The Boring Basics of CNC: Beginning

• 1
  Key takeaways
• 2
  What changes when you bore a hole
• 3
  Boring heads, bars and inserts
• 4
  Helical and circular interpolation in practice
• 5
  Speeds, feeds and depth of cut that hold size
• 6
  When boring is the wrong choice
• 7
  Boring compared with reaming and drilling

Drilling produces a hole that is close. Boring makes it true. A single-point tool sweeps a circle inside the hole, and the radius of that circle is set by the tool, not by the drill. That is the whole point of the operation, and it is where the basics of CNC boring start.

The drill leaves errors behind. The hole comes out slightly oversized, often lobed rather than round, and off-center by a few hundredths of a millimeter. Boring removes that error in one pass. The tool cuts only the high spots first, then all of the wall, so the hole cleans up to a diameter you commanded.

Boring also earns you position. Because the tool is interpolated on a controlled path, you can correct a hole that was drilled slightly off by shifting the work offset. On a mill that is a program edit, not a new part. On a lathe the same correction happens with the tool offset.

The trade-off is time. A boring pass removes little material and cannot run as fast as a reamer. You accept that cost when the hole carries a bearing, a seal, a piston or a dowel pin. If the hole only passes a bolt, you probably do not need to bore it.

• 1
  RoundnessSingle-point cutting averages out drill lobing; two-point contact follows it.
• 2
  Size controlAdjust the head or the offset in microns and re-cut; no new tool needed.
• 3
  PositionThe interpolated path can be shifted to bring a wandering hole back on center.

A boring head holds the cutting insert and gives you a way to change the cutting radius. On a machining center the head mounts in the spindle taper or in a collet holder. Its adjustment screw moves the insert outward in small increments, usually 0.01 mm per division or finer.

There are two common families. The adjustable boring head uses a sliding block for a wide range of diameters and is set by hand or with a dial indicator. The fine-boring head uses a differential screw and can hold a few microns across a production run. For holes under Ø20 mm, a solid carbide bar in a shrink-fit holder is often stiffer than any head.

The bar matters as much as the head. A bar that is too long for the bore will deflect under cutting load and cut a taper. The usual rule is to keep the bar length at no more than four times its shank diameter. Past that, switch to a heavier bar or accept two passes with a spring pass.

Inserts do the cutting. For aluminum, a sharp positive-rake insert with a polished face keeps built-up edge away. For stainless and titanium, a small nose radius and a light feed reduce work hardening. For cast iron and steel, a modest hone is enough. The insert also sets the surface finish: a 0.4 mm nose radius at 0.1 mm/rev typically lands around Ra 0.8–1.6 μm.

On a mill, boring happens in two ways. The tool can feed straight down the axis of the hole, which is true boring. Or the tool can spiral into the hole while stepping down, which is helical interpolation. Both produce a round hole, but they behave differently.

True axial boring plunges a single-point tool along the hole axis. The tool does not move sideways, so the machine's circular interpolation accuracy does not enter the result. That makes it the more accurate method for a deep, precise bore. It requires a bar long enough to reach the bottom of the hole, which is where deflection comes back.

Helical interpolation moves the tool in a spiral path, cutting the wall as it descends. It needs a smaller tool, reaches deep holes more easily, and clears chips well. The price is that the final diameter depends on the machine's ability to follow a circle. On a well-aligned machine that error is small; on a worn one it shows up as lobing.

Circular interpolation, a full circle at one depth, is used for shallow counterbores and finishing passes. It is fast and forgiving. It is also the method most affected by backlash and servo tuning, so it is a poor choice when the hole tolerance is tighter than ±0.02 mm.

• 1
  Axial boringBest roundness and size control; limited by bar length.
• 2
  Helical interpolationGood for deep holes and chip evacuation; diameter depends on machine accuracy.
• 3
  Circular interpolationFast finishing for shallow features; avoid for tight tolerances.

Boring cuts a small radial depth, so the load on the insert is low and the speed can be higher than you would use for a full-slot cut. In 6061 aluminum, 300–600 m/min is normal. In 304 stainless, 120–180 m/min. In Ti-6Al-4V, 40–70 m/min. Start at the low end and move up only if the chip breaks cleanly.

Feed per revolution sets the surface finish. A common target is 0.05–0.15 mm/rev for finishing, depending on nose radius. Feed too low and the insert rubs, which raises temperature and can smear the wall. Feed too high and the scallop height grows. For a 0.4 mm nose radius, 0.08 mm/rev gives a theoretical Ra around 0.8 μm.

Depth of cut is kept small on purpose. A finishing pass removes 0.1–0.3 mm radially on a diameter. That is enough to clean up the drill error without loading the bar. If a hole needs 2 mm of stock removed, take two passes rather than one. The first pass corrects the shape, the second sets the size and finish.

A spring pass helps when the bar deflects. Run the same pass again with no change to the offset. The tool cuts only the material it was pushed away from, which reduces the taper left by the first cut. It costs one extra pass and often saves a rework.

Boring is not always the answer. If the hole is small, short and only locates a bolt, drilling plus reaming is faster and cheaper. Reaming holds size well in a through hole with a consistent diameter, but it follows the drilled axis, so it will not correct position or roundness.

Deep holes are a boundary. Past a depth-to-diameter ratio of about 6:1, a standard boring bar chatters. The fix is a tuned or damped bar, or a different process. Boring on a lathe with a part that can be held in a steady rest works better for long, straight bores.

Thin walls are another boundary. A thin-walled tube will deflect under the cutting load and spring back after the pass, leaving an oval bore. Support the outside with a sleeve or reduce the depth of cut to 0.05 mm and take more passes.

Finally, consider the feature count. If a part has one or two tight holes, boring is easy. If it has twenty coaxial bores on the same axis, a dedicated line-boring setup is a better fit than interpolating each one on a mill.