Drilling with our CNC Machines

Small drills can work well in a CNC mill, but a high-speed milling spindle is a different tool from a geared drill press. Choose the method from the hole size and depth, the drill material, and the machine's capabilities. CNC spotting or a small pilot hole followed by finishing on a pillar drill is often a sensible workflow. For larger, relatively shallow holes, consider milling them with a smaller end mill.

Choose how to make the hole

Start with the hole diameter and depth, the tools you have, and whether you can move the part to a pillar drill.

Small hole through thin material: drill it in the CNC

For a job such as 2.5 mm holes through 3 mm aluminium plate, a short drill is a good starting choice. Small drills suit high spindle speeds, and drilling is a quick way to make a series of small holes.

Use the HSS or carbide starting settings below to choose rpm and feed, and check that the drill's shank fits the collet. Feed it firmly enough to make chips; creeping into the work is not a good substitute for choosing suitable settings.

Larger, shallow hole or counterbore: mill it with an end mill

For a job such as a 10 mm hole through 5 mm aluminium plate, consider a helical toolpath with a suitable 6 mm end mill. The cutter travels in a circle while gradually moving down. This makes the hole a little at a time, so you do not need to push a full-size drill through the material.

This is especially useful when you want to finish the holes without unclamping the part, or need several hole diameters with one cutter. Choose an end mill that can ramp, and follow the helical-milling section below for the toolpath and chip clearing. The cutter needs enough flute length to reach through the work.

Larger or deeper hole, and the part can move: locate it in the CNC, finish on a pillar drill

Use the CNC to make a spot or small pilot hole at each position, then clamp and align the part on the pillar drill for the final diameter. This is often the easiest route when a larger drill needs low rpm, or when a long hole will need frequent withdrawals to clear chips.

For example, an 8 mm HSS drill in aluminium at the 60 m/min starting speed needs about 2,400 rpm. That is below the 3,000 rpm load limit on Betongsuggan and Portalfräsen: finish on the pillar drill or mill the hole instead.

Think about the transfer before choosing this method: can you clamp the part on the pillar drill and align the drill with each spot or pilot? If the part is awkward to move or the hole positions must stay precisely aligned with other machined features, keeping it clamped in the CNC and milling the holes is often easier.

Larger drills need more turning and pushing force. This is why spotting followed by pillar drilling, or milling with a smaller cutter, is often a better choice than fitting the largest drill the CNC collet will hold.

For holes with tight tolerances, plan a finishing operation and measure the finished hole.

Why slowing the spindle reduces available power

The spindle curves for Betongsuggan's 3.7 kW spindle and Portalfräsen's 2.2 kW spindle show approximately constant torque: 1.47 N·m and 0.88 N·m, respectively. Slowing them down reduces power without increasing torque.

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.

Mechanical power is torque multiplied by rotational speed:

Power (W) = torque (N·m) × 2π × rpm / 60

With constant torque, power therefore falls in proportion to rpm. Scaling the nominal 24,000 rpm ratings gives:

At 3,600 rpm, Betongsuggan still has about the same torque as at high speed, but only 15% of its rated power. Drilling needs torque and axial feed force as well as power. The spindle must turn the drill, while the machine and workholding handle the force pushing it into the material.

A geared drill press can trade motor speed for spindle torque. The Metal room's Arboga E100, for example, has a listed motor power of only about 440 W and geared spindle speeds of 200–1,300 rpm. Simply lowering the speed setting on these direct-drive CNC spindles does not make that trade.

Choose settings for HSS and carbide drills

For ordinary shop-bought drills, use the starting points below. Identify the drill material, choose a cutting speed for the workpiece, then set a feed that makes it cut a proper chip.

HSS or solid carbide

Cobalt HSS is still HSS. A gold or black finish does not make a drill carbide. Look at the label: HSS, HSS-Co and solid carbide/VHM describe the tool material. Carbide-tipped masonry drills are a different tool from solid-carbide metal drills.

Starting cutting speeds

For short, sharp metal-cutting drills and shallow holes, start around these values. Use the machine's air assist or MQL for metals and keep chips moving.

These are practical starting values for our setup. Make a first hole in spare material and adjust from the chips, sound and finish. If you have reliable data for a particular drill, use it to refine the settings.

For plastics, a sharp HSS drill is usually enough. Carbide's heat resistance does not prevent the plastic from melting: use air and regular chip clearing rather than chasing higher rpm.

Convert cutting speed to rpm

For drill diameter D in mm and cutting speed vc in m/min:

rpm = 1,000 × vc / (π × D)

Example: HSS drills in aluminium at 80 m/min, within BZT's 60–100 m/min range:

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.

Larger drills need lower rpm, bringing them towards the spindle's lower speed limit. Raising rpm just to get more spindle power can overheat the drill. If the calculation exceeds the machine's maximum speed, cap the rpm and calculate the feed from that speed. BZT drilling speed calculator

Feed fast enough to cut

High rpm can make the calculated Z feed look alarmingly fast. Do not turn the feed down just because the spindle sounds fast. The drill needs to advance enough on each revolution for its cutting lips to take a chip. Too little feed makes the edges rub, generating heat and wearing the drill instead of cutting efficiently. It can also produce long chips that are harder to clear.

Starting feeds without a datasheet

For short 1–8 mm drills in aluminium or brass, use these feed ranges as a starting point. They work as an initial setting for both HSS and solid carbide; changing to carbide does not mean automatically doubling the feed per revolution.

With a short, sharp drill, start around the middle of the band. Keep a steady feed and check that chips leave the hole. A long, flexible drill or a larger drill on a light machine is a reason to use a shorter tool, mill the hole, or finish on the pillar drill.

Convert the chosen feed per revolution into the Z feed:

Feed (mm/min) = rpm × feed per revolution (mm/rev)

Worked example: a 2.5 mm drill in aluminium. Choose 0.05 mm/rev from the table. With HSS at 60 m/min, set about 7,600 rpm and 380 mm/min. With solid carbide at 100 m/min, set about 12,700 rpm and 635 mm/min. The higher rpm needs a proportionally higher Z feed to take the same chip per turn.

How feed changes with rpm at 0.05 mm/rev:

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, feeding at 500 mm/min advances the drill 0.05 mm per revolution. Turning the feed down to 50 mm/min reduces that to 0.005 mm per revolution — one tenth as much. Creeping into the work can make the operation run hotter and cut worse.

Feed in mm/rev is for the whole drill; do not multiply it by two for its two cutting lips.

Check the path and clearances with a dry run above the work, then use the calculated cutting feed. When changing rpm, adjust the linear feed in proportion to keep the chosen feed per revolution. If the spindle slows down or the tool bends under load, stop and check the tool, settings and method rather than trying to finish by feeding extremely slowly.

Keep the drill cutting during each peck. Avoid pausing with it spinning against the bottom of the hole; retract to clear chips instead.

CNC location followed by a pillar drill

Use the CNC to make a shallow locating spot or a small pilot hole with suitable tooling, then finish at the required diameter on a pillar drill. For metal, see the Arboga E100; a demonstration is required before first use.

Clamp the part securely at both machines. At the drill press, align the finishing drill to the CNC location before cutting. Allow for loss of location accuracy when transferring the part; use an appropriate fixture if that accuracy matters.

A shallow spot locates the drill tip; a pilot hole removes material through the hole. When spotting for a carbide drill, use a spot angle at least as large as the drill point angle, so the point contacts first.

Mill larger holes with a helical toolpath

In helical interpolation, an end mill smaller than the hole moves around in X and Y while descending in Z. This lets you choose the cutter diameter and depth per turn instead of removing the full hole cross-section with a drill. It is often useful for shallow holes and counterbores.

• Use an end mill suited to the material and rated for ramping. It needs enough end clearance to cut while descending.

• Set ramp angle or axial pitch from the tool's data. Confirm the path clears the hole centre; a single helix can otherwise leave a central core. Larger holes may need a pocketing strategy.

• Check flute length, reach, holder clearance and room for chips. Deep, narrow holes can be a poor fit for this method.

• Verify internal circular-feed compensation in CAM. The cutter centre travels a smaller circle than the hole wall; copying a straight-line milling feed can overfeed the cut. Do not apply the correction twice if CAM already handles it.

Use the machine's post-processor settings from CNC Intro, including “Allow helical moves: off” for LinuxCNC. The post converts the CAM toolpath into compatible moves. Check the posted toolpath and dry run it above the work.

Tool fit

Check shank diameter, not just cutting diameter. The Carvera Air has a standard 1/8 inch (3.175 mm) collet and needs a tool collar. To drill a 2.5 mm hole with that collet, use a drill with a 2.5 mm cutting diameter and a 1/8 inch shank. Use the correct available collet and collar for the tool. Betongsuggan and Portalfräsen use ER20 collets; select one that fits the shank.

Peck drilling and clearing chips

Chips travel out of the hole along the drill's flutes. As the hole gets deeper, they have farther to travel and more opportunity to pack together. Aluminium often makes long, stringy chips that tangle around the drill or jam in the flutes. Packed chips can bind and snap a drill.

Peck drilling divides the hole into short cutting strokes with retracts between them:

1. Feed down by the programmed peck depth at the normal cutting feed.

2. Retract to break the chip or pull the drill clear so chips can leave.

3. Return towards the previous depth, slowing to cutting feed before reaching uncut material.

4. Cut the next increment and repeat to the final depth.

Peck depth controls how far you drill before retracting; feed controls how fast you cut. For example, a fixed 2 mm peck adds 2 mm of depth on each cutting stroke. Keep the correct feed per revolution during those strokes. With ordinary twist drills and external air or MQL, use short pecks that let chips leave the hole. Shorten the pecks if chips start packing as the hole gets deeper. With carbide, keep re-entry smooth and the hole clear so the cutting edges do not hit packed chips.

Chip breaking or full chip clearing

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.

In LinuxCNC these are G73 and G83, respectively. Select the cycle in CAM and use the machine's post-processor. For a full retract, set the retract plane above the work so the drill actually clears the hole. A small lift deep inside the hole breaks chips but does not empty it.

Give the chips a way out

Use the machine's air assist, MQL or dust collection as described on its page. Check that chips leave the hole and clear away from its mouth, so the drill does not keep cutting the same chips. The spindle's water-cooling circuit cools the spindle; it does not cool or flush the cutting area.

If chips nest around the drill, the flutes pack up, or cutting load rises as the hole deepens, stop and clear them before continuing. Stop the spindle before clearing chips with a brush or removing chips wrapped around the drill. Adjust the peck depth, retract and chip removal before the next hole.

Check full-diameter depth versus drill-tip depth and clearance below a through hole, so the tool does not hit the table or fixture.

Background

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

• CNC Machines

• CNC Intro