How CNC Drilling Machine Works
This page explains how CNC drilling machine works on the shop floor: how the spindle, axes and control read a program, how the drill enters the material, and how you set speeds and peck depths so the hole lands on print. It is written for design engineers, CNC operators and buyers who need to judge whether a hole callout belongs on a drill or on a mill.
Key takeaways
How CNC Drilling Machine Works: Motion and Control
A CNC drilling machine makes holes from coordinates, not from a hand wheel. The control reads a program, moves the table or the spindle to an X and Y position, then feeds the rotating drill down along Z. The drill removes material with its two cutting lips and the chisel edge at the center. Everything else on the machine exists to hold that position and that feed rate steady.
The axes are driven by servo motors through ball screws and linear guides. A rotary encoder on each motor reports position back to the control hundreds of times per second, so the loop corrects for backlash and cutting force before the error shows up in the part. On a rigid machine with a warm spindle, position repeats well inside ±0.005 mm.
Depth comes from the Z command, but the real reference is the top of the material. Operators touch off the face, set that point as Z zero, and add the drill point allowance to the program depth. Skip the allowance and a blind hole comes out short by roughly 0.3 × the drill diameter.
The control also runs the canned cycles. G81 drills straight to depth. G83 pecks and retracts. G73 chips without a full retract. Choosing the wrong cycle is one of the most common reasons a deep hole comes out oversize or the drill snaps.
What the Drill Does Inside the Hole
A standard twist drill has a chisel edge at the center that does not cut cleanly. It pushes material ahead of the point until the lips take over. On a flat or angled surface, that push is what makes the drill walk off position before the flutes are fully engaged. A spot drill or center drill creates a cone that guides the point in.
As the flutes go deeper, chip evacuation gets harder. Chips pack into the flutes, friction rises, and the drill starts to rub instead of cut. The hole grows oversize, the surface turns rough, and the margin overheats. Pecking breaks the chip into short pieces and lets coolant reach the tip.
Hard materials change the tool, not the method. Aluminium 6061 and 7075 cut cleanly with uncoated or polished carbide at high surface speed. Stainless 304 and 17-4PH work-harden, so the drill has to keep cutting and never dwell. Titanium TC4 needs sharp edges, low surface speed and steady feed.
Soft and gummy plastics are the opposite problem. POM and PP can grab the drill and pull it into the hole. Use a sharper point angle, reduce the feed at breakthrough, and back the part with a sacrificial plate so the exit edge does not blow out.
Speeds, Feeds and Hole Quality
Surface speed sets spindle rpm. For carbide in aluminium, 150–300 m/min is normal. In mild steel, 80–120 m/min. In stainless, 40–70 m/min. In titanium, 25–45 m/min. Convert with rpm = (surface speed × 1000) ÷ (π × drill diameter). A Ø8 mm carbide drill in aluminium lands around 6,000–12,000 rpm, which is why the machine needs a spindle that reaches those speeds.
Feed per revolution controls chip thickness. A common starting point is 0.02–0.05 mm/rev for small drills, 0.10–0.25 mm/rev for Ø10–20 mm tools. Too light a feed rubs and work-hardens stainless. Too heavy a feed on a small drill bends it.
Hole position and hole size behave differently. Position depends on the machine, the fixture and the spot drill, so it holds tight. Size depends on the drill, the grind and the material, so a twist drill typically runs 0.03–0.08 mm over nominal. If the print calls for H7, drill undersize and ream.
Coolant matters most past 3×D. Through-spindle coolant reaches the tip where flood coolant cannot. Without it, peck depth should drop to 1×D and the feed should come down about 20 percent.
Step by Step: Drilling a Hole on a CNC Machine
Work through these in order. Most hole problems trace back to a step that was skipped.
- 1Read the print and pick the toolNote diameter, depth, tolerance and surface finish. Choose a drill 0.1–0.3 mm under the finished size if a reamer follows. Check flute length against hole depth.
- 2Check the setup before the spindle turnsConfirm the fixture clamps on a solid face, not over the hole. Indicate the vise or fixture within 0.02 mm. Verify the tool length offset with a setter or a touch-off on the material face.
- 3Spot drill the locationUse a 90° or 120° spot drill to a depth of about one third of its own diameter, so the cone is wider than the twist drill point. This is the step that fixes position.
- 4Drill with the right cycleHoles up to 3×D can run in one pass at 0.10–0.25 mm/rev. Past 3×D switch to G83 pecking with a 1×D–2×D peck. Keep feed steady through the cut; do not dwell at the bottom.
- 5Control breakthroughReduce feed by 30–50 percent in the last 0.5 mm when drilling into a cross hole, a thin wall or a laminated stack. Breakthrough is where drills grab and parts deform.
- 6Ream or bore only if the print needs itReam at two thirds of the drilling feed and about one third of the speed. Leave 0.1–0.2 mm radial stock. Bore instead when position or roundness is the critical callout.
- 7Deburr and inspectBreak both edges, then check diameter with pin gauges or a bore mic and position with a CMM or height gauge. Log the result against the tool offset so the next run starts from known numbers.
Which Hole-Making Method Fits the Callout
Match the method to the tolerance and the feature, not to habit.
| Method | Typical size band | What it holds | When to use it |
|---|---|---|---|
| Twist drilling | Ø0.5–40 mm | Position tight, size +0.03–0.08 mm | Clearance holes, tapped holes, pilot holes |
| Peck drilling (G83) | Depth past 3×D | Chip clearance, cooler drill | Deep holes in steel, stainless, titanium |
| Reaming | Ø1–25 mm | Size within 0.005–0.01 mm | H7 bores, dowel and pin holes |
| Boring on a mill | Ø6–200 mm | Position and roundness | Close-tolerance bores, interrupted cuts |
| Punching (sheet) | Ø1.5–25 mm | Fast, flat parts only | Thin sheet without a machined finish |
CNC Drilling Questions Engineers Ask
How does the machine know where the hole goes?
The program carries X and Y coordinates for every hole, taken from the CAD model or a drawing. The control moves the axes to each coordinate and the encoder loop confirms the position before the Z feed starts.
Position accuracy comes from the machine, the fixture and the spot drill far more than from the drill itself. If the fixture moves, every hole moves with it.
Why does my drilled hole come out oversize?
The usual causes are a dull or off-center grind, too light a feed, chips packing in the flutes, or a drill that is too long for the job. Rubbing heats the margins and the hole grows.
Check the drill point first, then raise the feed and add pecking. If the print needs a tight size, drill undersize and ream.
When should I stop drilling and bore instead?
Bore when the callout is about position, roundness or straightness rather than just diameter. A drill follows its own point, so it cannot correct a hole that started off location.
A single-point boring head cuts on one edge and corrects both size and geometry. It costs more cycle time, so use it where the tolerance demands it.
Do I need through-spindle coolant?
Not for shallow holes. Flood coolant is enough up to about 3×D. Past that, through-spindle coolant reaches the cutting edges and lets you keep the feed up.
Without it, shorten the peck to 1×D and reduce the feed about 20 percent. The drill will last longer even though the cycle takes longer.
How deep can a twist drill go before it needs a pilot?
A standard twist drill is reliable to about 5×D without a pilot, and 10×D with a pilot hole or a spot drill. Past that, use a long-series drill with a smaller point angle or switch to gun drilling.
Deep holes also drift. If the hole has to stay straight at 10×D or more, plan for a boring pass.
What tolerance can drilling hold on a production run?
At GreatLight, drilling and the following operations run to ±0.005 mm on position where the fixture and machine allow it, with 100 percent inspection before shipment and reports on request.
Size tolerance depends on the tool. A drilled hole typically runs over nominal; add reaming or boring when the print needs a controlled fit.
Send the Print, Get a Drilling Plan
Upload your drawing and we will return a quotation with a free DFM analysis within 12 hours, plus comments on which holes need reaming or boring.
12-hour quote100% inspectionNo minimum order quantity
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
