CNC drilling and eavesdropping: how holes and threads are actually made
This page explains the mechanics behind CNC drilling and eavesdropping, the numbers that decide whether a thread holds, and when the operation belongs on a 3-axis mill, a 5-axis center or a mill-turn. It is written for design engineers and buyers who review prints and process plans.
What happens at the tool tip during holemaking
A drill is a two-edge cutter with a chisel point at the center. The outer corner runs at the surface speed you programmed; the chisel edge runs at near zero. That one fact drives most drilling problems. Feed per revolution, not feed per minute, sets the chip thickness each edge has to carry.
For aluminium 6061 a common starting point is 0.10–0.25 mm/rev with HSS or carbide, 3,000–8,000 rpm depending on diameter. In 304 stainless the same drill wants 0.05–0.12 mm/rev and roughly one third the speed. Heat goes into the chip. When the chip comes out thin and powdery, the edge is rubbing and the drill will work-harden the hole.
The chisel edge does not cut well. It pushes material instead of shearing it, so it needs a pilot or a spot. A Ø10 mm twist drill with a 118° point leaves about 1.5 mm of dead zone at the center. That is where wander starts on an unsupported surface.
Peck depth matters more than peck count. On deep holes, retract every 1×D to 2×D so chips clear the flutes. Beyond 3×D without a peck, packed chips rub the wall and the hole grows oversize at the entrance.
How a tap removes material in a drilled hole
A tap is not a drill. It cuts on the chamfer, then the full thread form follows in the same helical path. The drilled hole must be the right size before the tap touches it. Too small and the tap stalls or breaks; too large and the thread crests come out flat and the fastener strips early.
The rule for cut taps is simple: hole Ø equals nominal thread Ø minus pitch. For M6 × 1.0 that is 5.0 mm. For M8 × 1.25 it is 6.75 mm. Form taps move metal instead of cutting it, so they need a larger hole, roughly nominal minus half the pitch. M6 × 1.0 form tap wants about 5.5 mm.
Thread depth has a limit. A blind hole should leave at least three full threads of engagement and a bottom clearance of about one pitch for chip room. Anything shorter and the bolt bottoms out before it loads. Anything deeper than 3×D on a small tap raises breakage risk sharply.
Cutting speed drops fast as taps get small. M3 in mild steel runs around 300–500 rpm with rigid tapping; M12 can run 600–900 rpm. On a floating holder the tap can pull off axis and the thread comes out skewed. Rigid tapping on a synchronized spindle avoids that.
Spot drilling, pilot holes and the order of operations
A spot drill does two jobs: it puts a small cone where the drill will start, and it sets the position. On a flat milled face with a rigid setup you can often skip it. On a cast surface, a curved wall or a cross-hole, skip it and the drill walks.
Spot depth should be just past the drill's point angle. If the spot is 90° and the drill is 118°, the drill corner touches first and you get chatter. Match the spot angle to the drill, or go slightly larger, and keep the spot diameter at roughly 1× to 1.5× the drill diameter.
Operation order on a typical plate: face, spot, drill, chamfer, tap, then deburr. Tapping last means chips from earlier cuts cannot fall into a finished thread. If the print allows, chamfer the hole before tapping so the first thread does not raise a burr that jams the gauge.
On parts with many holes, group tools by diameter. Each tool change costs time and adds a chance for position error. On our 5-axis centers with a Ø400 mm rotary table, holes on four faces can run in one setup, which holds true position far better than refixturing.
When drilling and tapping is the wrong process
Holes deeper than 10×D are a different problem class. Chip evacuation, drill deflection and coolant pressure all fight you. Gun drilling or a dedicated deep-hole cycle is the honest answer. Forcing a standard twist drill to 15×D usually ends in a broken tool inside the part.
Thin walls are the second limit. A hole 1 mm from a 1.5 mm wall will bulge as the drill passes through. Backing material or a support sleeve helps, but the print should allow the wall to grow or the hole to be reamed after.
Hardened steel above 45 HRC, Inconel and some titanium grades push tool life down hard. They can be drilled, but speeds drop to a fraction of mild steel and the process needs carbide, high-pressure coolant and a rigid setup. On a loose fixture the tool breaks before the hole is done.
Threads in soft plastics behave differently again. A cut tap in POM or ABS can tear the crest. Form taps or thread milling give a cleaner result. Thread milling also lets you cut a thread larger than the tool, which helps when the part is expensive and a broken tap would scrap it.
None of this makes drilling and tapping a bad choice. It is fast, cheap and repeatable when the hole is shorter than 5×D, the material is under 40 HRC and the wall is thick enough to support the cut.
Which process fits the hole
Pick by depth-to-diameter ratio, material and thread size.
| Condition | Drill + tap | Alternative |
|---|---|---|
| Depth under 5×D, steel or aluminium | Standard cycle, rigid tapping | None needed |
| Depth 5×D to 10×D | Peck cycle, 1×D retract | Thread mill for the thread |
| Depth over 10×D | Not recommended | Gun drilling, then thread mill |
| Hardened steel above 45 HRC | Carbide, low speed | EDM or thread milling |
| Plastic and soft alloys | Form tap | Thread milling |
| Blind hole, 3 threads max | Careful depth control | Thread mill with full profile |
| Thin wall under 2 mm | Support the wall | Ream after drilling |
| Thread over M20 in a costly part | Higher breakage risk | Thread mill |
The trade-off in one line
For holes under 5×D in aluminium or mild steel, drill and tap on a rigid synchronized spindle is the fastest and cheapest route; for deep holes, hard alloys or threads in a part you cannot afford to scrap, thread milling or gun drilling is worth the extra cycle time.
Questions engineers ask
What hole size should I put on the drawing for a tapped hole?
Put the thread callout, not the drill size. The shop picks the drill from the tap type and material. For a cut tap the drill is nominal minus pitch; for a form tap it is about nominal minus half the pitch.
If you want a specific minor diameter, add it as a reference dimension and mark it REF so the shop knows it is not a hard requirement.
How much thread engagement do I actually need?
In steel, one times the nominal diameter of full thread carries most of the load. In aluminium and plastics you want 1.5× to 2×. In cast iron, 1.5× is common.
For a blind hole, add about one pitch of clearance at the bottom for chips and lead. Three full threads plus that clearance is a practical minimum.
Why do my tapped holes come out oversized?
Usually the drill is running out of true, or the tap is not synchronized with the spindle. Check drill runout first; more than 0.05 mm TIR shows up as an oversized hole.
On a floating tap holder, misalignment adds to it. Rigid tapping on a synchronized spindle removes that source of error.
Can you tap a hole on the same machine after drilling?
Yes. On our mill-turn centers and 5-axis machining centers, drilling and tapping run in one setup with rigid tapping. That keeps the thread concentric with the bore.
On parts with threads on several faces, the Ø400 mm rotary table lets us index instead of refixturing.
Do you inspect threads?
Yes. Threads are checked with go/no-go gauges and, on request, with thread micrometers or optical comparison. Every part is inspected before shipment, and inspection reports are available on request.
We hold ±0.005 mm on critical bores and hole positions where the print calls for it.
What if the tap breaks inside the part?
We stop and assess. A broken tap in a blind hole can sometimes be removed by spark erosion or a tap extractor. If the part is a one-off prototype, we may remachine it rather than risk further damage.
This is one reason we quote thread milling for expensive parts with small threads.
Send us the print, get a process answer
Upload your drawings and we will come back within 12 hours with a quotation and a free DFM analysis, including hole and thread callouts that are hard to machine.
12-hour quote100% inspectionNo minimum order quantityNDA on request
Follow GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
