Materials

Drilling Aluminium: Speeds, Feeds and Tips

Workshop starting values and practical technique for wrought 6061-T6 and 6082-T6, covering tool geometry, coolant, chips and common drilling faults.

Aluminium conducts heat well but its low melting point makes edge welding the central problem. Silicon-rich cast aluminium is more abrasive than wrought stock and may favour carbide. The figures here are practical starting values for sound machines and correctly ground drills. Exact alloy, hardness, hole depth, coating, coolant delivery and machine rigidity remain decisive, so confirm production settings against the drill manufacturer's data.

Recommended cutting speeds

For wrought 6061-T6 and 6082-T6, begin near 80 m/min (262 SFM) with HSS or cobalt and 250 m/min (820 SFM) with a suitable carbide drill. Cobalt HSS can often run 25–50% faster than plain HSS while retaining hardness at the edge. Use carbide speeds only with rigid workholding, very low runout and coolant conditions that match the tool design.

Spindle speed follows RPM = cutting speed × 1,000 ÷ (π × diameter in mm). Use the nearest lower machine setting for a cautious first hole. Surface speed creates heat while feed creates chip thickness; reducing feed to almost nothing is not a safe substitute for reducing RPM because a rubbing edge generates heat without removing material.

Drilling Aluminium speeds and feeds table

The HSS and carbide columns use the starting surface speeds above. Feed ranges are diameter-based workshop values and should be adjusted within the range for drill geometry, power and rigidity.

Feed per revolution by drill type

Across common diameters, a useful overall band is 0.05–0.30 mm per revolution. Plain HSS jobber drills need conservative feed because their web and hot hardness limit thrust. Cobalt drills use similar chip loads but tolerate heat better. Solid-carbide drills usually need a firm, consistent feed to stabilise the margins and keep the edge cutting; they should not be hand-fed at high carbide surface speeds.

Start near 0.03–0.06 mm/rev for 2–4 mm drills, 0.07–0.12 for 5–8 mm, 0.14–0.20 for 9–13 mm, and 0.20–0.32 for 14–25 mm, then bias the choice for this material and the actual tool catalogue. Reduce thrust for thin sheet as breakthrough approaches and back the work with sacrificial material. For deep holes, preserve chip thickness but reduce surface speed and add reliable pecking rather than allowing flutes to fill.

Drill geometry and point angle

A sound starting geometry is 118–130° with a polished, high-helix flute. A split point lowers the thrust needed to start, reduces walking and is especially valuable without a pilot hole. Both lips must be equal in length and angle; an uneven hand grind makes one lip carry most of the cut, producing an oversized hole and rapid wear. Keep overhang short and use a spotting drill when position matters.

Web thinning reduces thrust on larger conventional drills, but excessive thinning weakens the point. Margin condition controls guidance and final size. Polished flutes reduce friction in adhesive materials, while robust edge honing supports carbide in abrasive work. Coatings are useful only when suited to the work: a coating cannot rescue poor geometry, runout or chip evacuation.

Coolant and lubrication

The normal choice is aluminium-safe soluble coolant, light oil or kerosene-type proprietary cutting fluid. Delivery matters as much as fluid name. Coolant must reach the lips before chips block access; an intermittent splash can thermally shock carbide or merely wet the outside of a deep hole. Through-tool delivery is best for deep CNC holes. On manual machines, stop safely to brush on lubricant and never reach toward a rotating drill.

Keep coolant concentration within its supplier's range and remove contaminated chips. Mist, smoke and fine dust need appropriate extraction and personal protection. If the material is normally cut dry, direct air or vacuum should move chips without spraying them toward people or precision slideways. Do not mix fluids casually, and check compatibility with the work alloy and subsequent finishing process.

Chip behaviour and peck drilling

Aluminium produces chips that are long, bright and ductile; it can weld to the lip and pack the flute. Healthy chips from both flutes should be similar in size and colour. One heavy chip and one light chip indicates unequal lips or runout. Long swarf must be controlled with guards and a chip hook after the spindle stops; never clear it by hand while the machine runs.

Peck once depth approaches three drill diameters, sooner if chips stop leaving freely. Retract far enough to clear the flutes, but avoid rubbing or dwelling when re-entering. Deep-hole cycles need room at the bottom for the point and chips. A parabolic-flute drill improves evacuation, and internal coolant can extend the depth achievable without full retracts. Reduce each peck as the hole deepens if chip travel becomes difficult.

Common problems and fixes

The characteristic risks are built-up edge, oversized holes and flute packing. The first response is to polish the flutes, keep feed positive, add lubricant and peck before chips compact. Also check spindle runout, chuck condition, work support, cutting-lip symmetry and actual hole depth. Changing RPM without correcting a loose setup usually moves the noise rather than solving its cause.

Preventing wandering, chatter and poor finish

Clamp the work flat and support it near the hole. Centre punching can guide a hand drill, but a machine setup is usually more accurate with a short, rigid spotting drill whose included angle is at least as wide as the following drill point. A narrow centre-drill cone can make the outer corners contact first and chip. Avoid large pilot holes; if thrust demands a pilot, keep it near the chisel-edge width so the main lips still cut continuously.

Chatter comes from a flexible loop involving the spindle, holder, drill and workpiece. Shorten every unsupported length, tighten the fixture and move away from the resonant speed. A feed that is too timid can let the margins skate. Poor finish may also come from recutting trapped chips or built-up material on the lips. Measure runout close to the point for critical holes rather than trusting the chuck by appearance.

Breakthrough, sheet and interrupted holes

As the point exits, remaining material becomes thin and cutting forces change abruptly. Ease the linear feed while maintaining control, especially with hand-fed machines. Backing plate reduces burrs and prevents thin sheet from climbing the drill. Step drills are often safer for larger sheet-metal holes. Clamp sheet securely; never hold it by hand because a grabbing drill can spin it like a blade.

Angled entries, curved surfaces, flame-cut edges and cross holes create interrupted loading. Spot-face when possible, use a short rigid drill, and reduce the starting speed. Carbide is vulnerable to chipping when only one lip contacts. A pilot feature, guide bush or specialised geometry may be justified where position or tool life matters.

Tool choice and tool life

HSS is tough, inexpensive and forgiving on manual machines. Cobalt HSS adds hot hardness without losing all that toughness, making it a strong choice for harder or hotter applications. Carbide offers wear resistance and productivity but demands rigidity and controlled runout. Replace or regrind a drill when thrust, noise, burr size or hole diameter trends upward; waiting for catastrophic failure risks the component and holder.

Record tool identity, lot, coating, stick-out, coolant, speed, feed, depth and number of holes. A small reduction in cutting speed often produces a disproportionately large tool-life improvement. Conversely, a speed that survives one trial is not automatically economical in a batch. Stable size, predictable wear and safe chip control matter more than the shortest isolated cycle.

Workshop starting procedure

Verify the material and drawing, select the shortest suitable drill, inspect its edges, and clamp the work. Calculate RPM from the chosen surface speed and select a feed in the diameter range. Arrange coolant and chip guarding before starting. Drill one hole while watching chips and listening for a steady cut. Stop the spindle, inspect the hole and tool, measure critical features, then adjust a single variable at a time.

These recommendations cover both British “aluminium” terminology and the language commonly seen on American tooling charts, where the same metal is spelled “aluminum”. The unit system does not change the cutting physics: convert metres per minute to SFM by multiplying by 3.281, and convert millimetres per revolution to inches per revolution by dividing by 25.4. Preserve enough significant figures to choose a machine setting, not to imply false precision.

Frequently asked questions