 60–80 / 0.10–0.15 | M3–M4 → 40–60 / 0.08–0.12.

Golden Rules for Stainless

• Don’t run the speed too low: below 50 m/min the temperature drops so much the material welds on. 80 m/min gives a better result.
• Coolant is a must: don’t cut dry; oil-based coolant is more effective than water emulsion.
• Consider solid carbide: solid (monolithic) carbide can give ≈ 50% longer life than coated in stainless.
• Don’t drive feed to zero: drop 0.20 → 0.15, but don’t go to 0.08 (hardening/sticking).
• Chip control: long chips worsen adhesion; use a chip-breaker geometry.

Section 3: Cast Irons (Group K)

Cast irons are brittle; used in heavy parts such as engine blocks, pump housings and machine beds. Hardness 150–300 HB. Cutting itself is easy, but vibration and impact can break the tool. The fine dust (silica) it produces is also a health risk.

• Turning (gray): V_c 150 / f 0.20 / a_p 2–3. Nodular: 100 / 0.15 / 1–2.
• Drilling: gray → 100 / 0.15–0.20 | nodular → 70 / 0.10–0.15.
• Facing: gray → 120 / 0.15 / 1–2.

Golden Rules for Cast Iron

• Control vibration: don’t leave the tool over-hanging, clamp the holder tight, prevent impact.
• Cold start on ceramics: halve the speed on first contact and ramp up.
• Dry cutting (gray iron): gray iron can be cut dry; coolant can turn dust into sludge and make things worse. Prefer cooling for nodular/white iron.
• Dust extraction is a must: fine silica dust fouls the machine and harms health; work with extraction.

Section 4: Aluminum and Light Metal Alloys (Group N)

Aluminum is light and easy to machine — but its adhesion tendency is very high. Aerospace, automotive and food industries use it widely. Hardness 50–120 HB. The material tends to weld to the edge; it’s chosen when fast production is needed.

• Turning: pure → 450 / 0.25 / 2–4 | Al-Si → 350 / 0.20 / 2–3 | Al-Mg → 400 / 0.25 / 2–3.
• Boring: pure → 400 / 0.20. Drilling: pure → 300 / 0.20–0.30 | Al-Si → 250 / 0.15–0.25.

Golden Rules for Aluminum

• Use high speed: low speed causes sticking; don’t go below 300 m/min. With PCD, 400–600 m/min is comfortable.
• PCD = an investment: expensive, but one can replace 50–100 ordinary tools; worth it if you machine a lot of aluminum.
• Coolant optional: can be cut dry; oil-based coolant slightly reduces adhesion.
• Chip control is critical: long/curled plastic chips can wrap the spindle; use a chip-breaker geometry.
• Edge sharpness: PCD and solid carbide must be very sharp; dulling drops performance instantly.

Section 5: Titanium and Nickel Alloys (Group S)

Titanium and nickel-based super alloys (Inconel, Hastelloy) are the heroes of aerospace and high-temperature applications; they keep their strength at high temperature. But they are very hard to machine: cutting speeds are low and thermal load concentrates at the edge. Be prepared for long jobs.

• Turning: titanium → V_c 60 / f 0.12 / a_p 0.5–1.5 | Inconel → 40 / 0.10 / 0.5–1.
• Drilling: titanium → 40 / 0.08–0.12 | Inconel → 25 / 0.06–0.10.
• Threading: titanium → 20–30 | Inconel → 15–25 (very slow; be patient).

Section 6: Hardened Steels (Group H)

Hardened steels are machined at 45–68 HRC; machine parts, dies and shafts fall here. It is the transition zone between ordinary and hard steel.

• Turning: 45–50 → 120 / 0.15 / 1–2 (carbide) | 50–55 → 90 / 0.12 / 0.5–1 (carbide) or 140 / 0.10 / 0.2–0.5 (CBN) | 55–62 → 140 / 0.10 / 0.2–0.5 (CBN, finishing).
• Boring: 45–50 → 100 / 0.12 (carbide) | 55–62 → 120 / 0.08 (CBN).
• Facing: 45–50 → 110 / 0.15 / 1–2.

• Test the hardness: tool grade can change completely between 50 and 55 HRC.
• Cold start on CBN/ceramic: first contact is critical above 55 HRC.
• Coolant is effective; use a chip breaker.

Cutting Tool Materials in Brief: What Each One Is and When to Use It

Before reading the table below it helps to know the materials behind the grades. A good cutting tool material needs five things at once: hard (to resist wear and deformation), tough (so it does not fracture), non-reactive with the workpiece, chemically stable, and resistant to sudden temperature changes. No material delivers all five at the top level, which is why the choice depends on the workpiece.

• Cemented carbide: tungsten carbide (WC) grains + a cobalt (Co) binder. Finer grains mean higher hardness; more binder means more toughness but a greater risk of softening under heat (plastic deformation). 80–90% of all inserts are coated carbide. Uncoated carbide (ISO 513 code: HW) is kept for HRSA/titanium and low-speed hard-part turning.
• CVD coating (HC): chemical vapour deposition at 700–1050 °C; thick and highly wear resistant. The Al₂O₃ layer acts as a thermal barrier and prevents crater wear. First choice for steel and stainless turning and for P/M/K milling inserts.
• PVD coating (HC): physical vapour deposition at 400–600 °C; a thin coating that keeps the edge sharp and adds edge toughness. Used on solid end mills and drills, grooving, threading and finishing inserts. Gold-coloured TiN makes wear easy to see; (Ti,Al)N resists oxidation at high temperature.
• Cermet (HT): a carbide based on titanium carbonitride. Resists adhesion and gives bright surfaces and tight tolerances, but its toughness and thermal shock resistance are low. Use it only in finishing, with low feed and depth, preferably dry; change the edge when flank wear reaches 0.3 mm.
• Ceramics (CA / CM / CN / CC): four families: oxide (Al₂O₃; chemically stable but weak against thermal shock), mixed (TiC additions, tougher), whisker-reinforced (SiC fibres; for nickel alloys, allows coolant) and silicon nitride/SiAlON (grey cast iron and HRSA). Their common limit is thermal shock and brittleness; they break in interrupted cuts and with irregular coolant.
• CBN (BN): cubic boron nitride; very high hot hardness. Used for finish turning of hardened steel above 45 HRC; above 55 HRC it is the only cutting material that can replace grinding. In softer steel below 45 HRC the ferrite wears CBN rapidly, so do not use it there. It also works for high-speed roughing of grey cast iron.
• PCD (DP): sintered diamond; the hardest and most wear-resistant material. At high temperature, however, it reacts with iron and dissolves, so it is used only on non-ferrous materials (high-silicon aluminum, MMC, carbon fibre). It is not used on steel or cast iron.

The letter codes in brackets come from ISO 513 and appear next to the grade name on the insert box. The table below summarizes which material group and which speed range each of these materials is used for.

Section 7: Quick Table of Cutting Tool Grades

Section 8: Cutting Parameter Formulas

Section 9: Quick Decision Tree and Warnings

Test-Piece Protocol (If You Don’t Know the Material)

• Lowest risk: coated carbide (CVD). Start at medium speed (V_c 150–180), f 0.15. Machine 1–2 minutes and observe.
• Result: cuts easily → raise speed 20%. Clogs after 30 min → lower 20%. Breaks → lower 30%. Rough surface / part heating → reduce feed (f).

Handling Adhesion

Symptoms: sticking on the tool, rough surface, torn built-up-edge particles. Fixes: raise cutting speed (low speed triggers adhesion); oil-based coolant; increase feed slightly (very low feed = sticking); check tool sharpness (a dull tool causes adhesion).

Impact and Fracture

Symptoms: sudden tool fracture, interrupted chips. Fixes: control vibration (bearings, holder tightness); reduce depth of cut (a_p −30%); switch to a tougher/more suitable grade; apply a cold start on ceramics.

Section 10: Shop Checklist

Conclusion

Cutting tool selection is both science and art: know the material group, learn its hardness, pick the tool from the table, compute the speed with the formulas, test, observe, adjust. Whatever brand you use, the basic rules are the same: low hardness = high speed + PVD coating; medium hardness = medium speed + CVD/cermet; high hardness = low speed + CBN/ceramic + cold start.

This Mentor CNC guide is prepared in light of the ISO 513 classification and industrial practice; always verify parameters against your own material and machine conditions. For the rest of the series, see the Cutting Tools category and our Turning, Milling and Drilling guides.