CNC Drill Press Guide: How the Cut Actually Happens

• 1
  What Happens at the Cutting Edge
• 2
  Speeds and Feeds: Setting Spindle RPM
• 3
  Fixturing, Bushings and Hole Position
• 4
  Where a Drill Press Stops Being the Right Tool
• 5
  Drill Press vs CNC Machining Center

The tool turns on a vertical axis. The workpiece sits on a table, and the spindle feeds downward. The chisel edge at the center of a twist tool does not cut. It pushes material aside. That is why a 10 mm twist tool needs a pilot hole or a split-point grind before it will start cleanly in 304 stainless.

Two angles control most of the behavior. Point angle sets how the tool enters the surface: 118° suits general steel, 135° suits harder alloys and thin sheet because it spreads thrust over a wider area. Web thickness sets how much force the center needs before the flutes take over. A thick web on a large tool means high thrust, which is the usual reason a light drill press stalls or walks.

Margin contact along the flutes stabilizes the tool inside the hole. Too much margin and the tool rubs, generating heat without cutting. Too little and the hole opens oversize. Runout at the spindle compounds both. A tool holder with 0.02 mm runout can produce a hole 0.05 mm oversize before any wear appears.

Chip evacuation decides surface finish more than spindle speed does. Long stringy chips wrap the flutes, raise torque, and score the wall on the way out. Pecking breaks them. The depth per peck matters: go too deep and the chips pack; go too shallow and you spend the cycle time rubbing instead of cutting.

• 1
  118° vs 135° pointUse 118° for mild steel and aluminum, 135° for stainless and sheet.
• 2
  Thin web, lower thrustSplit-point grinds cut required thrust, which helps small spindles.
• 3
  Runout adds to hole sizeMeasure at the holder taper, not at the tool tip alone.

Surface speed drives everything. For HSS tools in 6061 aluminum, run 60–120 m/min. In 1018 steel, drop to 20–30 m/min. In 304 stainless, 10–15 m/min. Carbide roughly triples those numbers, but only if the spindle is rigid enough to avoid chatter. Small drill presses with belt drive cannot hold high RPM under load, so the practical ceiling is lower than the chart says.

Feed per revolution sits between 0.05 mm/rev and 0.25 mm/rev for tools under 12 mm. The rule is simple: too little feed work-hardens stainless and rubs aluminum, while too much feed snaps small tools. A 6 mm carbide tool in 6061 wants roughly 0.10–0.15 mm/rev. A 3 mm tool wants closer to 0.05 mm/rev.

Peck depth should not exceed one tool diameter for deep holes, and half a diameter past 3× depth. Retract fully to clear chips. Coolant choice matters less than people expect on short holes, but on anything past 2× diameter in stainless, through-tool or flood coolant prevents the tip from glazing.

• 1
  Start conservativeCut recommended speed by 20% on first article, then climb.
• 2
  Listen for chatterA squeal at entry means RPM is too high for the setup.
• 3
  Check chip colorBlue chips in aluminum mean the feed is too slow.
• 4
  Lock the tableLoose clamps convert feed force into vibration.

Position error comes from three places: the layout, the fixture, and the tool walking on entry. The layout you can control with a spot tool. A stub spot drill 90° or 120° creates a cone that guides the following tool. Skip it and a standard twist tool will drift 0.1–0.3 mm on a smooth surface, more on rolled plate.

Drill bushings remove most of that drift. A slip-fixed bushing in a plate fixture holds the tool within 0.02 mm of nominal, provided the bushing bore is not worn. Hardened steel bushings last longer; diamond-coated bushings are for abrasive composites and carbide tools. Check bushing clearance every 500 holes and replace when the bore grows past 0.05 mm over the tool shank.

Clamping force should be directly under the hole, not at the far end of the part. Thin plate deflects upward as the tool exits, and that deflection is what tears the exit burr. Back the plate with a sacrificial board or a support plate. For holes under Ø3 mm in sheet, a support plate is not optional.

• 1
  Spot before you drillA 90° spot 1–2 mm deep is enough to start the tool straight.
• 2
  Clamp under the holeSupport at the exit stops the burr from tearing.
• 3
  Check bushing wearReplace when clearance exceeds 0.05 mm over the shank.

A drill press makes round holes on a single axis. It cannot interpolate a pocket, mill a flat, or hold a true position across a bolt circle without a fixture for every pattern. When a part needs six holes on a 200 mm bolt circle at ±0.05 mm true position, the setup cost of a drill press fixture usually exceeds the cost of a machining center running the same part.

Depth control is the second limit. Manual quill feed relies on the operator watching a scale or a stop. That is fine to ±0.2 mm. It is not fine for a counterbore that seats a bearing at ±0.02 mm. CNC drilling with a controlled Z axis holds depth to ±0.005 mm on our machines, which is the tolerance we quote for production parts.

Hole quality is the third. A drill press leaves a reamed or drilled finish around Ra 1.6–3.2 μm. If the drawing calls for Ra 0.8–1.6 μm or tighter, the hole needs reaming, boring, or a fine-boring head. Those operations belong on a mill or a lathe with a rigid spindle and a controlled feed, not on a quill.

Angle and location follow. A drill press drills normal to the table. Any angled hole needs an angle plate, and every angle plate adds stack-up error. Five-axis machining removes that error by tilting the tool instead of the part.

• 1
  One axis onlyNo interpolation, no flat bottoms, no pockets.
• 2
  Depth by eyeManual quill feed is a ±0.2 mm process at best.
• 3
  Finish ceilingDrilled walls sit around Ra 1.6–3.2 μm without reaming.