Drilling Machines and to Die CNC: How the Cut Actually Happens
This page explains what happens inside the hole on drilling machines and to die CNC, from the moment the point touches metal to the moment the drill retracts. We cover spindle load, chip evacuation, heat, hole accuracy and the limits of the process. Engineers and buyers can use it to judge whether a hole should be drilled, bored, reamed or moved to a mill-turn machine.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
What happens at the point on drilling machines and to die CNC
A twist drill does not cut the way an end mill cuts. The chisel edge at the center of the point has almost no cutting speed. It pushes and extrudes metal instead of shearing it. That is why a Ø10 mm drill can need more thrust than a Ø10 mm end mill at the same feed. The force goes into the web, not the flutes.
Once past the chisel edge, the lips take over. Cutting speed rises with diameter, so a Ø20 mm drill at 1,200 rpm sees roughly 75 m/min at the outer corner. Heat builds at that corner first. If coolant cannot reach it, the margin wears and the hole tightens within a few parts.
The margin, a narrow land behind each lip, rubs the wall. It guides the drill but also generates friction. Too much margin contact and the hole bell-mouths at entry; too little and the drill walks off center on an inclined surface.
Chip evacuation decides whether any of this stays stable. A chip that curls and exits is fine. A chip that packs in the flute stops the cut, spikes torque and usually snaps the tool on the retract stroke.
- 1Chisel edgeExtrudes metal, needs high thrust and often a spot drill first.
- 2Outer cornerHighest cutting speed and first place to wear.
- 3MarginGuides the drill and rubs the wall.
- 4FluteChip must clear it every stroke.
Toolholding, runout and the first 5 mm
Runout is the quiet killer. A drill held in a worn collet at 0.05 mm TIR will cut oversize by roughly twice that figure. Check the holder before blaming the drill. Clean the taper, seat the collet squarely, and measure TIR on the drill shank, not the flute.
Spot drilling matters more than most shops admit. A 90° spot about 0.5× the drill diameter gives the chisel edge something to bite. Skip it on a machined flat and the drill usually holds center anyway. Skip it on a casting skin and the hole moves.
The first 5 mm set the rest of the hole. If entry is off by 0.1 mm, the drill tends to keep that error for the full depth. Watch the entry on the first part, not the tenth. By then the pattern is set.
On drilling machines and to die CNC, the die side adds one more variable: the part may be clamped on a surface that is not square to the spindle. Check the setup, not just the tool.
- 1Measure TIR on the shankFlute measurement hides holder error.
- 2Spot on skin onlyCastings and forgings need it; flat stock often does not.
- 3Check entry on part oneEntry error carries to the bottom of the hole.
Heat, coolant and what it does to hole size
Drilling makes heat where the chips leave, not where the drill body sits. The outer corner runs hottest. Flood coolant aimed at the entry helps, but through-tool coolant aimed at the point helps more. On deep holes, through-coolant can be the difference between a stable process and a broken drill.
Heat grows the workpiece. A 100 mm aluminum part can move 0.02 mm or more between a cold start and a warm run. Measure holes after the machine has settled, or hold the part at a stable temperature. A hole that measures on-size at 9 a.m. may read undersize at 3 p.m.
Heat also grows the drill. A carbide drill at 100 m/min runs hotter than the shank. Thermal expansion of the tool is small but not zero. It shows up as a hole that tapers slightly over a long run.
Coolant concentration matters as much as pressure. Weak mix lets chips weld to the margin, and a built-up edge changes the effective diameter. Check concentration weekly on any machine running production.
- 1Aim coolant at the pointThrough-tool beats flood on deep holes.
- 2Let the machine settleThermal drift moves hole size by 0.02 mm or more.
- 3Check coolant mixWeak mix builds edge and changes size.
Peck cycles, chip control and drill life
A peck cycle is not always better. Every retract costs time and rubs the margin against the wall. On a 3:1 hole in aluminum, a single stroke with good coolant often beats a peck cycle on both cycle time and hole quality.
Peck when the chip cannot clear. The rule of thumb: if depth exceeds three times the diameter in steel or four times in aluminum, start pecking. Set the peck depth to roughly one diameter, not half a diameter. Too-short pecks polish the margin and wear the drill.
Full retract versus chip-break retract changes chip flow. A full retract clears chips but re-enters the hole every cycle. A chip-break retract keeps the drill in the hole and only breaks the chip. On ductile materials, chip-break often gives better tool life.
Feed and speed follow the material, not the machine's maximum. In 6061 aluminum, 100 to 150 m/min with 0.15 to 0.25 mm/rev is a reasonable starting window. In 304 stainless, drop to 20 to 30 m/min and keep the feed up so the edge cuts instead of rubbing.
Listen to the cut. A clean drill sounds steady. A drill that squeals is rubbing, and a drill that thumps is chipping. The sound changes before the hole does.
- 1Peck past 3×D in steelBelow that, single stroke usually wins.
- 2Peck depth about 1×DShorter pecks polish the margin.
- 3Keep feed up in stainlessLow feed rubs and work-hardens.
Where the process stops working
Drilling has a hard limit at high depth-to-diameter ratios. Past about 5:1 in steel, chip clearance and coolant reach become unreliable. Past 10:1, the drill body flexes and the hole drifts. That is when gundrilling or boring takes over.
Small holes have the opposite problem. Below Ø1 mm, drill stiffness drops fast and spindle runout dominates. A machine with 0.005 mm TIR can still break a Ø0.5 mm drill if the feed is not matched to the point geometry.
Thin walls deflect. A hole drilled 2 mm from a 1 mm wall will push the wall out before the drill finishes. Support the wall or drill before the wall is thinned.
Cross-holes break drills. When a drill exits into an existing cavity, the lips lose support on one side and grab. Reduce feed by half at the breakthrough point, or drill the cross-hole first.
- 1Past 5:1 in steelSwitch to gundrill or boring.
- 2Below Ø1 mmSpindle runout becomes the limit.
- 3Thin wallsDeflect before the hole is done.
- 4Cross-holesHalve feed at breakthrough.
Which hole-making method to pick
Match the method to the tolerance and the depth-to-diameter ratio, not to habit.
| Method | Typical hole tolerance | Best depth-to-diameter | When it is the wrong choice |
|---|---|---|---|
| Twist drill | ±0.05 mm to ±0.1 mm | Up to 3:1 | Tight bore or long deep hole |
| Drill plus ream | ±0.01 mm | Up to 5:1 | Blind hole with no room for chips |
| Boring head | ±0.005 mm or better | Any ratio if bar is rigid | Small diameters under Ø6 mm |
| Gundrill | ±0.02 mm | 20:1 and beyond | Short holes or low volume work |
| Mill-turn | ±0.01 mm | Depends on bar | Simple plate holes at high volume |
Symptom, cause and what to change
| Symptom | Likely cause | What to change |
|---|---|---|
| Hole cuts oversize | Holder runout or dull outer corner | Re-seat collet; replace or regrind drill |
| Hole bell-mouths at entry | Inclined surface or no spot | Add spot drill; face the entry flat |
| Drill squeals mid-cut | Rubbing from low feed | Raise feed per rev; check coolant |
| Chips pack in flute | Peck too deep or coolant weak | Shorten peck; increase concentration |
| Hole tapers over run | Thermal growth of part or tool | Let machine settle; check temperature |
| Drill snaps on retract | Packed chip or worn margin | Full retract; inspect margin wear |
The takeaway
If the hole only needs clearance, drill it and move on. If it carries a bearing or a pin, drill undersize and bore or ream to size. Drilling is a roughing process that happens to make round holes; treating it as a finishing process is where most scrap comes from.
Questions we get on drilling work
How tight a hole tolerance can drilling hold on its own?
A standard twist drill in a good holder holds about ±0.05 mm to ±0.1 mm on diameter, depending on material and depth. That is a starting figure, not a promise.
If the print calls for ±0.01 mm or better, plan on a boring or reaming pass. The drill makes the stock, the boring bar makes the size.
When should a hole move to a mill-turn machine instead?
When the part has features on more than one face, or when the hole is coaxial with a turned diameter. One setup beats two, and concentricity improves.
For a simple plate with through-holes, a 3-axis machine is faster and cheaper. The mill-turn only pays off when it removes a second operation.
Does peck drilling always improve hole quality?
No. Peck cycles add retract time and rub the margin against the wall on every stroke. On short holes in aluminum, a single stroke with good coolant usually gives a better wall and a shorter cycle.
Peck when the chip cannot clear, which generally means past 3×D in steel or 4×D in aluminum. Below that, try a single stroke first.
Why does the same program cut oversize after a tool change?
The new drill may have a different point angle or a slightly different diameter from the regrind. Even 0.02 mm of difference shows up in the hole.
Measure the first part after every tool change. If the size shifts, adjust the cutter compensation before running the batch.
What controls hole position more, the machine or the drill?
The machine controls position; the drill controls size and straightness. A machine with 0.005 mm positioning still makes a crooked hole if the drill walks at entry.
Spot drilling, a rigid holder and a square setup do more for position than a tighter machine spec.
How do we keep drilling data repeatable across shifts?
Fix the variables that drift: coolant concentration, tool change interval, and warm-up time. Write them on the setup sheet.
Measure the first part of each shift, not the last. Drift shows up early if you look for it.
Send us the drawing, get a drilling plan back
We review hole tolerances, depth ratios and material before quoting, so the process matches the print. Quotation and free DFM analysis within 12 hours.
12-hour quote100% inspectionNo minimum order
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
