CNC Boring Basics: How a Single-Point Tool Fixes a Hole

• 1
  What happens when a single-point boring bar cuts
• 2
  How boring is set up on a CNC machine
• 3
  Speeds, feeds and depth of cut for boring
• 4
  Bore geometry that boring can and cannot hold
• 5
  Boring compared with drilling, reaming and honing

Every set of CNC boring basics starts with one fact: the tool has a single point. A boring head holds one insert on the end of a bar, and that point sweeps a circle as the spindle turns. The circle it leaves behind is the hole. Because only one edge touches the work, the diameter is set by how far the insert sits from the spindle axis, not by the tool's own size.

That is the whole advantage. A drill is ground to a fixed diameter, so wear and resharpening push the hole off size. A boring head is adjustable. Move the insert out 0.02 mm and the hole grows 0.04 mm on diameter. On a fine-boring head, the adjuster reads in 0.01 mm or 0.002 mm steps, so the operator can dial in the last few microns.

The second effect is straightness. A drill wanders with the grain of the material and with any asymmetry in its two edges. A boring bar is supported over a long length and cuts on a path set by the machine. That is why a 300 mm deep bore can hold a straightness of 0.02 mm where a drilled hole would drift far more.

Radial force matters too. A single point pushes the bar away from the cut, so a long, thin bar deflects and the hole comes out tapered. Depth-to-diameter ratio is the number to watch. Past about 4:1, we switch to a carbide bar or a tuned bar with damping. Past 8:1, the setup needs a dedicated approach and slower feed.

• 1
  One point, one diameterInsert offset sets bore size, not tool diameter.
• 2
  Adjustable in micronsFine heads index in 0.01 mm or smaller steps.
• 3
  Straighter than drillingPath comes from the machine, not the drill tip.

Boring on a machining center usually follows a drilled or cast hole. The bar enters along the spindle axis, cuts a short length, and retracts. On a lathe, the bar is held in the turret and the part turns, which gives a rounder bore because the workpiece, not the tool, defines the circle. Both routes use the same insert geometry and the same rules for speed and feed.

Tool offset is the first thing to get right. The operator touches the insert to a known bore, records the X or Y offset, then bores a test cut and measures. One pass tells the truth. We aim to leave 0.3–0.5 mm on the radius for a finish pass in steel, and 0.2–0.3 mm in aluminium, so the finishing insert has enough material to cut rather than rub.

Retraction is where scrap happens. A boring bar must move off the wall before it leaves the hole, or the back of the insert drags a spiral scratch down the bore. Most controls handle this with a canned cycle, but the direction of the offset has to match the tool orientation. Get it wrong and the first part is ruined.

Coolant choice shows up in the finish. Through-tool coolant clears chips from a blind bore and keeps the insert cool. On deep holes, high-pressure coolant also helps break the chip. Without it, a long stringy chip wraps the bar and marks the surface on the way out.

• 1
  Touch off, then test cutMeasure one pass before running the batch.
• 2
  Leave stock for the finish pass0.3–0.5 mm on radius in steel.
• 3
  Retract off the wallPrevents a spiral scratch on the way out.

Boring runs slower than milling with the same material because the bar is slender and the overhang is long. In 6061 aluminium, a carbide insert runs at 200–350 m/min surface speed and 0.08–0.15 mm per revolution feed. In 1045 steel, expect 120–200 m/min and 0.05–0.12 mm per rev. Stainless 316 and 17-4PH drop to 80–150 m/min because the material work-hardens under the cut.

Depth of cut is limited by bar stiffness, not by the insert. A short bar in a rigid setup can take 2 mm on the radius in steel. A bar at 6:1 overhang should take 0.3 mm or less. Push past that and the bar sings, the finish goes rough, and the diameter wanders along the bore.

Chip control decides whether the insert survives. A negative rake insert with a molded chipbreaker curls steel into short C shapes that fall clear. A flat-top insert in the same cut makes a long ribbon that tangles. In aluminium, a polished positive-rake insert stops built-up edge from smearing the bore wall.

Surface finish follows from feed per revolution. At 0.05 mm per rev with a 0.4 mm nose radius, the theoretical Ra is around 0.3 μm. Double the feed and the finish roughly quadruples. That is the lever to pull when a drawing calls for Ra 0.2–0.8 μm. On our 5-axis centers, a light finish pass at 0.03–0.05 mm per rev gets there in most materials.

• 1
  Aluminium 6061200–350 m/min, 0.08–0.15 mm per rev.
• 2
  Steel 1045120–200 m/min, 0.05–0.12 mm per rev.
• 3
  Stainless 31680–150 m/min, light depth of cut.
• 4
  Finish feed0.03–0.05 mm per rev for Ra 0.2–0.8 μm.

A through hole in a plate is the easy case. Bore it from one side, keep the overhang short, and hold ±0.005 mm on diameter without drama. A blind bore with a flat bottom is harder, because the bar has to reach the corner and the insert needs a relief angle that clears the shoulder. Tell us the corner radius you need; a sharp internal corner cannot be bored.

Interrupted bores change the picture. A cross hole, a keyway or a cast window breaks the cut twice per revolution, and each impact loads the insert. We reduce feed by 30–50% and pick a tougher grade. A carbide insert that lasts all day in a solid bore can chip in twenty parts when the cut is interrupted.

Thin walls are the other trap. A 2 mm wall around a 40 mm bore will deflect as the insert pushes, so the hole comes out lobed and the wall springs back after the bar passes. Rough, let the part rest, then take a light finish pass. Clamping pressure matters as much as the cut.

Position, not just size, has to hold. A bore that is round and on diameter but 0.05 mm off centre will not accept the bearing. On a 4-axis or 5-axis machine, we bore in the same setup as the mating face so the perpendicularity and the centre distance come from one datum. That is usually better than hitting the tolerance on a second op.

• 1
  Through holesEasiest to hold at ±0.005 mm.
• 2
  Blind holesNeed corner relief; sharp corners are impossible.
• 3
  Interrupted cutsCut feed 30–50%, use a tougher grade.
• 4
  Thin wallsRough, rest, then finish light.