Cutting Speeds & Feeds Reference Chart: Drilling, Milling, Tapping, Reaming

Cutting speed (Vc, in metres per minute) and feed rate determine how fast a cutting tool removes material and how long it lasts. The right values depend on material being cut (carbon steel vs stainless vs aluminium vs cast iron vs hardened tool steel), tool material (HSS vs cobalt vs solid carbide), coating (uncoated vs TiN vs TiAlN vs AlCrN), and operation (drilling, milling, tapping, reaming). Get the parameters wrong by 30% in either direction and the tool dies prematurely; get them right and the tool runs at expected life with clean chip formation and minimal heat.

This reference compiles published industry ranges from Machinery's Handbook 31st Edition, Sandvik Coromant's Cutting Tool Handbook, Kennametal Innovations Catalogue, Iscar, Mitsubishi Materials, and OSG Threading Technical Guide. Ranges are wider than any single manufacturer's recommendations — they span typical industry-consensus values for AU machinists working across multiple brand tool sources.

Cutting Speed and Feed Rate Formulas

Spindle Speed (RPM) from Cutting Speed

The fundamental formula every machinist memorises:

n = (Vc × 1000) / (π × D) ≈ Vc × 318 / D

where:

• Vc = cutting speed in metres per minute (from material × tool tables below)
• D = tool diameter in mm
• n = spindle speed in RPM

Feed Rate from Spindle Speed

For drilling: vf = n × f (where f is feed per revolution in mm/rev)

For milling: vf = n × fz × z (where fz is feed per tooth in mm/tooth, z is number of teeth/flutes)

Worked Example — HSS Drill in Mild Steel

• Material: SAE 1018 mild steel, ISO VDI Group 1
• Tool: 10mm HSS uncoated jobber drill
• Recommended Vc (Group 1, HSS uncoated): 25-30 m/min — use 27 m/min midpoint
• Recommended feed (10mm Ø, Group 1): 0.10-0.20 mm/rev — use 0.15 mm/rev midpoint
• RPM = 27 × 318 / 10 = 859 RPM
• Feed rate = 859 × 0.15 = 129 mm/min

Worked Example — Carbide Endmill in Stainless 304

• Material: SAE 304 austenitic stainless, ISO VDI Group 14.1
• Tool: 8mm 4-flute solid carbide TiAlN-coated endmill, slotting
• Recommended Vc: 50-90 m/min — use 70 m/min
• Recommended feed per tooth (fz): 0.025-0.06 mm/tooth — use 0.04 mm/tooth
• RPM = 70 × 318 / 8 = 2,783 RPM
• Feed rate = 2,783 × 0.04 × 4 = 445 mm/min

HSS Drilling — Speeds & Feeds

Reference table for high-speed steel (HSS), cobalt HSS, premium HSSE, and coated HSS drill bits. Values are cutting speed Vc in m/min across published industry ranges. Feed rates apply to typical 6-12mm Ø jobber drills; scale up for larger Ø, down for smaller.

* For HSS in aluminium, TiAlN coating not recommended — Al chemically affinitates with Ti causing built-up edge (BUE). Use AlCrN coating or polished uncoated HSS-Co. ** Same caveat applies to carbide table below.

Carbide (VHM) Drilling — Speeds & Feeds

Solid carbide (VHM) tooling runs 3-5× faster than HSS-Co on the same material. Vc ranges below are for solid carbide drills (typically K15-K30 grade, sub-micron grain). Premium coatings (Aldura, Helica, Black Magic) push the upper end of these ranges further.

** For aluminium, AlCrN coating is preferred — TiAlN reacts chemically with Al causing BUE and poor surface finish. For brass and copper, polished uncoated VHM gives best chip evacuation.

Tapping — Speeds (Vc m/min)

Tapping speeds are typically 30-50% of drilling speeds because the tap has multiple cutting edges engaged simultaneously and limited chip evacuation through the flute. Use spiral-flute taps for blind holes, spiral-point (gun) taps for through holes. Reduce these speeds 10-20% for blind holes vs through holes.

Cold-forming (forming) taps run 30-50% faster than cutting taps in non-ferrous and ductile materials — no chip generated, displaces material instead. Use form taps in aluminium, copper, brass and steels up to ~32 HRC.

Endmill Milling — Speeds & Feeds

Endmill cutting parameters depend heavily on cut type — slotting (full-immersion, ae = D) vs profiling (ae = 0.1-0.5×D) vs finishing (light ae and ap). Below values are for SLOTTING (the most demanding cut). Reduce to ~70% Vc for profiling, increase 10-20% for light finishing passes.

Chip-load principle: total feed rate = RPM × feed-per-tooth × number-of-teeth. Increasing flute count reduces chip space — don't increase teeth without reducing depth-of-cut (ap × ae). For HSM (high-speed machining) with shallow ae/D, use ~2× these Vc values.

Reaming — Speeds & Feeds

Reaming is fundamentally different from drilling — light depth-of-cut (0.1-0.3mm typical), generous feed, slow Vc, and proper coolant or oil are essential. Reamer chatter and bell-mouthed holes typically indicate Vc too high or feed too low.

Maximum stock removal per reamer pass: ~3% of Ø, typical 1-2%. For high-tolerance hole production, drill to (Ø − 0.3-0.5mm) then ream.

Material-Specific Considerations

Stainless Steel (Austenitic 304/316/Duplex)

Austenitic stainless work-hardens rapidly under cutting pressure. Don't dwell. If cutting feels slow or labouring, the answer is speed UP and feed UP together — not slow down. Once work-hardened, the surface becomes harder than the tool and tool failure is rapid. Coolant essential. HSS-Co minimum; carbide TiAlN strongly preferred for production.

Aluminium (Wrought + Cast)

Highest cutting speeds of any common engineering material. BUT — TiAlN coating reacts chemically with aluminium at cutting temperatures. The Ti in TiAlN chemically affinitates with Al, causing built-up edge, premature tool wear and poor surface finish. Use AlCrN coating OR uncoated polished solid carbide for aluminium. Generous feed essential to prevent BUE; ample chip evacuation (high-helix flutes, low flute count) prevents chip recutting.

Brass

Sharp, free-cutting, low cutting force required. Use LOWER feed than steel — brass forms long curling chips that tangle if feed is too high. Generally machine dry or with minimal lubricant. Use SHARP geometry — dull tools cause work hardening.

Cast Iron (Grey & Nodular)

Highly abrasive due to silicon carbide and graphite content. Tool wear accelerates dramatically with insufficient coating. TiAlN coating gives best life; uncoated HSS is rapidly destroyed. Don't use coolant — grey iron is conventionally machined dry, as the graphite acts as a lubricant and water/coolant can cause workpiece corrosion. Use carbide for production-volume work.

Titanium (Ti-6Al-4V Grade 5 + others)

Low thermal conductivity = cutting heat concentrates at the tool tip, not the chip. Very low Vc required (Group 36: 8-12 m/min for HSSE, 30-50 m/min for carbide TiAlN). Coolant flood essential. Avoid speeding up — exponential tool life decrease. Use carbide or PCD for production.

Nickel Super Alloys (Inconel, Hastelloy, Monel)

The most difficult standard engineering materials to machine. Vc < 50 m/min even with carbide TiAlN. Extreme tool wear. Use AlCrN-coated carbide; specialised ceramic or PCBN inserts for production. Generous coolant, sharp geometry, slow Vc, generous feed (don't reduce feed — that accelerates work hardening).

Hardened Steel (above 45 HRC)

HSS tooling is not viable above ~45 HRC — the tool is softer than the workpiece at cutting temperatures. Solid carbide essential, with TiAlN, AlCrN or Aldura coating depending on hardness. PCBN inserts cost-effective for >55 HRC and production-volume.

Coolant and Lubricant Selection

Coolant choice affects tool life as much as cutting parameters. Three approaches:

• Flood coolant — best for most steel and stainless work; cools the cutting zone, evacuates chips, lubricates the tool/workpiece interface. Water-soluble emulsion (synthetic or semi-synthetic) typical.
• MQL (Minimum Quantity Lubrication) — fine oil mist; growing standard for aluminium and titanium machining, reduces coolant cost and disposal.
• Dry machining — required for grey cast iron (graphite acts as lubricant); also viable for aluminium with the right coating.

Tap-specific lubricants matter — see our Tap Magic cutting fluid guide for material-specific selection. For industrial degreaser cleaning between operations: degreaser selection guide.

Frequently Asked Questions

Q: What is Vc in cutting speed?

Vc stands for cutting speed, measured in metres per minute (m/min). It is the linear velocity of the cutting edge relative to the workpiece surface. Vc is the master parameter for cutting tool performance — published per material group × tool material × coating combination. From Vc and tool diameter, you calculate RPM.

Q: How do I calculate RPM from cutting speed?

RPM = Vc × 1000 / (π × D), or in practical form RPM ≈ Vc × 318 / D, where Vc is in m/min and D is tool diameter in mm. Example: 10mm drill at Vc 30 m/min = 30 × 318 / 10 = 954 RPM. Round to the nearest available spindle speed on your machine.

Q: What speed for drilling stainless steel 304?

Cobalt HSS drill (HSS-Co): Vc 10-14 m/min. Carbide TiAlN drill: Vc 60-90 m/min — significantly higher. For a 10mm carbide drill at Vc 75 m/min: RPM ≈ 2,386. Feed 0.08-0.14 mm/rev. Coolant flood essential. Don't dwell — stainless work-hardens on contact.

Q: What speed for milling aluminium?

Aluminium runs at the highest cutting speeds of any common material. HSS-Co endmill in 6061: Vc 70-100 m/min. Solid carbide AlCrN: Vc 200-400 m/min. Use AlCrN coating NOT TiAlN — TiAlN reacts chemically with Al and causes built-up edge. Generous feed essential (0.05-0.15 mm/tooth) to prevent chip recutting.

Q: HSS vs carbide cutting speeds — what's the difference?

Solid carbide runs 3-5× faster than HSS-Co on the same material because carbide retains 80% of its room-temperature hardness at 600°C (HSS retains 25%). A 10mm carbide drill in mild steel runs at Vc 100 m/min vs HSS at 25 m/min — that is roughly 4× faster cycle time. Carbide is brittle — needs rigid setup and continuous cut (no chatter, no interruption).

Q: Should I use coolant when drilling steel?

Yes for most steel work — water-soluble flood coolant cools the cutting zone, lubricates the chip-tool interface, and evacuates chips. EXCEPTIONS: grey cast iron is machined dry (graphite acts as natural lubricant). Some hardened steel applications are dry (high-speed machining with appropriate coatings handles the heat by exporting it in the chip).

Q: Why does my drill bit overheat?

Three common causes: Vc too high (reduce by 20-30%), feed too low (chip is too thin, the drill rubs rather than cuts — increase feed), or insufficient coolant. Discoloured chips (blue or straw colour) indicate excessive heat. Aim for chips that are slightly warm but still bright steel colour.

Q: What feed rate for a 10mm drill in mild steel?

0.10-0.20 mm/rev — use 0.15 mm/rev as a starting midpoint. At Vc 27 m/min (HSS uncoated) and 859 RPM, that gives feed rate = 859 × 0.15 = 129 mm/min. For carbide TiAlN at Vc 150 m/min (4,775 RPM) and feed 0.22 mm/rev, feed rate = 1,051 mm/min — almost 10× faster than HSS.

Q: What's the formula for feed rate in milling?

vf = n × fz × z, where n is RPM, fz is feed per tooth (mm/tooth), and z is number of teeth (flutes). A 4-flute endmill at 3,000 RPM with fz of 0.05 mm/tooth gives feed rate = 3,000 × 0.05 × 4 = 600 mm/min. Reduce z when slotting (full-immersion) to maintain chip space.

Q: Why does aluminium gum up the drill bit?

Built-up edge (BUE) — aluminium chemically affinitates with the tool material under heat and pressure, depositing on the cutting edge. Causes: TiAlN coating (Al-Ti reaction — switch to AlCrN), feed too low (chip too thin), Vc too low (insufficient heat to clear), or worn tool. Solution: AlCrN coating or polished uncoated carbide, increase feed, increase Vc, replace dull tool.

Q: Why is my carbide drill chipping in stainless?

Three causes: feed too low (carbide needs decisive cut, not rubbing — increase feed), Vc too high (carbide grade wrong for material — switch to a tougher K-grade like K20-K30), or unstable setup causing micro-chatter (rigidify the setup, reduce overhang). Stainless work-hardens — once the surface hardens, carbide edges chip. The fix is faster + heavier cut, not slower.

Related AIMS Engineering Reference Guides

• Workpiece Material Cross-Reference Chart — companion to this guide, identify your material group first
• Drill Bit Metric / Imperial Size Chart
• Threading Tap Size Reference
• Cobalt Drill Bit Guide — when HSS-Co outperforms standard HSS
• Carbide vs HSS End Mills — when carbide is worth the cost
• Tap Magic Cutting Fluid Guide

AIMS Cutting Tool Range

AIMS Industrial stocks the cutting tools matched to these parameters:

• Sutton Tools — Australian-made HSS, cobalt and solid carbide range (drills, taps, endmills, reamers)
• Cobalt Drill Bits — for stainless, alloy steel, harder applications
• Carbide Drill Bits — for production-volume and hardened steel work

Need help matching cutting parameters to a specific material × tool × machine setup? Contact AIMS on (02) 9773 0122 — we'll work through the right Vc, feed and coolant for your job.