Tapping Aluminum: Drill Sizes, Form Taps, Lube and Galling

Quick answer: In aluminum, use the standard chart drill for about 75% thread. For a 1/4-20 that’s a #7 (0.201 in) at 75.4%, and for an M6 it’s 5.0 mm at 77.0%. Always lubricate, since aluminum loves to weld itself to the tap. In ductile alloys like 6061, a thread forming tap is often the better tool, but it needs a larger drill (#1 for 1/4-20). For threads that will be assembled again and again, use a steel wire thread insert.

Wrought vs. cast aluminum

“Aluminum” covers a lot of alloys, and they tap very differently.

Wrought alloys such as 6061 (plate, bar, extrusions) are ductile and make long, stringy chips. The main risks are chips wrapping around the tap and metal smearing onto the cutting edges.

Cast alloys contain more silicon. Sandvik’s Jim Nielsen explains the trade-off: higher silicon makes the chips shorter but the material more abrasive, while lower silicon makes it gummier. YG-1’s Mark Ford describes cast aluminum’s chips as short, “almost as if you are machining cast iron.”

What that means for you:

• Wrought (6061 and similar): focus on chip evacuation and lubrication. Form taps work very well.
• Cast: focus on tool wear. Chips are less of a problem, but tap edges dull faster. OSG recommends nitrided taps for cast aluminum, and Tapmatic does the same for straight flute taps in cast aluminum.
• High-silicon cast: be careful with form taps (see below).

In shop experience, hard tempers like 6061-T6 tend to tap more cleanly than soft annealed stock or pure aluminum, which is more likely to smear. If threads come out torn in soft material, sharper tools and better lubricant usually help more than anything else.

Drill size: stick with 75%

For harder metals, many machinists drill oversize to cut torque. In aluminum, torque is rarely the problem, and the metal is soft, so you want the thread engagement.

Tapmatic’s guide recommends 65–75% thread for average work in free-cutting materials including aluminum, 60–70% for deep holes, and 75–85% for thin sheet and stampings. So the standard chart drill is the right default, and thin material can justify going a little tighter.

Chart drills for common sizes in aluminum:

When to go a size larger

Tapmatic also notes that soft materials can extrude into the thread root under tapping pressure, and that materials prone to galling may need a slightly larger hole. If a tap is binding, or the thread gauges tight, step up one drill size. On a 1/4-20, the #6 (0.204 in) gives 70.8%, still well within the range above.

For more on how drill size changes strength, see percent of thread.

Form taps and aluminum

Aluminum is one of the best materials for thread forming taps. OSG’s material table lists form tapping as the best method for both aluminum and aluminum alloys. Emuge lists wrought and cast aluminum among materials that cold form well.

Why form taps help here:

• No chips to wrap around the tap or pack a blind hole.
• Stronger threads, since the metal is cold worked. Emuge and OSG both say formed threads are generally stronger than cut ones.
• Less galling of the cut flank, because there’s no cutting edge for aluminum to build up on.

The catch is drill size. A form tap needs a bigger hole:

Those come from our form tap drill chart, which targets 65% thread. Check them against your tap maker’s chart.

Watch the silicon. Sandvik says form taps are a good choice in aluminum with less than about 10–12% silicon. Above that, castings get brittle and can fracture. If you don’t know the alloy of a casting, a cutting tap is the safer choice.

For the full comparison, see cut vs. form tapping.

Lubricant and galling

Galling is aluminum welding onto the tap. It shows up as torn, rough threads, rising torque, and sometimes a tap that seizes. OSG notes aluminum is soft and highly malleable, with poor surface finish likely, and recommends taps with sharper rake angles.

How to prevent it:

• Always lubricate. Norseman recommends kerosene or mineral spirits mixed with 15–25% petroleum cutting oil for aluminum. Purpose-made aluminum tapping fluids are a good option.
• Pick coolant carefully on machines. Sandvik’s Nielsen has seen full synthetic coolants cause welding within two or three holes, and advises coolants with additives chosen for aluminum.
• Form taps need even more lubricity. OSG lists chlorinated or oil-based non-water-soluble oils, as well as water-soluble oils, for form tapping aluminum.
• Use a sharp, smooth tap. Walter’s Luke Pollock recommends a sharp, polished tool to avoid bird-nesting. OSG recommends CrN coating for aluminum and DLC for dry aluminum work; both are designed to resist welding.
• Clear chips. On a hand tap, back off regularly. In blind holes use a spiral flute tap. Tapmatic recommends 40–50° high-helix spiral flute taps for long-chipping aluminum in blind holes, and spiral point taps for through holes.

Speed

Aluminum taps much faster than steel. Published starting points vary:

• Norseman (HSS): wrought alloys 80 SFM, die-cast 70 SFM, cast 60 SFM.
• OSG (HSS, general): rolled aluminum 10–20 m/min (about 33–66 SFM) for hand and spiral flute taps, 15–25 m/min (about 49–82 SFM) for spiral point taps; aluminum castings somewhat lower.

By hand, speed isn’t a concern. Focus on lubricant and chip clearing.

Thread inserts for soft metal

Aluminum is much softer than a steel screw, so the internal thread is usually the weak link. It also wears with repeated assembly. A stainless steel wire thread insert, such as a Heli-Coil, fixes both problems.

According to Stanley Engineered Fastening, Heli-Coil inserts protect and strengthen tapped threads in any material. They come in lengths of 1, 1-1/2, 2, 2-1/2, and 3 times the screw diameter, so a designer can balance the bolt’s strength against the parent metal’s shear strength, letting the bolt fail before the aluminum strips. Walter’s Pollock adds that an insert is also a common way to salvage an aluminum part with a stripped thread.

Use an insert when:

• The screw will come out often (access panels, fixtures, jigs).
• The joint needs more strength than the aluminum thread alone can provide.
• You’re repairing a stripped hole.

Inserts need their own tooling. The hole is drilled oversize and cut with an STI (screw thread insert) tap, available in coarse (STI-UNC) and fine (STI-UNF). Don’t use the standard tap drill sizes from our charts for an insert; use the drill size the insert maker specifies.

Quick checklist

1. Identify the alloy: wrought (6061) or cast.
2. Use the standard 75% drill for cut taps; go one size up if threads bind.
3. Consider a form tap in wrought or low-silicon cast alloy, with the larger form drill.
4. Lubricate every hole.
5. Use spiral flute taps for blind holes and spiral point taps for through holes. Plan blind-hole depth with our blind hole guide.
6. Use inserts for high-wear or high-load threads.

Need a clearance hole for the mating part? See the clearance hole chart.

Sources: OSG Tap Technical Guide Vol. 1 (Tables 13, 19, 21, 26, 28); Tapmatic, “Tapping Torque vs. Thread Strength,” “Drill Size Factors,” and “Tap Recommendations for Specific Materials”; Norseman Drill & Tool, “Feeds & Speeds for Taps”; Emuge-Franken, “Cold-Forming Taps”; Jim Lorincz, “Gummy, Stringy Material Meets its Match,” SME Manufacturing Engineering, 2022; Stanley Engineered Fastening, “Heli-Coil Design Guidelines.”