CNC Machining and Drilling: Where the Hole Goes Wrong
Drilling is the cheapest operation in CNC machining and drilling, and it is also the one that ruins the most parts. This page explains how the drill actually cuts, how deep and how fast it can go, and which hole features should be milled or bored instead. Written for engineers and buyers who read a drawing before they read a quote.
How CNC Machining and Drilling Cuts a Hole
A twist drill does not shear metal the way an end mill does. Its two cutting lips scrape the bottom of the hole at a fixed feed per revolution, while the margin and the chisel edge rub against the wall. That rubbing is friction, and friction is heat. Most drill failures start there, not at the cutting edge.
The chisel edge at the center has a high negative rake. It does not cut cleanly; it pushes and extrudes material until the lips take over. On a 10 mm drill, the chisel edge can account for more than half the total thrust force. If a machine lacks thrust stiffness, the drill walks before it bites.
Cutting speed at the periphery is where the heat is generated. A Ø10 mm drill at 1,500 rpm runs at about 47 m/min at the outer corner and close to zero at the center. The same spindle speed that burns the corner leaves the center smearing. That is why feed per revolution, not rpm alone, controls chip formation.
Chip evacuation decides whether the hole stays round. Chips that pack in the flute grind against the wall and push the drill off axis. Through-spindle coolant or a peck cycle solves most of it. Without either, a hole deeper than three diameters starts to drift.
- 1Point angle118° for general steel, 140° for flat-bottom starts in plastics and thin plate
- 2Helix angle28–30° general purpose; 40° for aluminium and deep holes
- 3Web thinningSplit point lowers thrust and stops walking on hard stainless
Speed and Feed Ranges That Hold Up
Surface speed is the number to set first. Uncoated HSS in mild steel runs 20–30 m/min. Cobalt HSS in 304 stainless drops to 8–12 m/min. Carbide with TiAlN coating in 6061 aluminium runs 100–200 m/min, and in P20 tool steel 60–90 m/min. Pick the speed, then read the feed from the drill diameter.
Feed per revolution scales with diameter. A Ø3 mm drill in steel takes 0.05–0.08 mm/rev. A Ø10 mm drill takes 0.15–0.25 mm/rev. A Ø25 mm drill takes 0.25–0.40 mm/rev. Feeding too light is the common mistake: the edge rubs, work hardens the surface, and the next pass breaks the drill.
Rigid tapping and drilling share the same spindle, so the setup decides both. A Ø6 mm carbide drill in 6061 at 6,000 rpm and 0.15 mm/rev removes material fast, but only if the tool holder runs under 0.01 mm TIR. Runout doubles the load on one lip and halves tool life.
Coolant choice follows the material. Aluminium wants high-pressure flood or mist. Stainless and titanium want through-coolant at 50–70 bar. Cast iron is often drilled dry, because coolant turns the graphite dust into a sludge that clogs the flutes.
- 1Peck depthFirst peck one diameter, then 0.5 diameter per peck in steel
- 2DwellAdd 0.1–0.2 s at the bottom on blind holes to clear chips
- 3ReamingLeaves 0.1–0.2 mm on diameter for H7 fits
Depth-to-Diameter: The Rule That Bites
Standard twist drills hold position and finish to about 3× diameter. From 3× to 5× you need a split point and a peck cycle. Beyond 5×, chip evacuation and drill drift become the limit, and a pilot hole or a gun drill earns its cost.
A 6× diameter hole is not simply a deeper version of a 3× hole. The flute volume is fixed, so chips must travel further against more wall contact. Coolant pressure at the tip falls off. Runout at the tip multiplies along the length. A Ø5 mm hole 50 mm deep is a different job from a Ø5 mm hole 15 mm deep, even on the same machine.
Drift is measurable. A Ø8 mm drill 80 mm long can wander 0.2–0.5 mm off center without a pilot. If the drawing calls for ±0.05 mm true position, drill undersize and bore to size, or mill the hole with a helical path.
Pilot holes should match the web thickness, not the drill diameter. For a Ø10 mm drill, a Ø3–4 mm pilot is right. A pilot as large as the finished hole removes the guidance the drill needs and lets it chatter.
- 13× DStandard drill, no peck needed on most aluminium
- 25× DSplit point plus peck; check coolant reach
- 310× DPilot or gun drilling; expect a second op
When to Drill, Ream, Bore, or Mill
Drilling is fast and cheap for holes that carry a bolt or a pin in a clearance fit. A drilled hole in aluminium typically lands within ±0.1 mm on diameter and ±0.15 mm on position. That is fine for M6 clearance. It is not fine for a bearing bore.
Reaming takes a drilled hole to an H7 fit. Leave 0.1–0.2 mm on diameter, keep the reamer coaxial with the drill, and use the same setup. Reaming in a second setup never holds concentricity. Reamers follow the existing hole, so they cannot fix position error.
Boring is the answer when the hole must be round, straight, and sized to ±0.01 mm. It needs a rigid bar and a separate pass, so it costs more. For a hydraulic cylinder bore or a spindle seat, that cost is not optional.
Milling a hole with a helical path gives position control the drill cannot match. On a 5-axis machine, an interpolated Ø12 mm hole in a curved surface can hold true position inside 0.03 mm. Slower than drilling, but it skips a second operation.
- 1ClearanceDrill only; ±0.1 mm on diameter is enough
- 2Interference fitReam or bore; drilling alone will not hold it
- 3Cross holesDrill after the main bore, or burrs trap the mating part
Reading the Chip and the Sound
Chips tell you what the cut is doing. Steel should produce short, curled, silver-to-straw chips. Blue or black chips mean the surface speed is too high. Fine powder means the feed is too light and the edge is rubbing. Long stringy chips in aluminium mean the feed is too low for the speed.
Sound changes before the drill breaks. A clean cut is steady. A squeal means the margin is rubbing. A rhythmic thump means the drill is chattering, usually from runout or a long overhang. Stop and check before the next hole.
Breakage is rarely sudden. On a Ø4 mm carbide drill, the corner wears first, then the thrust climbs, then the web cracks. Tool life monitoring by hole count is cheap insurance. Track holes per drill and change on schedule, not on failure.
Entry and exit are the two moments that scrap parts. On a curved or angled surface, drill into a flat spot or use a spot drill first. On a through hole, reduce feed to 30–50% for the last 0.5 mm so the lips do not grab and lift the part.
- 1Spot drill90° or 120°, depth to the shoulder only, never deeper
- 2Burr controlAdd a chamfer op; hand deburring hides size errors
- 3BreakoutSupport the exit side or back the part with a sacrificial plate
Drilling vs Reaming vs Boring vs Helical Milling
Pick the operation from the tolerance and the quantity, not from habit.
| Operation | Typical diameter tolerance | Position tolerance | Best for |
|---|---|---|---|
| Twist drilling | ±0.05–0.10 mm | ±0.15 mm | Clearance and tapped holes |
| Peck drilling | ±0.05 mm | ±0.10 mm | Deep holes, 3× D and beyond |
| Reaming | ±0.01 mm (H7) | Follows the drilled hole | Pin and dowel fits |
| Boring | ±0.005 mm | ±0.01 mm from a set datum | Bearing and cylinder bores |
| Helical milling | ±0.02 mm | ±0.03 mm | Curved surfaces, no second op |
The Trade-Off in One Line
If the hole is a clearance fit, drill it and move on. If it carries a bearing, a pin, or a seal, drill undersize and bore or ream it in the same setup. The extra pass costs minutes; a scrapped bore costs the whole part.
Common Questions on Holes
What depth-to-diameter ratio can you drill without a special setup?
Up to 5× diameter with a split-point drill, a peck cycle, and coolant that reaches the tip. Beyond that we pilot or gun drill.
The limit is chips, not the tool. Once the flute packs, the drill rubs and drifts.
Why does my drilled hole come out oversize?
Usually runout, a worn margin, or too light a feed. Check tool holder TIR first; anything over 0.02 mm will cut oversize on one side.
A drill with unequal lip length also cuts oversize. Regrind or replace it.
Can you hold ±0.005 mm on a drilled hole?
No. Drilling is a roughing operation for holes. We hold ±0.005 mm by boring or by helical milling on a 5-axis machine.
Drilled holes normally land within ±0.05–0.10 mm on diameter.
Does drilling need coolant on aluminium?
Yes, for chip evacuation and to stop built-up edge. High-pressure flood or mist both work.
Cast iron is often drilled dry, because coolant makes the graphite dust clog the flutes.
How do you stop the drill from walking on an angled surface?
Spot drill a flat seat first, or mill a small flat with an end mill. On a curved casting, a Ø6 mm flat is enough to start a Ø5 mm drill straight.
Reduce the feed on entry to about half for the first 1 mm.
Do you inspect every hole?
We run 100% inspection before shipment, with raw material checks, in-process monitoring, and final inspection. Reports are available on request.
For critical bores we record the actual size and roundness, not just pass or fail.
Send the Drawing, Get a Real Answer
We review hole callouts, tolerances, and depth-to-diameter limits before quoting, so the price you get matches the part you need.
12-hour quote and DFM100% inspectionNo minimum order quantity
More Machining Notes
We publish setup notes, tooling trials and inspection data from the factory floor.
