CNC Drilling and Solutions: How Holes and Threads Get Made
This page explains what actually happens when a CNC machine cuts a hole and then cuts a thread into it. We cover tool geometry, chip evacuation, thread pitch, tolerance stack-up, and the point where drilling stops being the right process. Written for design engineers and buyers who need to judge a part before it goes to a shop.
What CNC drilling and solutions actually do
A drill removes material with a rotating cutting edge at the tip. The margins behind the edge rub against the hole wall and keep the tool centered. Hole quality depends on the drill as much as on the spindle, because a drill with worn margins will cut oversize even on a rigid machine.
Tapping is a different motion. The tap is fed at a fixed ratio to spindle speed, so one rotation equals one thread pitch of axial travel. On a synchronized tapping cycle the feed and the spindle are electronically locked. Without that lock, the tap pulls itself into the cut and the thread pitch drifts.
Both processes share one enemy: heat that stays in the cut. A drill buried in aluminum at 3,000 rpm generates chips that carry most of the heat away. Recutting those chips doubles the thermal load on the edge. Through-spindle coolant or a peck cycle solves most of it.
Hole size, drill point, and tolerance stack-up
A standard 118° drill point leaves a cone at the bottom of a blind hole. The cone depth is roughly 0.3 × diameter, so a Ø10 mm hole needs about 3 mm of extra depth to stay clear of the cone. Ignore this and a bottoming tap will hit the cone before the thread is full.
Drilled holes rarely come out exactly on size. Cutting forces push the drill off axis, and the hole tends to measure slightly oversize at the entry and slightly undersize near the exit. For a hole that must hold ±0.005 mm, drill undersize and then ream or bore to the final dimension.
Thread strength depends on engagement, not on the hole. A 6H class thread in aluminum needs roughly 1.5 × diameter of full thread. In 316 stainless, going below one full diameter of engagement risks stripping under load, so increase the wall thickness or move to a coarser pitch instead of a longer screw.
When drilling is the right call and when it is not
Drilling wins on speed. A twist drill removes material faster per dollar than any other hole-making process, and it handles depth-to-diameter ratios up to about 5:1 without special tooling. For clearance holes, bolt holes, and pilot holes, it is almost always the first operation.
Deep holes change the math. Past a 10:1 depth-to-diameter ratio, chip evacuation fails and the drill wanders. Gun drilling holds straightness and finish on deep bores, while conventional drilling with a peck cycle remains cheaper up to roughly 8:1.
Boring is the answer for tight tolerance. A single-point boring head corrects position, roundness, and size in one pass, and it can hold ±0.005 mm comfortably. It is slower and needs a pre-drilled hole, so use it only where the drawing demands it.
Thread milling suits large or awkward threads. A thread mill cuts a helix with a single tool that handles any diameter within its range, and it produces a thread in materials where a tap would snap. Taps are still faster for small threads in production.
Material effects on hole quality and tool life
Aluminum 6061 and 7075 cut fast and tolerate high spindle speeds. The soft grades build a built-up edge on the drill lip, which makes the hole oversize and rough. Higher rake angles and polished flutes reduce that tendency, and a small chamfer at the entry keeps the edge clean.
Stainless 304 and 316L work-harden under the cutting edge. A dull drill rubs instead of cutting, and the surface below goes harder with every pass. Keep the feed per revolution high enough to stay under the hardened layer, and never let the tool dwell.
Titanium Ti-6Al-4V and Inconel 718 concentrate heat at the edge because they conduct it poorly. Cutting speeds drop sharply, coolant has to reach the tip, and tool changes come more often. These are the jobs where a thread mill beats a tap, because a broken tap in Inconel is expensive to remove.
Plastics behave in the opposite direction. POM and PEEK grab the drill and generate long stringy chips that wrap the tool. Sharp, polished flutes with a high helix, plus a fast retract, keep the hole clean.
Choosing between drilling, reaming, boring, and thread milling
Ratings assume a rigid machine and a stable setup.
| Process | Typical tolerance | Best depth ratio | Pick it when |
|---|---|---|---|
| Twist drilling | ±0.05 mm | Up to 5:1 | Clearance, bolt, and pilot holes |
| Peck drilling | ±0.05 mm | 5:1 to 8:1 | Chips jam or the drill wanders |
| Gun drilling | ±0.02 mm | 10:1 and deeper | Deep oil or coolant passages |
| Reaming | ±0.01 mm | Up to 8:1 | Hole needs a fine finish and size |
| Boring | ±0.005 mm | Any, after pre-drill | Position and roundness are critical |
| Tapping | 6H class | 1.5 × Ø engagement | Small threads in production |
| Thread milling | 6H class | Any diameter | Large threads or tough alloys |
The short verdict
For clearance and pilot holes, drill and move on. For a hole that must hold ±0.005 mm, pre-drill then bore. For small threads in production, tap; for large threads or tough alloys, thread mill.
Questions engineers ask
How deep can a twist drill go before I need a different process?
A standard twist drill handles roughly 5:1 depth-to-diameter with good chip evacuation. Between 5:1 and 8:1 it works with a peck cycle and through-coolant. Past 10:1, chip packing and drill wander make the result unpredictable, and gun drilling becomes the practical choice.
Why does my tapped hole strip even though the thread gauges pass?
Gauge size and thread strength are different checks. A 6H gauge confirms the thread form, not the engagement depth. If the full-thread length is under one diameter in stainless or under 1.5 diameters in aluminum, the thread can strip under load even though it gauges correctly.
Should I call out reaming or boring on the drawing?
Reaming is faster and gives a fine finish with a fixed size, so it suits production holes that need H7 fit. Boring corrects position and roundness as well as size, so it suits one-off parts and holes where the location matters more than the cycle time.
What causes a drilled hole to come out oversize?
Worn margins, an unbalanced drill, or a built-up edge on the lip. In aluminum the built-up edge is the usual cause. In steel, check runout first: a drill with 0.05 mm of runout will cut a hole well outside its nominal size at the entry.
How do you keep a tap from breaking in titanium or Inconel?
Reduce spindle speed, keep the feed synchronized, and use a thread mill where the geometry allows. A thread mill cuts with a smaller radial engagement and clears chips better, so the risk of a seized or snapped tool drops sharply in these alloys.
Send us the drawing and we will flag the hole features
We review hole size, depth ratio, thread engagement, and material before quoting, so the process is settled before the first chip.
12-hour quote and DFM100% inspection before shipmentNo minimum order quantity
More process notes from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
