Hole Making

An indexable drill — also called an insert drill or U-drill — is a steel body with pockets that hold replaceable carbide inserts, usually two, positioned so their cutting arcs overlap across the radius of the hole. When an edge wears you index the insert to a fresh corner or drop in a new one. There is no regrinding and no re-setting of length, and the body carries on for years.

The crossover point is diameter. Below roughly 12–14 mm a solid carbide drill is almost always the better buy: the insert pockets physically will not fit, and a solid drill holds position and size better anyway. Above that the economics invert — you are replacing a small insert rather than a whole solid drill, and the bigger the hole the more dramatic that difference becomes. Our U-drill bodies run from Ø14 mm up to Ø50 mm.

Depth is rated in diameters. A 3xD body drills three times its own diameter deep, 5xD five times. Buy for the depth you actually need — a longer body flexes more and evacuates chips less easily.

Where indexable drills are the wrong answer:

• Rigidity. They cut hard and unevenly on entry. They need a proper machining centre, a solid fixture and decent spindle power — not a worn pillar drill.
• Entry surface. Unlike a twist drill they do not cut at dead centre, so they want a flat, square face to start on. Angled or curved entries need a spot face first.
• Tolerance. They will not give you a reamed-grade hole. If the drawing calls for H7, plan on reaming afterwards.

Two separate decisions: the insert style and size are fixed by the drill body, and the grade is chosen by the material you are cutting. Get the style right or it will not sit in the pocket; get the grade right or it will not last.

Which style your body takes:

Which grade for your material:

• SPMG in SMU10 (Vortex) — aluminium and non-ferrous materials.
• SPKX, WCKX and WCMX in PH6920 (Palbit) — stainless steel, general steels and heat-resistant alloys.
• QCMT in CMUM25 (Vortex) — general use, and it turns as well as drills.

Reading the code. The letters give the shape and clearance; the digits that follow give the size, thickness and corner radius. An SPMG 090408 will not fit a pocket cut for an SPMG 050204 even though both are SPMG. Match the whole code, which is stamped on the insert and listed against the drill.

Inserts, screws and keys are all stocked as separate lines, so a worn edge never means buying a new body. Browse indexable drills and inserts →

Four substrates, in ascending order of hardness, price and fussiness about setup.

• HSS — the general-purpose choice for mild steel, aluminium, brass and plastics. Cheapest per drill, forgiving of a less-than-rigid setup, and it can be resharpened. It gives up once the material hardens or the cut gets hot.
• HSS-E (cobalt, typically 5–8% Co) — retains its hardness at higher temperature. This is the step up for stainless, tougher alloys and anything abrasive. Where plain HSS glazes over and stops cutting, cobalt keeps going.
• Powder metal (PM) — made by a different route, giving a finer and more even carbide distribution than conventionally melted HSS. Tougher and more wear resistant again, for high-volume and difficult materials, without carbide's brittleness.
• Solid carbide — roughly three times stiffer than HSS, so it barely deflects. That is what buys you positional accuracy and a consistent hole size, and it runs at far higher speeds and feeds. The trade-off is brittleness: it wants a rigid machine, a square entry and a steady feed. Interrupted cuts, spindle runout and a hand-fed drill press chip the edge, and a chipped carbide drill is scrap rather than a regrind.

Coatings add life on top of the substrate. TiAlN forms a protective oxide layer at cutting temperature, so it suits fast and dry work; TiN is a good general-purpose coating; specialist coatings like EGIAS on the OSG flat bottom drills and Axicoat on micro drills are tuned to those specific jobs. Uncoated remains the economical option in softer materials.

The short version: HSS for the toolroom and one-offs, cobalt for stainless, PM for volume in nasty material, carbide the moment accuracy or cycle time is what matters.

Always start from the manufacturer's cutting data for the specific drill and material — the numbers vary far too much between substrates and coatings for a single table to be safe. What does not vary is the method.

Spindle speed comes from the recommended surface speed. With Vc in m/min and diameter D in mm, rpm = (Vc × 1000) ÷ (π × D). The consequence people forget: surface speed is fixed by the material, so a 20 mm drill must run at a quarter of the rpm of a 5 mm drill in the same steel.

Feed is quoted per revolution for drills, not per tooth. Feeding too lightly is the more common mistake — it rubs rather than cuts, work-hardens the material and kills the edge faster than feeding hard.

Pecking. Up to about 3xD you can usually drill straight through in one go. Beyond that chips stop clearing on their own and you need a peck cycle — deep pecks to break the chip on a normal drill, full retracts once you are past roughly 5xD or in anything stringy.

Through-coolant changes the calculation. Coolant delivered at the tip flushes chips back up the flutes and takes heat out of the cutting zone, which lets you run deeper without pecking at all and dramatically extends life in stainless and heat-resistant alloys. If your machine has it, buy drills that use it.

Entry and exit. Reduce feed as the drill breaks through, or the unsupported edge grabs and chips — particularly with carbide and with indexable drills. On anything other than a flat square face, spot drill first.

118° is the traditional general-purpose twist drill point. It works in mild steel and aluminium and it is what most jobber drills come as.

135° to 140° is flatter, which spreads the cutting load over a wider edge and reduces walking on entry. It is the better choice for harder materials and stainless, and it is standard on most carbide drills.

Split point grinds away most of the chisel edge at the centre, where a conventional drill does not really cut at all — it extrudes. That means it self-centres, needs noticeably less thrust and can start without a centre punch.

Flat bottom drills cut a flat-based hole rather than a conical one. Use them for blind holes that must seat a flat component, for spot facing, and for starting on angled, curved or interrupted surfaces where a pointed drill would skate.

Spot drills put an accurate conical start in the surface so the drill cannot wander. Match or exceed the drill's point angle: a 90° spot drill under a 118° or 140° drill contacts at the periphery first, which is what you want. A spot that is narrower than the drill point contacts at the centre and can chip a carbide edge. We stock 90° and 120° cobalt HSS-E spot drills, uncoated and TiAlN coated.

Do you always need to spot? On a rigid machining centre with a self-centring carbide drill and a flat face, often not. On a manual machine, an angled or curved face, a long drill, or anywhere position matters — yes.

Stainless steel. The enemy is work hardening. Dwell or rub and the surface hardens under the edge, after which nothing will cut it. Use a firm continuous feed, never let the drill spin without advancing, and pick a 135–140° point. Cobalt HSS-E is the sensible minimum; carbide with through-coolant is the production answer. Keep it flooded.

Hardened steel. Above roughly 45 HRC only carbide is realistic, and it needs a rigid setup and a square entry. Reduce feed on breakthrough. Below that, PM and cobalt drills will cope with a slower surface speed.

Aluminium, brass and copper. Soft and gummy — the problem is chips welding to the flutes, not tool wear. Use polished or coated flutes, higher surface speeds, a generous feed to keep the chip moving, and clear chips often. Brass is the exception among the soft metals: it grabs, so a drill with less aggressive rake is easier to control.

Composites and carbon fibre. Abrasive rather than hard — they wear the edge away rather than blunting it. Carbide is essential; the failure mode is delamination and splintering at breakthrough, so back the workpiece with a sacrificial board and ease off the feed as you exit.

Plastics. Heat is the problem. Too much speed melts the material and it re-welds behind the drill. Slower speeds, sharp tools and frequent chip clearance. For small work, micro drills in uncoated grades are the economical choice.

Cast iron. Dry, dusty and abrasive. Usually run without coolant, and expect faster wear on everything.

Drilling and sizing are two different operations. A drill makes a hole roughly where you want it, at roughly the diameter you asked for. A twist drill typically cuts oversize, and the hole it leaves is not perfectly round or straight, with a torn rather than a burnished bore surface. For a clearance hole none of that matters. For a dowel, a bearing seat, a location pin or anything the drawing gives a tolerance to, it matters a great deal.

A reamer takes a small amount of material out of a pre-drilled hole and leaves it round, straight, on size and with a good surface finish. Our range covers H6, H7 and H11 tolerances — H7 being by far the most commonly specified on engineering drawings.

Practical points:

• Drill undersize by the reaming allowance — too much stock and the reamer cuts rather than sizes, too little and it burnishes without cleaning up the bore.
• Reamers follow the existing hole. They correct size and finish, not position. If the hole is in the wrong place or off-axis, a reamer will not save it — spot drill and bore instead.
• Straight shank reamers suit machining centres and mills, mounting straight into collet or drill chucks. Taper shank reamers go into Morse taper spindles and tailstocks, which is why they are the lathe choice.
• Carbide reamers considerably outlast HSS in cast iron, hardened steel and abrasive material. HSS stays the practical option for general workshop use in mild steel, aluminium and brass — cheaper, and straightforward to resharpen.
• A floating reamer holder lets the reamer follow the drilled hole rather than fighting any misalignment in the spindle.

See the full reamer range →