Drilling Stainless Steel: Feeds, Speeds and Drill Selection

Stainless steel drills like nothing else in the shop. It work-hardens under the edge, the chip stays long and stringy instead of breaking, and the heat does not flow into the chip the way it does on mild steel. A drill that runs fine on 1018 will glaze over, rub, and weld its flutes shut inside two holes in 304. The difference between a clean hole and a burned, oval one comes down to drill geometry, surface speed, feed pressure, and coolant pressure. This guide gives the starting parameters shops actually use, and the mistakes that turn a simple hole into a tool-eating operation.

Pick the drill grade before you touch the material

A standard HSS jobber drill survives on low-carbon steel but is the wrong tool for stainless. For 304, 316 and 17-4, use a cobalt HSS-E or a solid-carbide drill with a TiAlN or TiCN coating. Cobalt drills tolerate higher heat and resist work-hardening better than plain HSS; solid carbide runs faster and holds size longer, but it is brittle and needs a rigid setup. Point angle matters: a 135-degree split-point drill centers without a pilot spot and reduces the work-hardening zone, while a 118-degree general-purpose drill tends to walk and rub on the cut. For holes deeper than three times diameter, choose an internally-cooled carbide drill through coolant, because the flutes cannot evacuate long stainless chips without help. The broader material choice between 303, 304 and 316 changes drilling difficulty more than most buyers realize, as the stainless grade tolerance and cost comparison spells out.

Surface speed and feed, as starting numbers

Do not set the spindle by RPM alone. Start from surface speed. For 304 and 316 with a coated carbide drill, run roughly 80 to 120 m/min surface speed; with cobalt HSS, drop to 20 to 30 m/min. A 6 mm carbide drill at 100 m/min lands near 5,300 RPM; the same drill in 316 on a rigid machine might drop to 3,500 RPM to hold edge life. Feed per tooth is where most operators fail. Stainless needs a feed that bites through the work-hardened layer from the previous pass, otherwise the drill rubs and hardens the surface further. Plan on 0.08 to 0.15 mm per revolution for a 6 to 10 mm carbide drill, and 0.05 to 0.10 mm/rev for cobalt. Too light a feed is worse than too heavy: rubbing hardens the hole wall, and the next pass drills into a crust of hardened material. For very deep holes past 10 times diameter, the gun drilling service guide covers the dedicated deep-hole route.

Coolant, chip evacuation and peck cycles

Stainless throws heat into the workpiece and tool, not into the chip, so coolant is doing real work. Flood coolant through the spindle at 6 to 10 bar clears chips and cools the edge; through-tool coolant at 20 bar or more makes deep holes possible. If your machine only has flood coolant, use a peck cycle: retract the drill every 1.5 to 2 times diameter to break the chip and clear flutes, and flood generously on the retract. Without pecking, the long austenitic chip winds around the drill and rips the edge out on retract. Emulsion at 8 to 10 percent concentration works; straight oils run slower speeds but give better finish on stainless. Watch the chip color: a clean, short, violet-brown chip means the parameters are right, while a bright blue or smoked chip means heat is building and the drill is about to fail. Edge wear shows up fast, which is why the CNC tool wear monitoring guide matters on stainless jobs.

Common mistakes that ruin holes

The first mistake is drilling a spot mark with the wrong tool, then drilling into it. A spot drill that dwells hardens the surface, so keep spotting light or skip it with a 135-degree split point. The second is pecking too often and too deep, which lets the edge rub between pecks and work-harden the wall. The third is a loose setup: stainless drilling pushes high axial force, and a drill held in a sloppy collet or a part held in a soft jaw that flexes will walk and produce an out-of-round hole. The fourth is letting the drill get dull and pushing faster to compensate. A worn drill on stainless burns, welds chips to the flutes, and suddenly snaps; when the edge looks glazed, change it before the hole spoils. Use the right insert and drill grade for the job, as the CNC coolant types guide explains.

Getting consistent holes batch after batch

Once the first hole is clean, lock the parameters and write them down. Measure hole diameter at the top and the bottom on the first three parts, because stainless can pull a tapered hole if feed drops on breakthrough. Hold drill runout under 0.02 mm in the holder, and replace collets on a schedule rather than waiting for a wobble. For tapped holes, drill the tap drill size right the first time; a sloppy drilled hole makes a weak thread. A production stainless drill should last 150 to 300 holes on 304 before the edge needs regrind or replacement. Track that number on the job, and when it drops to half, change the drill rather than chase a bad hole. The hole is cheap, the scrapped part and the missed cycle are not.

⚙

Ready to Start Your CNC Project?

Get a free quote within 24 hours. ISO 9001 certified, 20+ years experience, low-volume friendly from 1 piece.

Get a Quote