Complete Guide to CNC Drilling Aluminum
Speeds, feeds, drill selection, chip control, deep-hole strategy, burr control and hole quality — written from production practice, not from a catalog.
Quick answer
CNC drilling aluminum needs a sharp, polished-flute drill, a real feed per revolution, high cutting speed and reliable chip evacuation. Correct parameters depend on the alloy, the hole depth-to-diameter ratio, drill diameter, workholding and machine rigidity — not on a single RPM number. Drilling on its own typically holds around IT11–IT13 on diameter; when a drawing calls for H7/H8 or tight true position, the hole is finished by reaming, boring or helical interpolation.
01Why Aluminum Is Harder to Drill Than It Looks
Every recurring defect in aluminum hole making traces back to the same four material properties. Understanding which property is driving a defect is what turns guesswork into a repeatable fix.
| Property | What it causes at the drill | Typical defect on the part |
|---|---|---|
| High ductility, low melting point 6061-T6 melts around 580–650 °C | Aluminum smears and pressure-welds onto the cutting edge instead of shearing away cleanly | Built-up edge, oversized and out-of-round holes, torn hole wall |
| Long, continuous chips | Chips coil rather than break, then pack into the flutes and stop evacuating | Chip packing, drill seizure, drill breakage, scored hole wall |
| High thermal conductivity ~167 W/m·K for 6061, roughly 3× steel | Heat is dumped into the workpiece and the chip, not carried away by the chip alone | Thermal growth during machining, parts measuring differently hot and cold |
| Low shear strength, high elongation | The last layer of material at breakthrough is pushed ahead of the drill rather than cut | Large exit burrs, cross-hole burrs, deformed thin walls |
The five failure modes below account for the overwhelming majority of aluminum drilling scrap. Each one has its own section later in this guide.
Built-up edge
Welded aluminum on the cutting lip changes the effective geometry and diameter of the drill mid-cut.
Chip packing
Flutes fill, the drill can no longer clear material, torque spikes and the tool seizes or snaps.
Oversized hole
Runout, built-up edge or an off-center web makes the drill cut a hole larger than its nominal diameter.
Exit burr
Material is pushed out at breakthrough instead of being sheared, leaving a ring that must be removed.
Poor hole finish
Re-cut chips and a smearing edge score the wall, so the surface fails the drawing callout.
Nearly always the chip
Four of the five above are chip problems in disguise. Fix evacuation first, then chase parameters.
02How the Alloy Changes the Job
The table below covers the wrought and cast alloys we drill most often in production. Machinability ratings are relative comparisons used across the industry, not absolute measurements — treat them as a starting point for tool and parameter choice.
| Alloy | Machinability | Drilling difficulty | What actually happens at the drill | Typical applications |
|---|---|---|---|---|
| 6061-T6 | Excellent | Easy | The benchmark. Chips break reasonably well in the T6 condition, tool life is long and hole quality is predictable. | General engineering, brackets, housings, jigs |
| 7075-T6 | Good | Medium | Harder and stronger, so cutting forces rise. Reduce cutting speed moderately and watch edge wear; chips are shorter than 6061, which helps evacuation. | Aerospace structure, high-load fittings, tooling |
| 2024-T3/T351 | Fair to good | Medium | Copper-bearing. Abrasive intermetallic particles accelerate flank wear, and in the T3 condition chips run long and stringy. | Aircraft skins and fittings, fatigue-critical parts |
| 5052-H32 | Good | Easy to cut, hard to finish | Non-heat-treatable and very ductile. It drills with low force but produces long gummy chips and the worst exit burrs of the common alloys. | Sheet metal enclosures, marine, fuel and fluid parts |
| 6063-T5 | Good | Easy to cut, gummy | Extrusion alloy, softer than 6061. Prone to smearing and built-up edge if the feed is too light or the edge is not polished. | Extruded profiles, heat sinks, frames |
| A356 / A380 cast | Fair | Hard on tools | Silicon content is the issue, not hardness. Hard silicon particles act as an abrasive; uncoated carbide wears quickly and PCD or diamond-coated tooling pays for itself in volume. | Die-cast and gravity-cast housings, automotive |
03Drill Selection: Which Tool for Which Hole
Spot Drill / Center Drill
A short, extremely rigid tool that creates a conical start so the following drill cannot walk. The point angle of the spot drill should be equal to or larger than the drill that follows, so the drill contacts at its outer corners first and stays centered. A 90° spot followed by a 140° drill is a common and damaging mismatch — the drill lands on its chisel edge in an unsupported cone and can chip.
You can often skip it. A modern solid carbide drill with a 140° self-centering point and a thinned web will start accurately on a flat, clean, square face without spotting. Spotting is genuinely required when the entry face is curved, angled, cast, interrupted or scaled, when using HSS jobber drills, or when true position is tight.
HSS and HSS-Co Twist Drill
Still the right answer for one-off work, soft fixturing, hand-fed operations and older machines with limited spindle speed. HSS tolerates interrupted cuts and marginal rigidity better than carbide because it bends before it breaks. The trade-off is cutting speed: HSS in aluminum runs at roughly 30–60 m/min, against 100 m/min and well beyond for carbide.
For aluminum specifically, look for a high-helix (parabolic) HSS drill rather than a standard jobber. The wider, more open flute is what clears a long aluminum chip.
Solid Carbide Drill
The default for production aluminum on a rigid CNC machine. Higher stiffness holds size and position better, the edge stays sharp far longer, and it supports the cutting speeds that keep aluminum from smearing. A ground, polished-flute solid carbide drill with a 140° self-centering point will typically start without spotting and hold diameter within a few hundredths of a millimeter over its life.
Carbide is unforgiving of what HSS tolerates: runout, a loose vice, a long tool overhang or an interrupted entry will chip it. Check runout at the drill tip before blaming the tool.
Through-Coolant (Internal Coolant) Drill
Coolant is delivered through channels inside the drill body and exits at the point. This does two things external coolant cannot: it cools the cutting edge where the heat actually is, and it flushes chips up and out of the flutes under pressure. Beyond roughly 4–5×D, external flood coolant simply does not reach the bottom of the hole — the chip column blocks it.
A through-coolant drill often lets you run a deep hole in a single pass at full feed where a solid drill would need heavy pecking, so cycle time can drop dramatically. It requires a machine with a through-spindle coolant system and adequate pressure; low pressure through a small-diameter drill achieves nothing.
Step Drill
A single tool that produces two or more diameters, or a hole plus its chamfer, in one plunge. In production this removes a tool change and guarantees the chamfer is concentric with the hole. Step drills are also the practical answer for thin sheet, where a conventional twist drill grabs and triangulates the hole as it breaks through.
The limitation is flexibility: the step geometry is fixed, so a design change means a new tool. Reserve them for stable, repeating features.
Helical Interpolation with an End Mill
Not a drill at all, but often the better answer. Milling a hole in a helical path lets one end mill produce any diameter above its own, adjusts size through cutter compensation without buying a new tool, and generates short chips that evacuate easily. It is the standard approach for large holes where a drill of that diameter would exceed the machine’s torque, and for holes where position accuracy is critical.
The trade-off is cycle time on small holes — below roughly 12 mm a drill is almost always faster. We compare the two approaches in Is CNC Drilling the Same as Milling?
| Tool | Best for | Avoid when | Typical cutting speed in aluminum |
|---|---|---|---|
| HSS / HSS-Co twist | Prototype, low volume, less rigid setups | Production volume, high spindle speed available | 30–60 m/min |
| Solid carbide | Production, tight size, good finish | Excessive runout, weak workholding, interrupted entry | 100–200 m/min |
| Through-coolant carbide | Depth beyond 4×D, short cycle time | No through-spindle coolant, or low pressure | 150–300 m/min |
| Step drill | Hole plus chamfer, thin sheet | Geometry still changing between revisions | As per the largest step diameter |
| PCD / diamond-coated | High-silicon cast alloys such as A356 and A380 | Low volume — tool cost is not recovered | 200–500 m/min |
| Helical interpolation | Large or non-standard diameters, tight position | Small holes in volume — slower than drilling | Per end mill recommendation |
04Drill Geometry That Actually Matters
Point angle — why 118°, 135° and 140° are not interchangeable
| Feature | Recommended for aluminum | Why it matters, and what goes wrong otherwise |
|---|---|---|
| Point angle | 130°–140° for solid carbide; 118° acceptable for HSS |
A flatter point distributes the cut, reduces thrust and self-centers, which is what allows spot-free starting. Sharper points penetrate easily but walk on entry and leave a larger exit burr because more material is pushed rather than sheared. |
| Helix angle | 35°–45° (high helix) | The single most aluminum-specific choice. A high helix acts like an auger and lifts the long aluminum chip out of the hole. A standard 30° helix, and certainly a low-helix drill intended for hardened steel, will pack solid in a deep aluminum hole. |
| Web thickness | Thin or thinned web | The web is the drill’s core. A thick web is stiff but its chisel edge extrudes rather than cuts, raising thrust sharply and pushing the drill off center. Web thinning cuts thrust noticeably and improves centering — it is a standard feature on good carbide drills. |
| Margin | Narrow, polished, often double margin | The margin is the narrow land that rubs the hole wall. Wide margins generate friction and are where aluminum welds itself to the drill. A double margin adds guidance for straightness in deep holes without adding contact width. |
| Flute surface | Ground and polished | A polished flute lowers the friction the chip sees on its way out. On a rough, as-sintered flute an aluminum chip drags, heats and eventually welds. This is a real and measurable difference in aluminum, far more than in steel. |
| Coating | Uncoated polished carbide, DLC, ZrN or TiB2. PCD/diamond for high-silicon cast alloys. |
See the warning below — this is the most frequently mis-specified item on the list. |
05Speeds and Feeds for Drilling Aluminum
Starting cutting speeds by alloy
These are working ranges for solid carbide drills with flood or through-tool coolant, at a depth of up to about 3×D. Use the lower end of each band for larger diameters, longer tools, weaker workholding or mist-only coolant.
| Alloy | Vc — solid carbide | Vc — HSS | Feed per rev (fn) | Preferred coolant | Note |
|---|---|---|---|---|---|
| 6061-T6 | 120–200 m/min | 35–60 m/min | 0.015–0.020 × D | Flood or through | The reference case; most forgiving |
| 7075-T6 | 100–160 m/min | 30–50 m/min | 0.015–0.020 × D | Flood or through | Higher strength, so lower Vc; watch flank wear |
| 2024-T3 | 90–150 m/min | 25–45 m/min | 0.012–0.018 × D | Flood | Abrasive; plan tool changes by hole count |
| 5052-H32 | 100–160 m/min | 30–50 m/min | 0.015–0.020 × D | Flood | Gummy; never let fn drop — rubbing makes it worse |
| 6063-T5 | 120–200 m/min | 35–60 m/min | 0.015–0.020 × D | Flood or MQL | Soft and sticky; polished flute is essential |
| A356 / A380 cast | 100–200 m/min (PCD: 200–400) | Not recommended | 0.010–0.015 × D | Flood | Silicon abrades carbide; diamond tooling for volume |
Worked starting values — 6061-T6, solid carbide, Vc = 150 m/min
This is the table to hand an operator. Spindle speeds are rounded to practical values, and the small-diameter rows are capped at 12,000 rev/min because most vertical machining centers will not exceed it — if your spindle is limited to 8,000 rev/min, accept the lower cutting speed rather than dropping the feed to compensate.
| Drill ø | Spindle speed n | Feed/rev fn | Feed rate Vf | Effective Vc | Cycle at L/D ≤ 3 |
|---|---|---|---|---|---|
| 3 mm | 12,000 rev/min (capped) | 0.05 mm/rev | 600 mm/min | 113 m/min | G81, full feed |
| 5 mm | 9,500 rev/min | 0.09 mm/rev | 855 mm/min | 149 m/min | G81, full feed |
| 6 mm | 8,000 rev/min | 0.11 mm/rev | 880 mm/min | 151 m/min | G81, full feed |
| 8 mm | 6,000 rev/min | 0.14 mm/rev | 840 mm/min | 151 m/min | G81, full feed |
| 10 mm | 4,800 rev/min | 0.17 mm/rev | 816 mm/min | 151 m/min | G81, full feed |
| 12 mm | 4,000 rev/min | 0.20 mm/rev | 800 mm/min | 151 m/min | G81, full feed |
| 16 mm | 3,000 rev/min | 0.25 mm/rev | 750 mm/min | 151 m/min | Check spindle torque |
| 20 mm | 2,400 rev/min | 0.28 mm/rev | 672 mm/min | 151 m/min | Consider helical interpolation |
Coolant strategy
| Method | Where it belongs | Strength | Limitation |
|---|---|---|---|
| Flood emulsion | General production, holes to about 4×D | Good bulk cooling, washes chips off the part, low cost | Cannot reach the bottom of a deep hole once chips fill it |
| Through-tool coolant | Deep holes, high-volume work, unattended running | Cools the edge and flushes chips out under pressure | Needs a through-spindle system and adequate pressure |
| MQL (minimum quantity lubrication) | Shallow holes, thin parts, dry-chip recovery | Excellent lubricity against adhesion; chips stay dry and sellable | Limited cooling; not suitable beyond about 3×D |
| Compressed air only | Very shallow holes, sheet, prototype work | Clears chips, no fluid to clean off the part | No lubrication, so built-up edge risk rises sharply |
| Fully dry | Rarely appropriate for aluminum | — | Aluminum welds to the tool almost immediately without lubricity |
06Drilling Cycles: G81, G83 and G73
| Code | Name | Tool motion | When to use it in aluminum |
|---|---|---|---|
G81 | Drilling cycle | Feed to depth, rapid retract to the R or initial plane. | Holes to roughly 3×D. Also correct for deeper holes when using a through-coolant drill that can clear chips on its own. |
G82 | Drill with dwell | As G81, plus a programmed pause at the bottom. | Spot facing, counterbores and chamfers where a flat, clean bottom face is required. |
G73 | High-speed peck | Feeds down by Q, retracts a small fixed amount, feeds again. The tool never leaves the hole. | Roughly 3–5×D. Breaks the long aluminum chip so it can be carried out, without paying the time cost of full retracts. |
G83 | Peck (deep hole) cycle | Feeds down by Q, retracts all the way to the R plane, then rapids back down before cutting again. | Beyond 5×D without through-coolant. The only cycle that genuinely evacuates chips and lets coolant back to the bottom. |
No.5114; on Haas it is Setting 22. If G73 is not breaking chips as expected, check that value before changing anything in the program — a retract set to 0.1 mm will not break an aluminum chip.
(TOOL 4 = 8MM SOLID CARBIDE DRILL, 140 DEG, HIGH HELIX) T4 M6 G90 G54 G0 X40. Y25. (position over hole) G43 H4 Z25. M3 S6000 (tool length on, spindle 6000 rev/min) M8 (coolant on - allow it to reach the tool) G83 X40. Y25. Z-48. R2. Q12. F840. (peck 12mm, full retract to R2) X70. Y25. (cycle repeats at each new position) X100. Y25. G80 (cancel cycle) G0 Z25. M9 M5
G83 with an I/J/K variable-peck form. Siemens 840D uses cycles rather than G-codes — CYCLE81, CYCLE83 — with named parameters. Heidenhain uses CYCL DEF 200 DRILLING and CYCL DEF 203 UNIVERSAL DRILLING. The strategy in this section is the same on all of them; only the syntax changes. Always confirm against the manual for your specific control and version.
07Deep Hole Drilling in Aluminum
| Depth (L/D) | Recommended approach | Speed factor | Feed factor | Watch for |
|---|---|---|---|---|
| up to 3×D | Standard carbide drill, G81 full feed | 100% | 100% | Nothing unusual |
| 3–5×D | G73 chip breaking, or through-coolant with G81 | 90% | 90% | Chip color and form at the flute exit |
| 5–8×D | Through-coolant drill strongly preferred; otherwise G83 | 80% | 80% | Rising spindle load through the cut |
| 8–12×D | Through-coolant long drill, pilot hole, G83 with reducing Q | 70% | 70% | Hole straightness and diameter drift at depth |
| 12–20×D | Dedicated deep-hole drill, high coolant pressure, rigid pilot | 60% | 60–70% | Runout is now the dominant variable |
| beyond 20×D | Gun drilling or BTA — a different process, not a longer drill | Process-specific | Requires dedicated equipment and setup | |
Speed and feed factors are applied to the values from Section 05. They are cumulative with any reduction already taken for the alloy or the setup.
The four things that decide whether a deep hole succeeds
- Runout, measured at the tip. A deep drill amplifies every thousandth of runout in the holder. Aim for under 0.02 mm total indicated runout for holes beyond 5×D, and under 0.01 mm beyond 10×D. A shrink-fit or high-precision hydraulic holder is not a luxury here — a standard ER collet chuck often cannot hold it.
- A correct pilot hole. Start with a short, rigid drill of the same nominal diameter, to a depth of about 1.5–2×D, and with a point angle equal to or wider than the deep drill. A pilot that is undersized forces the long drill to cut on its corners; a pilot with a narrower point angle leaves the long drill unsupported at its center.
- Coolant pressure, not coolant volume. Through-tool coolant needs pressure to push a chip column upward. Small-diameter deep drills in particular need high pressure to work at all. If the machine cannot supply it, the honest answer is to change the process, not to push the tool.
- Reducing the peck as you go. The first peck can be aggressive; the last should not be. Evacuation difficulty rises with depth, so the Q value should fall with depth. Variable-peck forms of the cycle exist on most controls specifically for this.
08Chip Evacuation — the Real Problem in Aluminum
Three distinct chip failures
Chip welding
Aluminum pressure-welds to the cutting edge and the flute wall. The drill effectively grows a new, wrong-shaped cutting edge out of the workpiece material.
Driven by: low feed per revolution, insufficient lubricity, aluminum-bearing coatings, unpolished flutes.
Chip packing
The flute volume fills faster than chips can leave. Torque climbs, coolant is blocked, and the tool either seizes or snaps.
Driven by: depth beyond the cycle’s capability, low helix angle, no peck, coolant that cannot reach the tip.
Re-cutting chips
Chips that fell back into the hole are cut a second time. They score the wall, damage the margin and can wedge the drill.
Driven by: insufficient retract height, chips left in a blind hole, blowing chips back in with air.
The countermeasures, in the order worth trying
- Get the feed per revolution right first. Most “chip problems” are actually a feed that is too light. A proper chip load produces a chip thick enough to break and stiff enough to travel.
- Use a high-helix, polished-flute drill. Geometry moves the chip; parameters only create it.
- Match the cycle to the depth. G81 to 3×D, G73 to 5×D, G83 beyond — as covered in Section 06.
- Deliver coolant where the cutting is. Through-tool beyond 4×D; flood positioned to actually hit the hole, not the vice.
- Add an air blast for blind holes. Directed to lift chips out of the hole, not across it. A poorly aimed air jet pushes chips straight back in.
- Raise the retract plane on blind holes. Retracting only 1 mm above the face on a G83 does not give the chip anywhere to go.
- Clear the fixture between parts. Aluminum chips that build up around a vice will find their way back into an open hole.
09Burr Control
| Burr location | Why it forms | How to control it at the machine |
|---|---|---|
| Entry | Material is displaced upward as the drill point enters, especially with a sharp point angle or a worn edge. | Spot or chamfer first; keep the edge sharp; a chamfer cut after drilling removes it completely and cheaply. |
| Exit | The remaining wall becomes too thin to support the thrust, so it bends outward and folds instead of shearing. | Reduce feed to roughly 30–50% over the last 1–2 mm of breakthrough; support the exit face with a backing plate or sacrificial material; use a sharp, unworn drill; consider a step drill or a back-chamfer tool. |
| Cross hole (intersecting bores) | The drill breaks into an existing bore at an angle, with nothing behind the cut and no way to reach the resulting burr. | Drill the cross hole before the main bore where the sequence allows; otherwise plan abrasive flow machining, thermal deburring or a dedicated back-deburring tool into the route. |
| Thin wall / sheet | The part flexes away from the drill, then springs back; the hole triangulates and the edges tear. | Use a step drill or sheet-specific geometry; clamp close to the hole; back the sheet with sacrificial material; reduce thrust with a flatter point angle. |
Deburring methods and where each belongs
| Method | Best for | Cost per part | Limitation |
|---|---|---|---|
| In-cycle chamfer tool | Accessible entry and exit faces, production volume | Very low | Needs tool access to both sides of the feature |
| Back-chamfer / reverse deburr tool | Blind-side hole edges reachable through the hole | Low | Diameter-specific; fragile in small sizes |
| Manual deburring | Prototypes, low volume, awkward geometry | High and variable | Operator-dependent, hard to guarantee consistency |
| Vibratory / tumble finishing | Small parts in batches, uniform light edge break | Low in volume | Can round sharp features you wanted to keep |
| Abrasive flow machining | Internal cross-hole intersections, hydraulic manifolds | Medium to high | Specialist process, fixturing cost |
| Thermal deburring (TEM) | Complex internal burrs across many holes at once | Medium in volume | Specialist equipment; not suited to all geometries |
10Hole Accuracy: Drilling, Reaming, Boring and Interpolation
| Process | Typical diameter capability | Typical surface finish | What it is actually good at |
|---|---|---|---|
| Drilling | IT11–IT13 roughly ±0.05 to ±0.15 mm depending on diameter |
Ra 1.6–6.3 µm | Removing material quickly and establishing the hole. Not a sizing operation. |
| Reaming | IT7–IT8 roughly ±0.01 to ±0.02 mm in common sizes |
Ra 0.8–1.6 µm | Sizing and finishing an existing hole. A reamer follows the hole it is given — it corrects size, not position. |
| Boring | IT6–IT7 or better, equipment dependent | Ra 0.4–1.6 µm | Correcting both size and position, and producing non-standard diameters. The slowest and most controllable option. |
| Helical interpolation | Good true position; diameter controlled by cutter compensation | Ra 0.8–3.2 µm | Large or non-standard diameters, tight position, and any size adjustment without a new tool. |
11Eight Common Aluminum Drilling Problems and How to Fix Them
These are the failure modes that actually generate scrap and rework on aluminum jobs. For each one, the left column is what is really causing it — which is often not the obvious answer — and the right column is the order in which to change things. Change one variable at a time, and record what you changed.
Drill breakage, usually part-way down a deep hole
Likely cause
- Chips packing in the flutes and jamming the drill — by far the most common cause in aluminum.
- Coolant not reaching the cutting edge, so the chip welds and the flute loses its clearance.
- Peck depth left constant beyond about 5×D instead of being reduced as the hole gets deeper.
- Excessive runout in the holder, which loads one lip far more than the other.
- Feed reduced "to be safe", which produces stringy chips instead of broken ones.
What to change
- Switch from G81 to G73, and beyond 5×D switch to G83 with full retract.
- Reduce peck depth progressively as depth increases — not a single fixed
Qfor the whole hole. - Move to a through-coolant drill above 5×D if the machine supports it.
- Check runout at the drill shank; target under 0.02 mm TIR for deep holes.
- If chips are long and stringy, increase feed slightly rather than reducing it.
Built-up edge and aluminum welding to the flutes
Likely cause
- An aluminum-hostile coating — TiAlN and AlTiN both promote adhesion in aluminum.
- Cutting speed too low, so the chip smears instead of shearing cleanly.
- Feed too light, so the edge rubs and generates heat without removing material.
- A rough, unpolished flute surface that gives the chip somewhere to key into.
- Insufficient coolant concentration or flow at the cutting zone.
What to change
- Use uncoated polished carbide, or a DLC, ZrN or TiB2 coated drill designed for aluminum.
- Raise the cutting speed into the recommended band for the alloy rather than backing it off.
- Bring the feed up to roughly 0.015–0.02 × D per revolution.
- Increase coolant flow and check the emulsion concentration against the supplier specification.
- Inspect the flutes between holes on a long run; a drill that has started welding will not recover on its own.
Hole comes out oversized
Likely cause
- Runout in the spindle, holder or collet — the drill sweeps a circle larger than its own diameter.
- Unequal lip lengths after regrinding, so one lip does all the cutting and the drill is pushed sideways.
- No spot drill, so the drill wanders on entry and enlarges the mouth of the hole.
- An overly long, unsupported drill flexing under load.
- Expecting a drilled hole to hold a tolerance that drilling cannot hold in the first place.
What to change
- Measure runout with an indicator at the drill body, not at the holder taper.
- Use hydraulic, shrink-fit or high-accuracy collet holding rather than a worn ER collet.
- Spot the hole first, or use a self-centering 135° split-point drill.
- Shorten the drill projection to the minimum that clears the feature.
- If the print calls for H7 or H8, plan a reaming or boring operation — do not chase it with the drill.
Hole position is out of tolerance
Likely cause
- The drill walked on entry, particularly on a curved, angled or cast surface.
- Work offset or datum set from the wrong feature, so every hole is shifted together.
- Part lifting or shifting in the fixture under thrust load.
- Spot drill diameter smaller than the drill, leaving no chamfer for the drill point to seat into.
- Position measured from a different datum than the one used to set the job.
What to change
- Spot with a drill larger in diameter than the hole, at a point angle wider than the drill point.
- Re-verify the work offset before blaming the tool — a whole pattern shifted the same way is a datum problem. See our CNC machining process for how datums are set in production.
- Add clamping or support directly under the hole location.
- On angled or cast faces, mill a small flat before spotting.
- Confirm the inspection datum matches the drawing datum scheme before rejecting parts.
Heavy burrs at the hole exit
Likely cause
- Full feed maintained right through breakthrough, so the last of the material is pushed rather than cut.
- Worn drill — a dull point tears the exit instead of shearing it.
- Thin or unsupported wall at the exit face, which deflects away from the drill.
- Soft, gummy alloy such as 1100 or 5052 that simply tends to form a lip.
- Breaking through into an intersecting bore or a cavity with no backing.
What to change
- Reduce feed to roughly half over the last 1–2 mm of breakthrough.
- Set a tool-life limit by hole count rather than waiting for visible wear.
- Back up the exit face with a sacrificial plate or fixture support where geometry allows.
- Add a controlled back-chamfer or a deburring pass to the program rather than leaving it to hand work.
- Specify the required edge condition on the drawing so it is quoted and inspected, not assumed.
Poor bore surface finish — scoring, smearing or a dull grey wall
Likely cause
- Chips being dragged back up the flutes and re-cut against the finished wall.
- Built-up edge material transferring from the flute onto the bore.
- Margin of the drill rubbing because the drill is bent, worn or running out.
- Coolant breaking down or too dilute, so lubricity is lost.
- Retracting under feed instead of rapid, which lets the drill polish and smear the wall.
What to change
- Improve chip evacuation first — finish problems in aluminum are usually chip problems.
- Change to an aluminum-specific geometry with polished flutes and a high helix angle.
- Verify runout, and replace any drill that has visible flank wear or aluminum build-up.
- Check coolant concentration and filtration; recycled coolant full of fines will score the bore.
- If the print requires a specific Ra in the bore, plan reaming or boring rather than relying on drilling.
Chip packing and long stringy swarf
Likely cause
- Feed per revolution too low to break the chip — the classic aluminum mistake.
- Low helix angle drill that does not lift chips out of the hole quickly enough.
- Peck cycle not used at all, or
Qset too large for the depth. - Wrought alloys such as 1100, 3003 and 5052 that are naturally gummy.
- Air blast used alone on a deep hole, with no flushing action.
What to change
- Increase feed per revolution first — heavier chip loads break more reliably.
- Use a high-helix (35–40°) aluminum drill and a G73 chip-breaking cycle.
- Reduce
Qand let the cycle break the chip more often rather than fighting it. - On gummy alloys, accept shorter pecks and higher coolant pressure as the normal condition.
- Watch the chip form at the spindle — short C-shaped chips mean the parameters are right.
Coolant delivery failure on deep or through-coolant holes
Likely cause
- Blocked coolant channels in a through-coolant drill, often from fines in unfiltered coolant.
- Through-spindle coolant pressure too low for the hole depth and drill diameter.
- Flood nozzles aimed at the spindle rather than at the hole.
- Coolant tank level dropping during a long unattended run.
- Air pockets forming in the line after a tool change, so the first holes run dry.
What to change
- Filter the coolant properly and flush the drill channels when a tool is loaded.
- Raise through-spindle pressure with hole depth; deep small-diameter holes need the most.
- Program a short coolant-on dwell before the first peck after a tool change.
- Add tank level and pressure checks to the shift start-up routine.
- Treat any hole cut without coolant as suspect — inspect it rather than assuming it is fine.
12Drilling Aluminum vs Drilling Steel
Most drilling habits are learned on steel, and almost all of them need adjusting for aluminum. The two materials fail in opposite directions: steel punishes you for going too fast, aluminum punishes you for going too slow and too light. If you carry steel parameters straight across, you will get built-up edge, stringy chips and poor bores.
| Factor | Aluminum | Carbon & alloy steel |
|---|---|---|
| Cutting speed (carbide) | Roughly 100–200 m/min — speed is your friend | Roughly 60–110 m/min — speed is the limit |
| Dominant failure mode | Adhesion, built-up edge, chip packing | Abrasive and thermal wear at the cutting edge |
| Chip behavior | Long, ductile, tends to string and weld | Shorter, more brittle, breaks more readily |
| Helix angle | High, typically 35–40° for fast evacuation | Standard 25–30° |
| Point angle | 118° or 135° split point | 135° or 140° for harder grades |
| Coating | Uncoated polished, DLC, ZrN, TiB2; never TiAlN/AlTiN | TiAlN and AlTiN are the standard choice |
| Feed philosophy | Feed heavier to break the chip — light feed causes smearing | Feed moderately; excess feed chips the edge |
| Thermal behavior | Conducts heat into the part; part growth is a real accuracy issue | Heat stays in the chip and tool; part growth is smaller |
| Coolant role | Primarily flushing and lubrication to stop welding | Primarily cooling the cutting edge |
| Burr formation | Heavy, ductile burrs; deburring is a planned operation | Smaller, more brittle burrs |
| Peck strategy | G73 chip breaking early, G83 beyond about 5×D | G83 used earlier because chip load is the constraint |
| Typical tool life driver | Adhesion and coolant delivery | Cutting speed and edge temperature |
13How We Drill Aluminum in Production
Everything above is process theory. What follows is how it is actually sequenced on our shop floor in Xiamen, where aluminum hole features are produced daily across automotive, machinery, electronics and medical work. The sequence matters more than any single parameter: each stage removes a specific source of error, and skipping one moves that error into the finished part.
Two habits do most of the work. First, we set the drilling parameters from the alloy and the depth ratio, not from a shop-wide default — a 6061 bracket and a 7075 fitting do not get the same numbers. Second, the inspection method is chosen at process planning, not after the first article. If a hole is going to be checked with a plug gauge, the process has to be capable of that before the job runs, not argued about afterwards.
Where the process gets tightened
- Threaded holes. Tapping drill size is checked against the required thread engagement, not taken from a generic chart, because aluminum threads strip easily when engagement is over-specified.
- Deep holes above 10×D. Runout is verified on the machine, coolant pressure is recorded, and peck depth is stepped down through the hole.
- Thin-wall housings. Exit-side support and reduced breakthrough feed are built into the program rather than left to the operator.
- Sealing faces. Where an O-ring or gasket crosses a hole, the edge condition is specified and inspected because a burr there is a leak path.
Typical aluminum hole work we run
- Automotive and machinery brackets in 6061-T6 — bolt patterns where true position matters more than hole size.
- Electronics and heat-sink plates in 6063 and 6061 — large hole counts, burr-free requirement on both faces.
- Structural fittings in 7075-T6 — higher strength, tighter fits, more reaming and boring in the route.
- Cast housings in A356 and ADC12 — abrasive silicon content, so PCD or diamond-coated tooling and controlled tool-life limits.
14CNC Aluminum Drilling FAQs
What speed and feed should I use for drilling aluminum?
For solid carbide drills in 6061 aluminum, a common starting point is a cutting speed of 120–200 m/min with a feed of roughly 0.015–0.02 mm per revolution per millimeter of drill diameter. Convert speed to spindle RPM with n = Vc × 1000 ÷ (π × D), then feed rate with Vf = n × fn. So a 6 mm drill at 150 m/min runs about 7,960 RPM at roughly 0.10 mm/rev, which is about 800 mm/min. Reduce speed for 7075 and cast alloys, and treat every published figure as a starting value to be confirmed against your machine, holder rigidity and coolant delivery.
Do I need peck drilling for aluminum?
It depends on depth. Below about 3×D a straight G81 cycle with good coolant is usually enough. From roughly 3×D to 5×D, a G73 high-speed peck cycle breaks the chip without losing cycle time. Beyond 5×D you need G83 full-retract pecking so the chips are actually cleared from the hole rather than just broken. The reason is that aluminum chips are ductile and will pack in the flutes, and a packed flute is the single most common cause of drill breakage in aluminum.
What is the best drill bit for aluminum?
For most production work, a solid carbide drill with a high helix angle of 35–40°, polished flutes, a 135° split point and either no coating or an aluminum-friendly coating such as DLC, ZrN or TiB2. High-speed steel is acceptable for occasional or low-volume work, and PCD or diamond-coated drills are worth the cost in abrasive high-silicon cast alloys such as A356 and ADC12. Above about 5×D, a through-coolant carbide drill will outperform anything else.
Why does my drill keep breaking or grabbing in aluminum?
Almost always chip packing rather than excessive load. Aluminum produces long ductile chips that jam in the flutes, and the drill then either seizes or snaps. The usual contributing factors are a feed that is too light to break the chip, no peck cycle or too large a peck depth, coolant not reaching the cutting edge, and excessive runout. Counter-intuitively, the first fix is usually to increase the feed per revolution, not reduce it — a heavier chip breaks more reliably than a thin one.
Can you drill aluminum without coolant?
Shallow holes below about 2×D can often be drilled with air blast or minimum quantity lubrication, and this is common on high-speed machines because it keeps the chips out of the hole. Anything deeper needs real coolant, because aluminum's problem is adhesion rather than heat: without lubrication the chip welds to the cutting edge, builds up, and destroys both the hole finish and the drill. Never run a deep or through-coolant drill dry.
What tolerance can drilling hold in aluminum?
A drilled hole is a roughing feature. In practice, expect roughly IT11 to IT13 on diameter with a surface finish in the region of Ra 1.6–6.3 µm, and note that drills generally cut slightly oversize. If the drawing calls for H7 or H8, or a specific bore finish, the hole has to be reamed, bored or helically interpolated as a separate operation. Position accuracy is a different question again, and depends on spotting, runout and workholding rather than the drill itself.
How deep can you drill in aluminum?
With a standard jobber-length carbide drill and a good peck cycle, up to about 5×D is routine. From 5×D to 10×D you want a through-coolant drill, verified runout under roughly 0.02 mm, and peck depths that reduce as the hole gets deeper. Beyond 10×D the process becomes specialized — a pilot hole, a dedicated deep-hole drill and higher coolant pressure — and past about 20×D gun drilling is normally the right answer rather than a conventional twist drill.
Why should you not use TiAlN or AlTiN coated drills in aluminum?
Those coatings are designed for steel and high-temperature alloys, where their aluminum-oxide layer resists heat. In aluminum workpieces, the same chemistry promotes adhesion: the workpiece material welds to the coating, built-up edge forms quickly, hole finish degrades and the drill fails early. For aluminum, use uncoated polished carbide, or DLC, ZrN or TiB2 coatings, which are specifically chosen for their low affinity to aluminum.
What is the difference between G73 and G83?
Both are peck drilling cycles, but they do different jobs. G73 is a high-speed peck cycle: the drill retracts by a small amount set as a machine parameter, just far enough to snap the chip, then continues. It is fast and suited to moderate depths. G83 is a full-retract peck cycle: the drill withdraws completely from the hole on every peck, which clears the chips and lets coolant back in, at the cost of cycle time. Use G73 for chip breaking up to about 5×D and G83 for genuine chip evacuation beyond that.
How do you drill aluminum without burrs?
You cannot eliminate burrs entirely in a ductile material, so the aim is to control them. Reduce the feed to around half over the last one to two millimeters of breakthrough, keep the drill sharp and replace it on a hole count rather than on appearance, support the exit face where the geometry allows, and program a back-chamfer instead of leaving deburring to hand work. Most importantly, state the required edge condition on the drawing so it is quoted, produced and inspected rather than assumed.
15Why Aluminum Hole Quality Decides Whether the Part Works
Holes are where most aluminum parts are actually assembled, sealed, located or cooled. A hole that is 0.05 mm oversize, 0.1 mm out of position or carrying an uncontrolled burr does not fail on the inspection report — it fails at assembly, on the test rig, or in the field. That is why hole strategy belongs in the quotation conversation, not in the machinist's hands on the day.
Assembly and fit
Dowel holes, bearing bores and press fits depend on diameter and roundness. Drilling alone will not hold H7, so if the print says H7 the route has to include reaming or boring — and that has to be priced in from the start.
Position and stack-up
Bolt patterns that mate with another component live or die on true position. Spotting, runout control and workholding decide this, and no downstream operation can pull a hole back onto position.
Sealing
Where a hole crosses an O-ring groove or a gasket face, a burr is a leak path. Edge condition needs to be a specified, inspected requirement rather than a subjective judgement.
Thread strength
Aluminum threads strip easily. Tapping drill size, thread engagement and hole finish determine whether a threaded hole survives the torque spec or fails on the first assembly.
Flow and cooling
In manifolds, cold plates and heat sinks, hole size, intersection quality and internal burrs directly affect flow rate and pressure drop. Deep-hole strategy is a performance issue here, not a cosmetic one.
Cost
Over-specifying hole tolerance adds reaming, gauging and scrap risk to every part. Under-specifying it causes rework and field failures. Getting it right at the drawing stage is the cheapest change you will ever make.
Need Aluminum Parts with Hole Quality You Can Actually Rely On?
Send a drawing or 3D model and our engineering team will review hole tolerances, depth ratios, thread requirements, edge conditions and inspection method before we quote — so the process route matches what the part actually needs. Goldcattle has manufactured custom precision components in Xiamen, China for 26 years as a national high-tech enterprise, with all production in-house and no outsourcing.
Achievable tolerances depend on part geometry, alloy, hole diameter, depth ratio and inspection requirements. Capability figures given in this guide apply to suitable features under controlled conditions and are confirmed per part at quotation.
