EN

Boring Speed, Feed and Bar Deflection

Boring takes an existing hole and gives it its exact size, straightness and finish — things a drill simply cannot do. The cutting speed maths is the same as in turning; what changes everything is that the tool works cantilevered out at the bottom of the hole. So this calculator gives you, alongside the cutting conditions, the deflection of the bar and the diameter error it produces.

In boring, the limit is almost never the cutting speed — it is overhang. Deflection goes with the cube of the length sticking out: double the overhang and the error grows eightfold. Pulling the bar out 10 mm too far costs more accuracy than any speed setting ever will.

Other operations: turning, drilling, milling, threading, tapping.

Bore and bar

δFpL (overhang)d
Step 1 — Recommended cutting speed

These three choices only suggest a cutting speed, which is copied straight into the Vc field in step 2. You are free to replace it with your own.

≈ 180–260 HB

Recommended range: 135 to 240 m/min — starting value 180 m/min

Step 2 — Bore

Filled in by step 1. Editable: if your tooling supplier gives you a figure, theirs wins.

Keep it low in boring: 0.05 to 0.15 for finishing. Never exceed the nose radius of the insert.

On the radius. Keep it above the nose radius, or the tool rubs instead of cutting.

On a light pass the radial share of the cutting force rises: proportionally, the bar deflects most when finishing.

Step 3 — Boring bar

Use the biggest bar that fits: stiffness goes with the fourth power of the diameter.

Length clamped out of the holder, not the total length of the bar.

Asterisks mark the shop terms that decide whether a bore comes out to size; plain definitions sit in the glossary.

Boring, reaming, honing and broaching: which process for which tolerance

Four ways to finish a hole, four different jobs. The drawing decides — axis, depth, tolerance — not the tool that happens to be in the cupboard.

Boring is a single-point cut on a bar. It will true an axis, cut a shoulder, and open a diameter no reamer is made for. A short bar, with the cut kept in order, holds something like an IT grade* of IT7–IT9. Surface finish sits around Ra 1.6–6.3 µm unless that last pass is cut as a finish and not as a shy roughing cut.

Reaming is a multi-tooth sizer. It copies the drilled axis, so a location error stays where the drill put it. Size and roundness improve — IT6–IT7, Ra 0.4–1.6 µm — when the allowance is right. Honing is stones on an expanding mandrel, rotating and stroking: IT4–IT5, a cross-hatch, Ra down to 0.05–0.2 µm, the hydraulic-cylinder finish. Broaching pulls a toothed bar through the hole — splines, keyways, a D-hole — around IT6, a fast cycle, and a tool expensive enough that a one-off feels the cost.

An H7 on a 40 mm hole 15 mm deep is a reamer after a good drill. An H7 on a 40 mm hole 120 mm deep, or a bore that has to clean up an oval already there, is boring. A cylindricity* of 0.005 mm on a tube is a hone. A clearance hole for a bolt is nobody’s honing job.

“Just bore it” is the right sentence only when the axis or the stock is wrong. A single edge can be set onto a new axis; a reamer can only follow the hole it was given. When that hole is already where it should be, a reamer is faster and kinder to the budget.

Choosing a boring bar: diameter, material, damped bars, L/d working limits

The bar is the process. Insert grade is a footnote. Diameter as large as the hole will swallow — 0.7–0.85 × the bore is the usual window, still leaving chip space. A steel bar works up to an L/d of about 4, L being the stick-out*. A heavy-metal shank, tungsten, is taken towards 6. Solid carbide towards 8: about three times the Young’s modulus of steel, so the same stick-out bends less. A damped bar, anti-vibration, with an internal mass, goes to 10–14 × D when the cut stays civilised. The families on this page match those limits. Past a limit, the deflection on the screen is only the polite version of the noise at the spindle.

I = π · d⁴ / 64  ·  δ = Fp · L³ / (3 · E · I)

I is the second moment of the round section, δ the bend at the tip. Stiffness climbs with d⁴. A 16 mm bar is not “a bit stiffer” than a 12 mm bar: 16⁴ / 12⁴ ≈ 3.2. Pulling the stick-out in by 20% cuts the deflection by half, because length enters as L³. Changing Vc does nothing to δ. Nothing. Speed is not a rigidity knob.

A steel bar at L/d = 7, fitted with a “better insert”, is still a steel bar at L/d = 7. The bend changes with a carbide shank, a damped body, or a setup taken from the other side so that L falls. Failing that, the size is recovered on a pass that adds no depth.

The spring pass, and why it brings the size back

The bar bends under the cut. The bore comes out small by twice the deflection, the error being on the diameter: the radius is short by the radial give, the diameter by twice that. A spring pass* is the same offset run again with nothing extra to take — or a whisker of feed and no new ap. Force collapses, the bar stands up, and the edge skims the stock the first pass missed. A few micrometres come off, sometimes 10–20 on a long bar, and the plug gauge goes.

It is no magic on a rigid carbide bar at L/d = 2, where the first pass hardly left the wall. Repeated springing on stainless can polish the bore and work-harden the skin. The pass earns its keep on a steel bar at L/d = 4–6, and on any finishing cut whose last pass was heavy enough to push. This calculator prints the missed stock as a diameter error. That is the metal the spring pass is for.

Heat is the snag. A spring pass on a part still warm from roughing measures right at the machine and small in the morning. Size is taken at the temperature of the inspection, or the compensation and the thermometer go on the sheet together.

Nose radius versus depth of cut: the ap > r rule and what happens when it is broken

When ap falls below the nose radius*, the only contact is the arc. The tool is not cutting on a straight edge. Radial force climbs, the chip becomes a smear, the surface looks burnished, and stainless work-hardens under the rub. The shop rule on a real cut is ap ≥ 1.5–2 × rε. A 0.8 mm nose wants something like 1.2–1.6 mm of ap for roughing. Finishing breaks the rule on purpose — 0.2 mm with a 0.4 mm nose — and pays with deflection and a spring pass.

Break the rule on a long bar and the rubbing arc feeds chatter: helical marks appear whose pitch owes nothing to the feed. The nose comes down before ap is dropped into rubbing. A 0.2 mm nose is a finishing boring insert; it will not take a 2 mm depth of cut. A 0.8 mm nose will not leave an Ra of 0.8 µm at 0.25 mm/rev without a fight.

The same geometry is ordinary outside, in turning. Inside a hole the radial component has nowhere to go but into the bar, so the rule is stricter, not looser.

Chatter in boring: reading the marks, and fixing it with feed rather than speed

Helical ripples whose pitch is not the feed are regenerative chatter*. A corkscrew is the same thing, often with torsion on a long bar. A scaly tear means the cut has gone past “a bit noisy” and is wrecking the surface. Boring chatter is the bar’s natural frequency talking to the chip.

On a mill, spindle speed is sometimes hopped onto a stable lobe. In a bore the excitation is once per revolution per edge, and the bar is a cantilever with a very clear note. Speed changes a little; the note stays. Feed is the knob. A little more feed can thicken the chip, raise the damping and kill the song, if the insert is a tough grade that will take it. A little less feed drops Fp and δ. Both work, on different days. What rarely works is a 40% drop in spindle speed “until it quiets”. The edge only rubs.

  1. The stick-out is shortened first. Nothing else comes close.
  2. A bigger bar, carbide, or a damped body.
  3. A smaller nose, positive rake, an entering angle close to 90°.
  4. Then the feed. Then, if the note remains, a 10% speed change.

Still noisy after that, and the part itself is ringing. It needs support, a bore from both ends, or the retirement of the 12 mm bar in a 50 mm hole that was chosen because it fitted the holder on the machine.

Boring a blind hole: chip evacuation and through-coolant

A through bore dumps chips out of the far side. A blind bore is a bucket. Long stringy chips wrap the bar, scratch the wall, and then lock. The insert needs a breaker that makes C-chips or short commas, not clock springs. Stainless is the usual offender.

Through-coolant down the bar, 20–70 bar at the nose, is the real fix: it cools, lubricates, and pumps the chip back out of the entrance. External flood on a 5 × D blind bore is theatre. The fluid never sees the edge. Pecking — retract, unwind the nest, go back — is the fallback when flood is all there is and the hole is shallow. On a deep blind bore a coolant-fed bar is not an upgrade. It is the tool.

Dead space stays at the bottom for the chip and for the insert radius. A square-bottom call is a grooving tool or a special, not an 80° diamond on the end of a 200 mm stick-out.

Boring heads on a mill: micrometric adjustment, balance, maximum RPM

A boring head on a machining centre is a micrometer that rotates. Vernier or dial: 0.01 mm on the diameter on a shop head, 0.002 mm on a fine one. The sequence is loosen, tick, lock, take a cut, measure, tick again. The first cut is a witness. The second cut is the size. Chasing the number on the first pass is how an H7 is overrun and the job becomes scrap.

Balance starts to matter once spindle speed climbs. An offset slide with an insert on one side is a lump. Fine at 800 rev/min on a 50 mm bore. Ugly at 4,000 on a 20 mm bore. Makers print an nmax for a reason: bearings, slide, clamp. Exceed it and the setting creeps, the head rings, and eventually something lets go. A second insert, opposed to the cutting one and doing no cutting, is a balance weight, not decoration.

A head is a fair choice for one hole. For a family of holes, a dedicated cartridge, or a rough drill plus a finishing head, is faster than a slide that has to be set twice a shift because someone bumped it.

ISO fits H7, g6, h6: reading a tolerance table and aiming at the right size

H is the hole that sits on the nominal as its lower limit. The 7 is the grade, the width of the band. A 50 H7 is 50.000 to 50.025 mm, roughly — the table for that diameter range is what gets read, not one memorised line. Shafts are lowercase. An h6 sits under the nominal, 50.000 down to 49.984 mm or so. A g6 is a little smaller still, for a sliding fit. H7/h6 is a locational clearance. H7/g6 slides more. H7/p6 is a press, and that shaft is not a boring job.

The aim is the middle of the hole band, not the nominal. On an H hole the nominal is the edge next to scrap. 50.012 mm on a 50 H7 leaves room for a warm part, a worn edge, and a gauge calibrated in another room. The 50 on the drawing is not the target. The target is the centre of the H7 band.

Target, band and gauge belong on the setup sheet as numbers. “Bore 50 H7” without a number is how three operators make three different sizes, all technically inside, each of them matching a different shaft.

Measuring: bore gauge, plug gauge, air gauge, and the effect of part temperature

A telescoping gauge plus a micrometer is a skill. A dial bore gauge, zeroed on a setting ring, is a process. A go/no-go plug is a gate: the go end passes through, the no-go end does not enter. It does not report 12 µm. An air gauge is a production tool — fast, a micron if the jet is clean — and useless when the bore is a taper that was never mapped.

Steel grows about 12 µm per metre per °C. A 50 mm bore, 10 °C warm from cutting, is 6 µm big while it is measured, and right in the morning. Aluminium is twice that. The measurement is taken at 20 °C, or a compensation is applied. A cold plug in a warm hole goes. A warm plug in a cold hole does not. Both people are sure the other cannot measure.

The bore gauge is zeroed on a ring that has sat next to the part, not on a micrometer held in a sweaty hand. The setting ring is the standard. The micrometer is a transfer, and every transfer leaks a micron. Beside a 50 H7, a band only from 50.000 to 50.025 mm, that leaked micron and the 6 µm of warmth are a real slice of the tolerance, not a footnote.

Cylindricity and taper: what three measurements at three depths show

One reading at the mouth is a rumour. Three depths — mouth, middle, bottom — and two directions, 0° and 90°, make a map. Six numbers.

  • Taper, smaller at the bottom — insert wearing, or the bar deflecting more as it reaches the far end, the classic pattern. Compensate, take a spring pass, or shorten the bar.
  • Taper, bigger at the bottom — the bar is following a drilled banana, or the headstock or the spindle is not square to the travel, or chips packed at the mouth and the tool cut free below them.
  • Oval (0° ≠ 90°) — clamp distortion, a thin wall, an unbalanced head, or a part that left the chuck oval and was bored round only at the mouth.

Cylindricity is the combination: the surface lying between two coaxial cylinders. A taper of 15 µm and an oval of 8 µm is not “about 15”. The six readings are reported, then the call. A drawing with a cylindricity of 0.01 mm and a 4 × D bore is a damped bar and a hone, not a 12 mm steel stick and a hopeful look.

Boring stainless and cast iron: opposite problems — work hardening versus abrasion

Austenitic stainless: a built-up edge*, work-hardening, stringy chips, a surface that looks torn if the edge rubs. Positive rake, a sharp edge, TiAlN or similar, feed high enough to get under the skin — 0.12 mm/rev is not aggressive here — Vc moderate, often 60–120 m/min on carbide, coolant at the nose. A dwell is forbidden. One spring pass, then stop.

Grey iron: graphite is a built-in chipbreaker, and the hard carbides and the sand in the casting skin are a built-in grinding paste. Short chips, abrasive flank wear, a dusty slideway. CVD-coated carbide or ceramic, a honed edge, dry or a little air, and Vc can run high. The wear is honest and slow. The finish is a dull grey, not a polish. Chasing Ra 0.4 with a steel-grade chipbreaker only notches the edge.

They feel like opposite shops. They are. The insert that is happy in 304 dies of abrasion in GJL-250. The K-grade that skins iron all week builds an edge and tears 316. ISO 513 is what keeps that lesson from having to be learned twice.

Reclaiming a worn bore: sleeving, weld build-up, repair tolerances

A worn bearing seat is rarely “just take a tenth and fit an oversize”. Either the bore is opened to a standard repair size and sleeved, or metal is added and bored back to nominal. Sleeving: a clean, concentric bore, a press or Loctite or a shrink, then the sleeve bored to the drawing. Bronze in a steel housing for a shaft; steel in aluminium for a thread or a bearing. Weld or spray build-up is for a housing that cannot be enlarged — engine blocks, a one-off — and it wants heat treatment, then a true bore, not a file.

Repair tolerances recreate the original fit, not “H8 because the part is old”. If the shaft is still h6, the hole is still H7, even when that H7 now lives in a sleeve. Concentricity to the rest of the part is the hidden specification: a sleeve that is round in the wrong place is a new vibration.

The wreck is measured before any cut. Minimum wall still left, the oval, the crack that may be there — those decide sleeve versus scrap. Boring cannot heal a split housing.

Stick-out is cubic: twenty millimetres of bar length versus a new grade

When the bore rings, the reach is often for a different insert. The geometry that moved is L. δ ∝ L³. 100 mm of stick-out against 80 mm is 100³/80³ ≈ 2.0. Twice the banana. Twenty millimetres more in the clamp, a shorter holder, a millimetre more of bar in the bush — a tool change done with an Allen key.

Grade, coating, chipbreaker: they change wear and the chip. They do not change 3EI. Extra money, if L cannot move, goes into a carbide shank or a damped bar. Extra time goes into a spring pass. It does not go into a “more expensive P10” on a steel bar humming at L/d = 6.

Raising spindle speed will not straighten a deflected bar. The diameter error this calculator prints comes from Fp, L, E and I. Vc is not in the formula. That absence is the proof.

Lead angle, rake and the radial force that bends the bar

Fp, the push-off*, is a slice of the cutting force. This page uses about 35% on roughing and 55% on finishing, because a light finishing cut on a nose radius is a more radial event. The entering angle decides where the rest goes. At 90°, the edge that cuts a square shoulder, most of the force runs along the bar, into the spindle, and the radial push is at its smallest. At 75° or 60° the chip thins, but the force tilts towards the wall and Fp grows. Boring bars are therefore set as close to 90° as the job allows, rarely below 75°. Positive rake drops the total force. A hone, or a negative land, raises it and buys edge strength.

When deflection is the scrap, the set is a positive, small-nose cartridge at 90° or close to it, a roughing pass deeper than the radius, then a light finish plus a spring pass. A sharp corner at the bottom of an 8 × D bore, a steel bar, and a cylindricity of 5 µm are three demands. Any two of them can be met. Not all three.

A threading bar inside a bore is this problem on a 60° point. Even more of the force is radial, and there is even less forgiveness.

How much stock to leave after the drill

Too little stock and the boring insert rubs on the work-hardened skin of the drill margin, following every wander. Too much, and a finishing bar is asked to rough. On a 30–50 mm hole, 0.8–1.5 mm on diameter for a rough boring pass, then 0.3–0.5 mm for the finish, is a sane band. Small bores need less in millimetres and more care. An 8 mm bore with 1 mm a side is a slotting cut, not a bar.

A U-drill or a twist drill that already holds 0.2 mm is a finish-bore candidate: one pass, a spring pass, done. A drilled hole that wandered 0.4 mm off axis needs enough stock for the bar to true it. ap has to bury the error, not kiss it. The bad hole is measured before the good one is programmed.

When to stop boring and send it to hone

Boring can deliver size. Honing delivers a straight, round, quiet bore with a cross-hatch that holds oil. A call for Ra 0.2, for a cylindricity of a few micrometres, or for a hydraulic tube, is already hone work. The stock left for the stones is 0.02–0.05 mm on diameter, even. “Just a tenth more” with a 0.2 mm nose at 6 × D puts a chatter spiral into the wall that no stone is glad to erase.

Engine cylinders, valve guides, a servo bore: a clean hole, slightly small, tapered the right way if it tapers at all, then a hone. The bar’s job ends when the axis is true and the stock is even. After that, a different trade.

Glossary

IT grade
The ISO step that sets how wide a size band may be. The 7 in H7 is that step: a smaller number is a tighter band. The letter, not the number, says whether the band starts on the nominal size.
Cylindricity
A form tolerance on the whole bore, not on one diameter. The surface has to lie between two cylinders that share an axis, so taper and oval both spend the same allowance.
Stick-out
The free length of bar beyond the holder, the L in L/d. The tip of that cantilever bends with the cube of L, which is why a short extra bit of bar costs more size than it looks.
Spring pass
A second pass at the same tool offset, with no fresh depth of cut, or with only a trace of feed. Cutting force falls, the bar springs back towards the wall, and the edge takes the skin the deflected pass left behind.
Nose radius
The rounded corner of the insert, written rε. When the depth of cut is smaller than this radius the wall is touched only by the curve, and the force on the bar turns more radial.
Regenerative chatter
Vibration that feeds on itself: each revolution cuts the wavy surface left by the one before, and the wave grows. In a bore the mark is a helix whose spacing is not the feed, because the bar’s own note sets it.
Built-up edge
Workpiece metal stuck to the tool tip, often called BUE, so the edge doing the cutting is no longer the insert that was fitted. On austenitic stainless it appears when the edge rubs, and the wall looks torn.
Push-off
The radial slice of the cutting force, Fp, that bends a boring bar away from the wall so the bore measures small. On this page that slice is taken as about 35% of the cutting force in roughing and about 55% in finishing.

Related calculators