Drilling, Reaming, Tapping and Boring
Drill speeds and feeds, thrust and torque, pecking, reaming, tapping speeds, boring bars and hole accuracy.
Drilling: speed, feed and depth
A twist drill cuts with two lips and pushes with a chisel edge at the center (see the figure). Drills are fed per revolution, not per tooth, and run at the low end of the speed ranges because the heat is generated deep in a hole where little coolant reaches.
| Material | HSS drill speed |
|---|---|
| Aluminum | 60 to 90 m/min (195 to 295 SFM) |
| Brass | 45 to 70 m/min (150 to 230 SFM) |
| Plastics | 30 to 60 m/min (100 to 195 SFM) |
| Mild steel | 22 to 30 m/min (70 to 100 SFM) |
| Alloy steel (annealed) | 15 to 25 m/min (50 to 80 SFM) |
| Stainless steel | 10 to 18 m/min (35 to 60 SFM) |
| Cast iron | 20 to 30 m/min (65 to 100 SFM) |
| Titanium | 6 to 12 m/min (20 to 40 SFM) |
| Wood | 60 to 100 m/min (195 to 330 SFM) |
| Drill diameter | Feed (steel, HSS) | Feed (inch) | RPM at 25 m/min |
|---|---|---|---|
| 3 mm | 0.05 mm/rev | 0.002 in/rev | 2 653 rpm |
| 6 mm | 0.10 mm/rev | 0.004 in/rev | 1 326 rpm |
| 10 mm | 0.15 mm/rev | 0.006 in/rev | 796 rpm |
| 12 mm | 0.18 mm/rev | 0.007 in/rev | 663 rpm |
| 16 mm | 0.22 mm/rev | 0.009 in/rev | 497 rpm |
| 20 mm | 0.25 mm/rev | 0.010 in/rev | 398 rpm |
| 25 mm | 0.30 mm/rev | 0.012 in/rev | 318 rpm |
Feed per revolution is roughly 0.01 to 0.02 × the diameter for steel (larger for aluminum and plastics, smaller for stainless). Carbide drills run two to three times faster and need rigid, runout-free setups.
Worked example: a 12 mm hole in mild steel, 30 mm deep
- At 25 m/min the speed is n = 1 000 × 25 ÷ (π × 12) = 663 rpm. At 0.18 mm/rev the feed rate is 119 mm/min.
- The drill must travel 30 mm plus the point (about 0.3 × D = 3.6 mm): 33.6 ÷ 119 = 17 s without pecking.
- Torque on the drill: M = kc f D² ÷ 8 = 3 415 × 0.18 × 12² ÷ 8 ÷ 1 000 = 11.1 N·m, a power of 0.77 kW (check: removal rate 14 cm³/min × 3 415 ÷ 60 000 = 0.77 kW; see Cutting Force, Power and Torque).
- A drill press clamped work holds that torque; a part held by hand does not: it spins (see Workholding).
Starting a hole without it walking
- The chisel edge does not cut: it pushes a patch of material aside, which is why a drill wanders on a flat surface.
- Spot it first with a center drill or a spotting drill (a 90° or 120° point that is stiffer than the main drill) or a center punch.
- A split point (135°) removes most of the chisel edge and self-centers; use it for steels and stainless.
- Large holes: use a pilot hole of about the chisel-edge width of the large drill (a quarter of the diameter), which lowers the thrust by about a third and gives a rounder hole.
- Clamp, and back up the exit with scrap so that the drill does not grab as it breaks through.
Deep holes and pecking
| Depth | Method | Why |
|---|---|---|
| Up to 3 × D | No peck needed | Chips clear along the flutes |
| 3 to 5 × D | Peck about 1 × D | Withdraw to clear the chips |
| 5 to 10 × D | Peck 0.5 × D; coolant | Chips pack; flood or through-tool coolant |
| Over 10 × D | Gun drill or high-pressure coolant through the tool | Standard twist drills fail here |
Worked example: pecking a 60 mm hole with the 12 mm drill
- At 5 diameters deep, peck by 0.5 × D = 6 mm: 10 pecks. The cutting time at 119 mm/min is 30 s.
- Each peck retracts to the surface and rapids back: 660 mm of extra travel at 10 000 mm/min adds about 4 s: pecking is slower but the only way to clear the chips without a coolant-through drill.
- In G-code, G83 is the peck-drilling cycle (full retract), G73 the chip-breaking cycle (a small retract).
Reaming for size and finish
A reamer removes only a little material (0.1 to 0.3 mm on the diameter) with many teeth, and follows the drilled hole, so it improves size and finish but not position. The speed is about half the drilling speed and the feed about twice the drill feed, with the work well lubricated.
Worked example: a 10 mm H7 hole
- Drill 9.8 mm (leaving 0.10 mm per side); ream to 10 mm at 12 m/min = 382 rpm (47 % of the drill’s 812 rpm), a feed of 0.30 mm/rev (115 mm/min), with cutting oil.
- Do not reverse a reamer in the hole, and do not stop it in the cut: both mark the surface.
- A reamed hole holds H7 (+0.015 mm on 10 mm); the same hole as drilled is about ten times looser (see Fits in Practice).
Tapping
A tap cuts a thread in a drilled hole; the feed is exactly the pitch per revolution, so the feed rate is RPM × pitch. Tap drill sizes are in the Tap Drill Calculator; here are the speeds.
| Material | Tap speed (HSS, cutting tap) | Notes |
|---|---|---|
| Aluminum | 15 to 30 m/min | Cut tap, spiral flute; lubricant |
| Brass | 15 to 25 | Straight flute; light oil |
| Mild steel | 8 to 15 | Spiral point for through holes; cutting oil |
| Stainless steel | 3 to 8 | Spiral point, sharp, tapping paste; never stop |
| Cast iron | 8 to 15 | Dry or light oil |
| Titanium | 2 to 6 | Slow, sulfurized oil; short engagement |
Worked example: an M6 × 1 thread in aluminum, 12 mm deep
- Tap drill = D − P = 6 − 1 = 5.0 mm (77 % thread).
- At 20 m/min the speed is 1 061 rpm. The feed rate must be RPM × pitch = 1 061 × 1 = 1 061 mm/min (G84 does this in the control). The thread takes 0.7 s.
- In stainless steel the speed falls to 8 m/min (424 rpm) and the tap drill to the larger size (about 65 % thread) so that it takes less torque.
- Thread-forming taps displace the metal instead of cutting it (no chips, a stronger thread in soft metals) and need a larger drill: about 5.5 mm for M6.
- Use rigid tapping (a synchronized spindle) or a tension-compression holder; clear chips in blind holes with a bottoming tap or a spiral-flute tap; back out the tap often when tapping by hand.
Boring
A single-point boring bar enlarges and corrects a hole. It is a cantilever, so its stiffness is the limit: deflection grows with the cube of the overhang and falls with the fourth power of the bar diameter (see Cutting Force, Power and Torque). Speeds and feeds follow turning (see Turning, Threading and Surface Finish) at the lower end, with a small depth of cut and a feed of 0.05 to 0.15 mm/rev.
Worked example: a 20 mm bore with a 14 mm bar
- At 120 m/min the speed is 1 910 rpm; at 0.08 mm/rev the feed rate is 153 mm/min.
- A steel bar 14 mm in diameter sticking out 60 mm (L ÷ D = 4.3) with 50 N of radial force deflects 0.009 mm; a carbide bar deflects 0.003 mm (2.9 times less) because its modulus is three times higher.
- At six diameters of overhang the steel bar deflects 0.02 mm: keep L ÷ D under 4 for steel bars and use carbide or damped bars beyond that.
- Take a spring pass: repeat the last cut with no extra depth to remove the deflection error.
How accurate is each process?
| Process | Tolerance grade | Typical result | Notes |
|---|---|---|---|
| Twist drill | IT11 to IT13 | ±0.1 to ±0.25 mm on 10 mm | Oversize by 0.05 to 0.2 mm; rough, can wander |
| Drill then reamer | IT7 to IT8 | H7: +0.015 mm on 10 mm | Good size and finish; follows the drilled hole’s line |
| Single-point boring | IT6 to IT7 | ±0.01 mm | Corrects position and straightness; slower |
| Honing | IT5 to IT6 | a few micrometers | Finishing bores and cylinders |
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Drill wanders or starts off the mark | Chisel edge on a flat surface, drill not square | Spot or center-drill first; use a split point and a rigid setup |
| Hole is oversize or oval | Poorly ground point, bent drill, runout | Use a good drill and holder; check runout; drill a pilot |
| Drill burns or turns blue | Speed too high or no coolant | Lower the speed; flood or peck with oil |
| Drill breaks as it exits | Work not backed up, feed too high at the break-through | Back the work; slow the feed at the exit |
| Chips jam in a deep hole | No pecking, no coolant | Peck by 0.5 × D; use coolant-through or a gun drill |
| Tap breaks | Hole too small, chips, no lubricant, misalignment | Larger tap drill; spiral flute for blind holes; use a tap guide |
| Reamed hole is rough or tapered | Reamer run backwards or off-center, too little or too much stock | Leave 0.1 to 0.3 mm; use a floating reamer holder; clean flutes |
Related
- Speeds and Feeds: the overview of this guide.
- Speeds and Feeds by Material: the speeds by material.
- Turning, Threading and Surface Finish: boring uses the turning data.
- Tap Drill Calculator, Drilling, Tapping and Fasteners and Power Tools and Shop Machines (the drill press).
FAQ
What speed should I run a drill?
n = 1 000 × V ÷ (π D) with 25 m/min for steel, 60 to 90 for aluminum and 10 to 18 for stainless (HSS); a 12 mm drill in mild steel runs at about 660 rpm.
How fast should a tap run?
Slowly: 8 to 15 m/min in steel, 15 to 30 in aluminum; the feed in mm/min equals the RPM times the pitch.
Do I need to peck drill?
Yes for holes deeper than about three diameters: withdraw to clear the chips, or use coolant-through or a gun drill for very deep holes.
Why ream a hole?
A drilled hole is oversize and rough (IT11 to IT13); a reamer brings it to H7 size and a smooth finish, but does not correct its position.
References
- Oberg, E., et al., Machinery’s Handbook (drilling, reaming, tapping and boring data).
- Sandvik Coromant, Metal Cutting Technology (drilling and boring); ISO 235 (twist drills) and ISO 2162.
- Tool makers’ catalogs (Guhring, OSG, Dormer, Sandvik, Kennametal).
Last reviewed: October 2026. Speeds, feeds and thrust are typical starting values: use your drill maker’s data.