Boring Bar Feeds & Speeds Calculator 2026

Boring enlarges and trues an existing hole with a single-point tool mounted on a boring bar. It is usually the next step after drilling when diameter control, straightness, or finish must improve. On this page, treat the output as a boring start point rather than a full production release, because holder clamp, bar projection, insert reach, and chip evacuation still decide whether the setup is really stable.

The L/D ratio is unsupported bar length divided by bar diameter, and it is the fastest way to judge boring rigidity risk. Low ratios are forgiving, while long overhang magnifies deflection and chatter quickly because stiffness falls sharply as projection grows. It is still only a screen: clamp length, insert geometry, bore clearance, and machine stiffness can move the real stability limit sooner or later than the simple ratio suggests.

Boring uses a single-point tool to enlarge holes and can adjust diameter by changing depth of cut. It works at any diameter but is slower due to single-point cutting. Reaming uses a multi-flute fixed-diameter tool for finishing to exact size with excellent surface finish. Reaming is faster but limited to standard diameters and removes only 0.1-0.3mm per side. For CNC work: drill → rough bore to within 0.5-1mm → finish bore to size, OR drill → bore → ream for best finish. Boring is more flexible; reaming is faster for standard sizes.

Use anti-vibration bars when a standard steel or carbide bar is running out of stability margin, when the material is difficult, or when finish and size cannot tolerate chatter marks. They can extend the usable window, but they do not fix poor clamp security, weak machine structure, or bad insert reach. Even with a damped bar, treat long-overhang results as starting points that still need a proving cut.

Insert selection for boring depends on three factors: (1) Bore diameter — small bores require small inserts (CCMT 0602 for 10-20mm bores, CCMT 09 for 20-40mm). (2) Material — coated carbide (CVD/PVD) for steel and cast iron, cermet for finishing, CBN for hardened steel, PCD for aluminum. (3) Operation — positive rake inserts (CCMT, DCMT) for finishing and light cuts, negative rake (CNMG) for roughing with stronger edges. Always use the largest insert that fits the bore, as larger inserts provide more cutting edge strength and better chip control.

A common first screen is bore diameter roughly equal to bar diameter plus enough clearance for the body and chips, but that is not the whole answer. Small bores get difficult fast because insert reach, body clearance, chip evacuation, and coolant delivery all tighten at once. If clearance is limited, use this calculator as an early go/no-go check and confirm the exact toolmaker geometry before release.

The first levers are lower feed, larger nose radius, sharper geometry, and less overhang. But boring finish often degrades because of vibration, chip re-cutting, or body clearance before the theoretical Ra math looks bad. Use this calculator to understand the direction of change, then validate the target with a finish-specific check and a real test bore.

Chatter usually starts with too much overhang for the bar, but it is amplified by weak clamping, insufficient bar diameter, poor insert edge condition, chip packing, and running on the wrong speed band. Common first moves are changing speed 15-20%, reducing DOC, shortening projection, or switching to a stiffer or damped bar. If the bore has cross holes, interruptions, or tight clearance, expect more testing than the calculator alone can provide.

Rough boring removes the bulk of material (1-3mm DOC per side) and prioritizes MRR. Use larger inserts, higher feeds (0.15-0.25 mm/rev), and moderate speeds. Fine boring achieves final diameter and surface finish (0.1-0.5mm DOC per side) with precision and lower forces. Use smaller positive inserts, light feeds (0.05-0.10 mm/rev), and higher speeds. For holes with IT7 tolerance or better, always use a two-pass strategy: rough bore to within 0.3-0.5mm of final size, then fine bore to dimension.

Standard boring G-codes: G85 — Boring cycle with feedrate retract (leaves smooth wall). G86 — Boring cycle with spindle stop before retract (prevents drag mark). G87 — Back boring cycle (cuts on retract for back faces). G88 — Manual retract boring (operator controls retract). G89 — Boring with dwell at bottom (cleans up blind hole bottom). For CNC turning: no special cycle needed, program as a standard facing/turning operation using boring bar. Most lathe boring uses G71 rough cycle followed by G70 finish cycle for multi-pass operations.