Cutting Speeds & Feeds Chart
What Is Cutting Speed — and Why It's Not the Same as RPM
Cutting speed is the speed at which the cutting edge moves through the material — measured in metres per minute (m/min) in Australia, or surface feet per minute (SFM/SFPM) in US references. It describes how fast metal is being sheared, not how fast the spindle is turning.
RPM — revolutions per minute — is the spindle speed. The two are related by the diameter of the tool or workpiece. A small-diameter drill running at the same RPM as a large one has a much slower cutting speed at the tip. This is why you can't use a single RPM figure across all jobs: the correct RPM depends on both the cutting speed for the material and the diameter of the tool.
Getting this distinction clear is the foundation of everything else in this guide.
The RPM Formula
The formula converts cutting speed (m/min) and tool diameter (mm) into spindle speed (RPM):
N (RPM) = (CS × 1,000) ÷ (π × D)
Where CS = cutting speed in m/min and D = drill or tool diameter in mm.
Because π ≈ 3.1416, this simplifies to:
N ≈ (CS × 318) ÷ D
This shortcut is accurate enough for any workshop calculation.
If you encounter US references using SFM (surface feet per minute), the equivalent formula is:
N (RPM) = (CS × 3.82) ÷ D (inches)
To convert: 1 SFM ≈ 0.305 m/min. A US chart showing 100 SFM = approximately 30 m/min.
Worked examples
Example 1: Drilling mild steel with a 10 mm HSS drill bit. Recommended cutting speed for mild steel with HSS: 25 m/min.
N = (25 × 318) ÷ 10 = 795 RPM
Example 2: Drilling aluminium with a 6 mm HSS drill bit. Recommended cutting speed for aluminium with HSS: 80 m/min.
N = (80 × 318) ÷ 6 = 4,240 RPM
Example 3: Drilling 304 stainless steel with a 12 mm cobalt drill bit. Recommended cutting speed for stainless with cobalt: 18 m/min.
N = (18 × 318) ÷ 12 = 477 RPM
If your drill press or lathe doesn't reach the calculated speed exactly, set it to the nearest available speed below — running slightly slow is always safer than running fast.
Cutting Speed Reference Table — by Material and Tool Type
These are recommended cutting speeds for general workshop use. They are conservative starting points — experienced machinists may run higher, particularly with carbide tooling on rigid CNC setups. For manual drills, bench drill presses, and lathes, use the lower end of the range.
| Material | HSS (m/min) | Cobalt HSS (m/min) | Carbide (m/min) | Notes |
|---|---|---|---|---|
| Mild steel (up to 250 HB) | 20–30 | 30–45 | 80–120 | Most common workshop material. Start at 25 m/min with HSS. |
| Medium carbon steel (250–350 HB) | 15–25 | 25–35 | 60–100 | Reduce speed as hardness increases. |
| Alloy / tool steel (>350 HB) | 8–15 | 12–20 | 40–70 | Hard materials require cobalt or carbide. HSS wears rapidly above 350 HB. |
| Stainless steel (304 / 316) | 10–18 | 15–25 | 40–70 | ⚠️ Work hardening risk — see warning below. Use cobalt or better. |
| Stainless steel (free-machining 303) | 18–25 | 25–35 | 60–90 | Easier to machine than 304/316. Standard HSS acceptable. |
| Cast iron (grey) | 20–30 | 30–45 | 80–150 | Drill dry — no cutting fluid. Abrasive but not tough. |
| Aluminium alloys | 60–100 | 80–150 | 200–400 | High speeds required. Use cutting fluid to prevent built-up edge. |
| Brass / bronze (free-cutting) | 30–60 | 50–80 | 100–200 | Often drilled dry. Sharp tools essential — dull tools grab. |
| Copper | 25–45 | 40–70 | 100–180 | Ductile — tends to smear. Reduce feed rate. |
| Titanium (Grade 5) | 6–12 | 8–15 | 20–50 | Extremely low speed. Carbide strongly preferred. Flood coolant essential. |
| Nylon / Acetal (POM) | 30–60 | — | 80–200 | Use sharp HSS. Risk of melting at high speed. Drill dry or compressed air. |
| HDPE / UHMWPE | 20–50 | — | 60–150 | Low melting point — keep speeds conservative. Compressed air cooling. |
For more on HSS vs cobalt vs carbide tool selection, see our complete drill bit selection guide.
Drill Speed Chart — RPM by Diameter and Material (HSS)
This table gives calculated RPM values for HSS drill bits across common diameters and materials. Values are rounded to the nearest whole number. Use the mid-range cutting speed for each material as the basis.
Cutting speeds used: Mild steel 25 m/min · Alloy steel 15 m/min · Stainless 12 m/min · Cast iron 25 m/min · Aluminium 80 m/min · Brass 45 m/min
| Drill Ø (mm) | Mild Steel | Alloy Steel | Stainless 304/316 | Cast Iron | Aluminium | Brass |
|---|---|---|---|---|---|---|
| 3 mm | 2,653 | 1,592 | 1,273 | 2,653 | 8,488 | 4,775 |
| 4 mm | 1,989 | 1,193 | 955 | 1,989 | 6,366 | 3,581 |
| 5 mm | 1,592 | 955 | 764 | 1,592 | 5,093 | 2,865 |
| 6 mm | 1,326 | 796 | 637 | 1,326 | 4,244 | 2,387 |
| 8 mm | 994 | 597 | 477 | 994 | 3,183 | 1,790 |
| 10 mm | 796 | 477 | 382 | 796 | 2,546 | 1,432 |
| 12 mm | 663 | 398 | 318 | 663 | 2,122 | 1,194 |
| 16 mm | 497 | 298 | 239 | 497 | 1,592 | 895 |
| 20 mm | 398 | 239 | 191 | 398 | 1,273 | 716 |
| 25 mm | 318 | 191 | 153 | 318 | 1,019 | 573 |
| 32 mm | 249 | 149 | 119 | 249 | 796 | 447 |
| 40 mm | 199 | 119 | 95 | 199 | 637 | 358 |
For cobalt HSS: multiply the stainless steel and alloy steel RPM values by 1.5–1.8. For example, a 10 mm cobalt drill in 304 stainless: 382 × 1.5 = 573 RPM.
For carbide: multiply all HSS values by 3–5 depending on material. See the carbide section below.
For a full drill size reference including fractional and letter sizes, see our drill bit size chart.
⚠️ Stainless Steel: The Work-Hardening Trap
Austenitic stainless steels (304, 316, 316L) work-harden rapidly when the cutting tool dwells, rubs, or moves too slowly through the material. Once the surface work-hardens, you are drilling hardened steel — with a drill bit that was not designed for it. Tools break, holes go off-centre, and the workpiece is often scrap.
The mistakes that cause work hardening:
- Speed too low: The tool rubs rather than cuts. Heat builds without material removal.
- Feed too light: The drill skims the surface instead of biting in. Even at correct speed, inadequate feed causes rubbing on the chisel edge.
- Dwelling: Pausing mid-hole allows the work-hardened layer to form directly at the tip.
- Dull tools: A worn cutting edge rubs. Always use sharp tooling on stainless — cobalt HSS (M35) is strongly preferred over standard M2.
The rule with stainless: commit to the cut. Correct speed, steady feed, sharp cobalt drill, cutting fluid throughout. Do not let the tool pause in the hole.
See our drill bit guide for cobalt drill recommendations and our cutting fluids guide for correct fluid selection on stainless steel.
Carbide and Cobalt: Why More Speed Means Better Results
The most common mistake with carbide tooling is running it at HSS speeds. It feels like the conservative choice — it isn't. Carbide is engineered to work at elevated temperatures. At low speeds, it rubs rather than cuts, generates concentrated heat at the tip, and wears out faster than HSS would in the same application.
Speed multipliers by tool grade
| Tool Grade | Speed vs Standard HSS | Best Applications |
|---|---|---|
| HSS M2 (standard) | Baseline (1×) | General-purpose drilling: mild steel, aluminium, plastics, brass |
| Cobalt HSS M35 (5% Co) | 1.5–1.8× | Stainless steel, alloy steel, hardened materials, abrasive workpieces |
| Cobalt HSS M42 (8% Co) | 1.8–2.2× | High-tensile alloy steels, titanium, Inconel, demanding production work |
| Solid carbide | 3–5× | CNC machining, hard materials, high-volume production, non-ferrous metals |
| Carbide-tipped (insert) | 3–4× | Lathe turning, milling, large-diameter boring |
Running carbide at 1× (HSS speed) is not just suboptimal — the tool will underperform and wear faster than HSS run correctly. If you have changed to carbide but are still using HSS speeds, increase speed progressively until you reach the recommended range.
Important caveat for manual machines: carbide is brittle. It performs at elevated speeds but has less shock tolerance than HSS. On manual drill presses and lathes with vibration or flex, HSS or cobalt is often the better practical choice. Solid carbide is optimised for rigid CNC setups.
Lathe Turning Speeds
The same formula applies to lathe turning — but D is now the workpiece diameter (the diameter being cut, not the finished bore). As you turn material away and the diameter reduces, the cutting speed at the tip drops. On CNC lathes with constant surface speed (CSS) mode, the spindle automatically compensates. On manual lathes, reset speed periodically as the diameter changes significantly. For full coverage of the lathe RPM formula, surface speed by material, G96 vs G97, facing-cut math and chuck speed limits, see our Lathe RPM Formula Guide.
| Material | HSS (m/min) | Carbide Insert (m/min) | Surface Finish Note |
|---|---|---|---|
| Mild steel | 25–35 | 100–200 | Higher speed improves finish. Use cutting oil for HSS. |
| Medium carbon steel | 18–25 | 80–150 | Reduce for heavy roughing cuts. |
| Alloy / tool steel | 10–18 | 50–100 | Keep depth of cut shallow on hard materials. |
| Stainless 304/316 | 15–22 | 50–90 | Consistent feed is critical. Avoid dwelling. |
| Cast iron (grey) | 25–35 | 100–180 | Dry cutting preferred. First pass removes abrasive skin. |
| Aluminium alloys | 80–150 | 300–600 | High speed + sharp tools = excellent finish. Use kerosene or light cutting oil. |
| Brass / bronze | 40–80 | 150–300 | Positive rake angle tools prevent grabbing. Often turned dry. |
| Copper | 30–60 | 120–250 | Ductile — tends to smear. Sharp tool, moderate feed. |
Feed rate for turning (starting point): 0.05–0.15 mm/rev for finishing; 0.2–0.5 mm/rev for roughing. Reduce for hard materials and small diameters.
Milling Cutting Speeds
For end mills and face mills, the cutting speed applies to the tool diameter (not the workpiece). Solid carbide end mills are the standard for CNC milling. HSS end mills are used in manual mills and on softer materials. For full coverage of end mill types, flute count selection by material, coatings (and the AlTiN-on-aluminium trap) and how to choose, see our End Mill Guide.
| Material | HSS End Mill (m/min) | Carbide End Mill (m/min) |
|---|---|---|
| Mild steel | 20–30 | 80–150 |
| Alloy steel | 12–20 | 50–100 |
| Stainless 304/316 | 10–18 | 40–80 |
| Cast iron | 20–30 | 80–150 |
| Aluminium | 60–100 | 200–500 |
| Brass | 30–60 | 100–250 |
Feed per tooth (fz) starting points: 0.01–0.03 mm/tooth for steel with carbide; 0.02–0.05 mm/tooth for aluminium. Multiply by number of flutes to get feed per revolution, then by RPM to get table feed rate (mm/min).
Axial depth of cut: for slotting, keep axial depth ≤ 1× tool diameter. For side milling with radial engagement ≤ 50%, axial depth can be increased to 1.5–2× diameter.
Tapping Speeds
Tapping requires lower speeds than drilling in the same material — the cutting action is more demanding because the tap is removing material across the full thread profile simultaneously. A good starting point is 50–60% of the drilling speed for the same material and tap diameter.
| Material | HSS Tap (m/min) | Cobalt Tap (m/min) | Cutting Fluid |
|---|---|---|---|
| Mild steel | 8–12 | 12–18 | Cutting oil or tapping paste |
| Medium carbon steel | 5–8 | 8–12 | Sulphurised cutting oil |
| Stainless 304/316 | 4–7 | 6–10 | Heavy-duty tapping fluid (e.g. Trefolex) |
| Cast iron | 8–12 | 12–18 | Dry or light oil |
| Aluminium | 15–30 | 25–45 | Kerosene, WD-40, or cutting oil |
| Brass / bronze | 12–20 | 18–30 | Light oil or dry |
| Copper | 8–15 | 12–20 | Light cutting oil |
| Engineering plastics | 10–20 | — | Dry or compressed air |
For machine tapping (tapping head or CNC), match the feed rate precisely to the thread pitch: feed per revolution (mm/rev) = thread pitch (mm). Any mismatch breaks the tap. For more on tap selection, thread forms, and hand tapping technique, see our taps and thread cutting guide. If a tap breaks, see our guide on how to remove a broken tap.
Feed Rate Basics
Cutting speed controls how fast the edge moves through the material. Feed rate controls how much material is removed per revolution — or per tooth on a milling cutter. Both affect tool life, surface finish, and heat generation.
For drilling
Feed rate in drilling is measured in mm per revolution (mm/rev). A practical starting guide:
| Drill Diameter | Mild Steel | Stainless | Aluminium | Brass |
|---|---|---|---|---|
| Up to 3 mm | 0.025–0.05 | 0.02–0.04 | 0.05–0.10 | 0.05–0.10 |
| 3–6 mm | 0.05–0.10 | 0.04–0.08 | 0.10–0.20 | 0.10–0.15 |
| 6–12 mm | 0.10–0.20 | 0.06–0.12 | 0.15–0.30 | 0.15–0.25 |
| 12–25 mm | 0.15–0.30 | 0.10–0.18 | 0.20–0.40 | 0.20–0.35 |
| 25 mm+ | 0.20–0.40 | 0.12–0.20 | 0.25–0.50 | 0.25–0.40 |
Values are in mm/rev. On a manual drill press without a feed rate scale, aim for a steady, consistent downward pressure — not pecking, not forcing. Chips should be curling out of the flutes freely.
Feed rate and tool life
Too low a feed rate (light passes) causes the cutting edge to rub rather than bite. This generates heat without efficient material removal, accelerating wear — and on stainless, causes work hardening. Too high a feed rate overloads the cutting edge, produces vibration, and can snap the drill, particularly at small diameters.
The sweet spot: chips should be continuous curls (for ductile materials like steel and aluminium) or small broken chips (for brittle materials like cast iron and brass). If you're getting dust or powder, feed is too light or the tool is dull.
Cutting Fluid Selection
Cutting fluid reduces heat at the cutting edge, flushes chips from the flute, and improves surface finish. It extends tool life significantly in materials that generate heat (stainless, titanium, alloy steels) and is optional or counterproductive in others.
| Material | Recommended Fluid | Notes |
|---|---|---|
| Mild steel | Soluble cutting oil or neat cutting oil | Standard workshop cutting fluid works well |
| Stainless steel | Heavy-duty tapping/cutting fluid (Trefolex, Tap Magic) | Essential — do not drill dry |
| Alloy / tool steel | Sulphurised cutting oil | High EP (extreme pressure) additive recommended |
| Aluminium | Kerosene, WD-40, or light cutting oil | Prevents built-up edge. Flood preferred on CNC. |
| Brass / bronze | Dry or light oil | Often machined dry at low-to-moderate speeds |
| Cast iron | Dry | Cutting fluid causes cast iron paste — clogs flutes |
| Titanium | Flood coolant (soluble oil) | Continuous flood essential — titanium ignites if chip heat builds |
| Engineering plastics | Dry or compressed air | Most cutting oils attack plastics or cause swelling |
For a detailed breakdown of cutting fluid types, mixing ratios, and brand recommendations, see our cutting fluids and cutting oils guide.
Fault-Finding: What Went Wrong and How to Fix It
| Symptom | Likely Cause | Fix |
|---|---|---|
| Drill bit turns blue or black | Speed too high or cutting fluid absent | Reduce RPM 20–30%. Add cutting fluid. |
| Drill bit burning, tip welded to workpiece | Speed too high + no cutting fluid, or dull tool | Check tool sharpness first. Reduce speed. Use cutting fluid. |
| Drill bit squealing, won't bite | Speed too high or work-hardened surface (stainless) | For stainless: increase feed, ensure sharp cobalt bit. For other materials: reduce speed. |
| Excessive chatter / vibration | Speed too high, loose workpiece, worn spindle, or resonance | Check workpiece clamping first. Change speed up or down by 20% — chatter is resonant and often stops at a different speed, not necessarily slower. |
| Ragged or torn hole finish | Dull drill, too-low speed, or incorrect point geometry for material | Sharpen or replace drill. Increase speed moderately. Check point angle is correct for material. |
| Chips not clearing, drill grabbing | Feed too heavy, flutes clogged, insufficient chip relief | Reduce feed. Peck drill (withdraw periodically) to clear chips. Add cutting fluid. |
| Drill walking / wandering on entry | No centre punch, high speed on entry, or short drill overhang | Centre punch before drilling. Reduce speed on entry. Use a pilot hole for large diameters. |
| Drill breaking on entry | Feed too heavy, drill binding, or hitting the vice jaw | Reduce feed pressure. Check clearance. Use a pilot hole. |
| Oversized hole | Drill running out of true, worn chuck, or dull cutting edge causing deflection | Check runout. Replace chuck jaws if worn. Use a fresh drill bit. |
| Stainless getting harder as you drill | Work hardening from rubbing (speed too low or feed too light) | Increase feed pressure to ensure the drill is cutting, not rubbing. Use sharp cobalt bit. No dwelling. |
The chatter paradox: The instinct when chattering is to slow down. But chatter is a resonant vibration — it occurs at a specific frequency determined by machine stiffness, tool length, and cutting speed. Reducing speed doesn't always stop the resonance; sometimes increasing speed does. Before slowing down, also check the workpiece is rigidly clamped, the tool overhang is as short as practical, and the tool isn't worn.
Deep Holes: When to Adjust Speeds and Feeds
Standard cutting speeds assume hole depth ≤ 4× drill diameter (4D). Beyond this, chip evacuation becomes the constraint. Chips pack in the flutes, generate heat, and dramatically increase the risk of drill breakage.
| Hole Depth | Speed Adjustment | Feed Adjustment | Technique |
|---|---|---|---|
| Up to 4D (standard) | None | None | Continuous cut acceptable |
| 4D–8D | Reduce 10–20% | Reduce 10–20% | Peck drill: withdraw every 2D to clear chips |
| 8D–15D | Reduce 30–40% | Reduce 30–40% | Peck drill every 1–2D with full withdrawal to clear flutes |
| Over 15D | Reduce 40–50% | Reduce 50% | Consider gun drill or deep-hole drill. Coolant through tool preferred. |
In gummy materials like aluminium and copper, chips weld to the flutes quickly. Frequent peck cycles and generous cutting fluid are essential even at standard depths.
For step drill applications where multiple diameters are drilled in a single pass, see our step drill bit guide for speed recommendations by material and step size.
Choosing the Right Drill Bit for the Job
Cutting speed is only part of the equation — the right tool for the material is equally important. A correct speed with the wrong drill geometry will still produce poor results. The three grades in AIMS's drill bit range cover most workshop applications:
| Application | Recommended Grade | Key Materials |
|---|---|---|
| General workshop drilling | HSS M2 (standard) | Mild steel, aluminium, brass, plastics, timber |
| Stainless steel, alloy steel | Cobalt HSS M35 | 304/316 stainless, heat-treated steel, spring steel |
| Hard or exotic alloys | Cobalt HSS M42 | High-tensile alloy, Inconel, titanium (manual machines) |
| High-volume CNC production | Solid carbide | All metals and plastics on rigid CNC setups |
| Carbide-tipped (insert) | Indexable insert drill | Large diameters, production turning and boring |
Drill smarter, not harder.
Shop drill bits & tapping tools from Sutton, Champion & Bordo
Browse AIMS's drill bit range including Sutton Tools, Champion, and Bordo — or visit the taps and threading tools collection for tapping accessories.
For a full breakdown of drill bit types, coatings (TiN, TiAlN, black oxide), and point geometry, see our drill bit selection guide.
Frequently Asked Questions
What is the difference between cutting speed and RPM?
Cutting speed (measured in m/min) is the speed at which the cutting edge moves through the material. RPM is the spindle rotation speed. The two are linked by the tool or workpiece diameter: RPM = (cutting speed × 318) ÷ diameter (mm). A large-diameter tool needs fewer RPM to achieve the same cutting speed as a small-diameter tool.
What is the formula for calculating drill RPM?
In metric: N (RPM) = (CS × 1,000) ÷ (π × D), which simplifies to N ≈ (CS × 318) ÷ D. CS is the cutting speed in m/min and D is the drill diameter in mm. Example: 10 mm HSS drill in mild steel (25 m/min) → (25 × 318) ÷ 10 = 795 RPM.
What is SFM and do I need to use it in Australia?
SFM (surface feet per minute) is the imperial equivalent of cutting speed, used widely in US references and some US-origin tooling data. Australian and metric references use m/min. To convert: divide the SFM value by 3.281 to get m/min. A table showing 80 SFM is approximately 24 m/min.
What cutting speed should I use for mild steel with an HSS drill?
20–30 m/min, with 25 m/min as a practical starting point for standard workshop conditions. For a 10 mm drill, this gives approximately 800 RPM. For a 6 mm drill, approximately 1,300 RPM. Use cutting oil or soluble cutting fluid, and start at the lower end if the machine has any vibration or flex.
Why does carbide need to run faster than HSS, not slower?
Carbide is engineered to work efficiently at elevated cutting temperatures. At low speeds it rubs rather than shears, generating localised heat without efficient cutting — which causes rapid edge wear. Carbide tools should be run at 3–5× the HSS speed for the same material. Running carbide at HSS speeds makes it perform worse than HSS, not better.
What happens if I drill stainless steel too slowly?
Austenitic stainless steels (304, 316) work-harden when the cutting tool rubs rather than cuts. Once the surface hardens, you are drilling hardened steel with a bit not rated for it — the tool fails rapidly and the hole quality deteriorates. Correct speed, steady feed, sharp cobalt drill, and cutting fluid throughout are all required. Never dwell in the hole and never allow the tool to stop under load.
What is feed rate and how is it different from cutting speed?
Cutting speed determines how fast the cutting edge moves tangentially through the material (m/min). Feed rate determines how much material is removed per revolution — measured in mm/rev for drilling and turning. Both affect tool life and surface finish. Too little feed causes rubbing; too much overloads the cutting edge. For drilling, a starting guide is 0.05–0.10 mm/rev for a 6–12 mm drill in mild steel.
What cutting speed should I use for tapping?
Tapping speeds are lower than drilling speeds because the tap cuts across the full thread profile simultaneously. A general starting point is 8–12 m/min for HSS taps in mild steel, and 4–7 m/min in stainless. For machine tapping, the feed rate must exactly match the thread pitch: feed (mm/rev) = pitch (mm). Use cutting fluid on all materials except cast iron and plastics.
What causes chatter, and does slowing down fix it?
Chatter is resonant vibration between the cutting tool and workpiece. It occurs when the cutting frequency coincides with the natural frequency of the setup. Slowing down doesn't always resolve it — sometimes the fix is to increase speed and move away from the resonant frequency. Also check: workpiece clamping rigidity, tool overhang length (shorter is stiffer), and whether the tool is worn. A worn cutting edge is a common overlooked cause of chatter.
How do I know if my drill speed is too fast?
The drill bit tip discolours — turning straw, brown, blue, or black, indicating heat damage. The bit squeals, the cutting edge smears rather than shears, and the swarf is powdery rather than curling chips. On stainless, the workpiece surface becomes noticeably harder to penetrate — a sign of work hardening. Reduce speed by 20–30% and ensure cutting fluid is being applied at the cutting zone.
How do I know if my drill speed is too slow?
Slow drilling in most materials produces poor chip formation (torn rather than clean chips), a rough hole finish, and sluggish progress. In stainless steel, slow speed is more dangerous — it causes the surface to work-harden. In general, if the drill is making no progress despite firm feed pressure, and the tool appears sharp, the speed is likely too low or the work has hardened.
Do I need to reduce speed when drilling deep holes?
Yes. Standard cutting speeds assume a hole depth of 4× drill diameter (4D) or less. Beyond 4D, reduce speed and feed by 10–20% and use a peck drilling technique — withdrawing the drill periodically to clear chips from the flutes. Beyond 8D, reduce by 30–40% and increase the frequency of peck cycles. Chip evacuation is the limiting factor in deep holes, not cutting speed itself.
Can I use the same cutting speeds for drilling and lathe turning?
The recommended cutting speeds for each material are similar but not identical. Turning generally allows slightly higher speeds than drilling because the cutting geometry is more favourable and heat is distributed differently. The main difference is that in turning, D is the workpiece diameter (which reduces as you turn material away), so RPM needs to be adjusted progressively. Use the drilling chart as a starting point for turning, then increase speed moderately if the tool and workpiece allow.
What is the recommended cutting speed for drilling aluminium?
60–100 m/min for HSS, 80–150 m/min for cobalt, and 200–400 m/min for carbide. Aluminium requires high cutting speed for a good surface finish and to prevent the material from building up on the cutting edge (built-up edge or BUE). Use a sharp, polished-flute HSS drill with a light cutting fluid (kerosene, WD-40, or soluble oil) and maintain a consistent feed rate. At low speeds, aluminium galls onto the drill tip.
How much faster can carbide run compared to HSS in the same material?
Typically 3–5× faster. In mild steel: HSS at 25 m/min vs carbide at 80–120 m/min. In aluminium: HSS at 80 m/min vs carbide at 200–400 m/min. The multiplier is higher for materials where carbide's thermal resistance is most valuable — hard steels and titanium. For softer materials like brass and aluminium, the practical benefit of carbide over cobalt HSS is smaller, and cobalt HSS may be the better choice for workshop use due to its greater toughness and lower cost.