Drilling with the CNC machines

How to make holes on the CNC machines: when to drill in the CNC, when to finish on a pillar drill, and when to mill the hole instead, with ready-made settings for the most common case, small holes in aluminium.

The short version

• Small holes (up to about 6 mm): drill them in the CNC, using the settings below.

• Larger holes: spot them in the CNC and finish on a pillar drill, or mill them with an end mill.

• Feed firmly. A drill fed too slowly rubs instead of cutting, gets hot and goes dull.

• Peck deep holes and keep chips moving out of the hole with air or MQL (minimum-quantity lubrication).

• Test on scrap first, then adjust from the chips, the sound and the finish.

Choose a method

Things to weigh:

• Larger drills need low rpm and a lot of torque and push. The CNC spindles are weak at low rpm (see Why not just slow the spindle down?). A geared pillar drill is the right tool for them.

• Moving the part costs accuracy. If the holes must line up precisely with other machined features, or the part is awkward to clamp on the pillar drill, keep it in the CNC and mill the holes.

• Milling handles many hole sizes with one cutter, and finishes everything in one clamping.

Before starting

• Check the shank, not just the cutting diameter.

  • Carvera Air: standard 1/8 inch (3.175 mm) collet, and the tool needs a tool collar. A 2.5 mm hole needs a drill with a 2.5 mm tip and a 1/8 inch shank.

  • Betongsuggan and Portalfräsen: ER20 collets; pick the one that fits the shank.

• Use a short drill. A long, flexible drill wanders and breaks.

• Check the depth. The full diameter ends above the drill tip. For through holes, leave clearance below the part so the drill doesn't hit the table or fixture.

• Dry run the program above the work to check the path and clearances.

Drilling in the CNC

Step 1: Know the drill material

Cobalt HSS is still HSS. A gold or black coating does not make a drill carbide; read the label. Carbide-tipped masonry drills are not metal-cutting drills.

Step 2: Look up the settings

Aluminium quick reference for short, sharp drills in shallow holes. Speeds are worked out from 60 m/min (HSS) and 100 m/min (carbide), and the feed is the starting range from the table in step 3.

Start in the middle of the feed range. A 6 mm HSS drill is just above the 3,000 rpm limit; spotting and finishing on the pillar drill is often easier.

For other materials or sizes, work it out as described in step 3.

Step 3: Calculate settings for other materials

Cutting speed (how fast the drill's edge moves through the material):

Feed per revolution for 1–8 mm drills in aluminium or brass, HSS or carbide alike:

Then calculate:

1. rpm = 1,000 × cutting speed ÷ (π × drill diameter in mm)

2. Z feed (mm/min) = rpm × feed per revolution

If the rpm is above the machine's maximum, use the maximum and calculate the feed from that. The BZT drilling speed calculator does the same sums.

Worked example: 2.5 mm drill in aluminium, 0.05 mm/rev

• HSS at 60 m/min: 1,000 × 60 ÷ (π × 2.5) ≈ 7,600 rpm; 7,600 × 0.05 = 380 mm/min

• Carbide at 100 m/min: ≈ 12,700 rpm; 12,700 × 0.05 = 635 mm/min

Higher rpm needs a proportionally higher Z feed to take the same chip per turn.

HSS drilling in aluminium. At 80 m/min, a 2.5 mm drill needs about 10,200 rpm, 6 mm about 4,240 rpm, and 8 mm about 3,180 rpm. A shaded band shows 60 to 100 m/min. The GPenny 3,000 rpm load limit and 24,000 rpm maximum are marked.

The chart uses 80 m/min, the middle of BZT's 60–100 m/min range for HSS in aluminium. The bigger the drill, the closer it gets to the 3,000 rpm limit.

Notes:

• Plastics: a sharp HSS drill is enough. Carbide doesn't stop plastic melting; use air and clear chips often instead of raising the rpm.

• Don't double the feed for carbide. The feed ranges are the same for both.

• Feed per revolution is for the whole drill. Don't multiply it by the two cutting lips.

• Don't raise the rpm to get more power. It overheats the drill.

Step 4: Feed fast enough to cut

At high rpm, the Z feed can look alarmingly fast. Don't turn it down just because the spindle sounds fast. Each cutting lip has to take a real chip on every turn. Too little feed makes the edges rub: the drill heats up, goes dull and makes long chips that are hard to clear.

For an example feed of 0.05 mm per revolution, Z feed increases with rpm: 200 mm/min at 4,000 rpm, 500 at 10,000, and 600 at 12,000. At 10,000 rpm, reducing Z feed to 50 mm/min gives only 0.005 mm per revolution.

At 10,000 rpm, 500 mm/min gives 0.05 mm per revolution. Turning it down to 50 mm/min gives only 0.005 mm, a tenth of the chip. The drill runs hotter and cuts worse.

• When changing rpm, change the Z feed by the same proportion.

• Never let the drill dwell, spinning at the bottom of the hole. Retract instead.

• If the spindle slows down or the tool bends, stop and check the tool, settings and method. Don't try to finish by creeping.

Step 5: Peck and clear chips

Chips leave the hole along the drill's flutes. The deeper the hole, the further they travel and the more easily they pack. Aluminium makes long, stringy chips that wrap around the drill. Packed chips can snap a drill.

Peck drilling cuts the hole in short strokes:

1. Drill down one peck depth at normal cutting feed.

2. Retract to break or clear the chip.

3. Rapid back to just above the previous depth, then switch to cutting feed.

4. Repeat to full depth.

Peck depth sets how far it drills between retracts; feed sets how fast it cuts. Keep the normal feed during each peck. Start with short pecks and make them shorter if chips pack as the hole gets deeper.

Schematic drill-tip paths. G73 makes small retracts inside the hole to break chips. G83 returns above the work between pecks and then approaches the previous depth before feeding into new material. Blue means cutting feed, red retract, grey return.

Select the cycle in CAM and use the machine's post-processor. For chip clearing, set the retract plane above the work; a small lift inside the hole doesn't empty it.

Give the chips a way out:

• Use the machine's air assist, MQL or dust collection as described on its page. The spindle's water cooling only cools the spindle, not the cut.

• Watch that chips leave the hole and get blown clear of its mouth.

• If chips nest around the drill or the load rises as the hole deepens, stop and clear them, then shorten the pecks for the next hole.

• With carbide, keep re-entry smooth and the hole clear, so the edges don't hit packed chips.

Spot in the CNC, finish on a pillar drill

1. In the CNC, drill a shallow spot or a small pilot hole at each position.

2. Move the part to a pillar drill. For metal, use the Arboga E100; a demonstration is required before first use.

3. Clamp the part securely and line the drill up with each spot before cutting.

4. Drill to the final diameter, pecking out chips on deep holes.

• Spot or pilot? A spot only guides the drill tip. A pilot hole removes material all the way through.

• Spotting for a carbide drill: use a spot angle at least as large as the drill's point angle, so the drill's point touches first.

• Accuracy: some is lost when the part is moved. Use a fixture if it matters.

Mill the hole with a helix

In helical milling, an end mill smaller than the hole circles in X and Y while moving down in Z. The hole is cut a little at a time, so there's no need to push a large drill through. It works well for shallow holes and counterbores, and one cutter can make several hole sizes.

• Cutter: an end mill suited to the material and rated for ramping, with enough flute length to reach through the part.

• Ramp: set the ramp angle or pitch per turn from the tool's data.

• Centre: check that the path clears the middle of the hole. A single helix can leave a core; larger holes may need a pocket toolpath.

• Reach: check flute length, holder clearance and room for chips. Deep, narrow holes are a poor fit.

• Feed on curves: the cutter centre travels a smaller circle than the hole wall, so a straight-line feed can overload the cut. Check that CAM compensates for this, but only once.

• Post-processor: use the settings in CNC Intro, including Allow helical moves: off for LinuxCNC. The post converts the helix into moves the machine can run. Check the posted toolpath and dry run it above the work.

Why not just slow the spindle down?

A pillar drill has gears: it trades motor speed for turning force (torque). The Arboga E100 has only about 440 W but runs at 200–1,300 rpm through gears, so it has plenty of torque for large drills.

The CNC spindles have no gears. Their torque stays about the same at any speed, 1.47 N·m on Betongsuggan (3.7 kW) and 0.88 N·m on Portalfräsen (2.2 kW), so their power falls with the speed:

Two aligned graphs for the GPenny spindles. Power rises with rpm to 3.7 kW on Betongsuggan and 2.2 kW on Portalfräsen; torque stays near 1.47 and 0.88 N·m. At 3,600 rpm, power is 555 and 330 W. Below 3,000 rpm is marked no load.

Power (W) = torque (N·m) × 2π × rpm ÷ 60. With constant torque, power is proportional to rpm.

A large drill needs low rpm, high torque and a strong push into the material. At low rpm the CNC spindle has the same small torque and only a fraction of its power, and the machine and workholding have to take the push. That is why large holes go to the pillar drill, or get milled with a smaller cutter, rather than using the largest drill the collet will hold.

Sources

Based on Erik Cederberg's explanation in #cnc on 4 November 2026 and the follow-up about helical milling.

• CNC Machines

• CNC Intro