Boring bars are the lathe tool that enlarges and finishes a hole that's already there. Drill it first, bore it second — that's the standard sequence when you need a hole that's bigger, straighter, rounder or more accurately positioned than a drill bit can produce on its own. Done well, a boring bar can hold a hole within a thou or two of a target diameter and produce a surface finish that drills can't touch.
Done badly, boring bars chatter, deflect, walk off centre and produce holes that look like a corkscrew on the inside. Most of what separates the two is setup: the right bar diameter for the job, the right insert geometry, the right centre height, and an honest assessment of how much stick-out you're getting away with.
This guide covers the boring bar families (indexable, brazed, solid carbide, anti-vibration), how to read the ISO designation code stamped on the shank, the insert geometry decision (CCMT vs DCMT vs TPMT), the L:D ratio rule that prevents 80% of chatter, centre-height setup, speeds and feeds, materials, and the Seco and Maxigear range stocked at AIMS for Australian workshops.
What is a boring bar and what is it used for
A boring bar is a single-point cutting tool used on a lathe to enlarge and finish an existing hole. The bar is held in a tool post or turret, fed into the workpiece (which is rotating in the chuck), and cuts material from the inside surface of the hole as it advances. Unlike a drill, which produces a hole by removing a cylinder of material from solid stock, a boring bar enlarges a hole that's already been drilled, cast, forged or punched.
The five common applications:
- Sizing a hole accurately — drills produce holes that are typically 0.05–0.2 mm oversize and rarely concentric with the spindle axis. A boring bar can hold ±0.01 mm and runs true to spindle centreline.
- Producing non-standard hole sizes — there's no drill bit for a 27.5 mm hole, but you can drill 26 mm and bore to 27.5 mm.
- Improving surface finish — drilled holes have a rough surface (Ra 3.2–6.3 µm typical). A boring bar can produce Ra 0.8–1.6 µm or better with the right insert.
- Boring castings and forgings — when there's no drilled hole to start with, just a cast bore or rough forged opening, boring is the only practical way to bring it to size.
- Tapered and stepped bores — a boring bar with the compound slide can produce a precise taper. Multiple cuts at different depths produce stepped bores for shaft/bearing fits.
Boring vs drilling vs reaming — what each operation actually does
Three operations that all enlarge a hole. They do different things and they're not interchangeable.
| Operation | Produces | Tolerance | Surface finish | When to use |
|---|---|---|---|---|
| Drilling | A hole from solid stock | ±0.05–0.2 mm typical | Ra 3.2–6.3 µm | First operation — getting the hole started |
| Boring | An enlarged, more accurate hole | ±0.01 mm achievable | Ra 0.8–1.6 µm typical | When you need accuracy, concentricity or non-standard size |
| Reaming | A hole at exact reamer diameter | H7 / H8 standard | Ra 0.4–1.6 µm | Finishing a hole to a precise standard size after drilling or boring |
The standard sequence for a precision hole on a lathe is: drill → bore → ream. Drill to ~0.5 mm undersize. Bore to within ~0.1 mm of finish size to take out drill error and centre the hole on the spindle axis. Ream to the final precise size.
For a deeper dive into when each tool is right, see our Reamer Guide for finishing operations and Choosing the Right Drill Bit for the hole-starting step.
Boring bar vs boring head — the lathe vs mill distinction
The terminology trips beginners up constantly. The two tools do the same job — boring an internal hole — on different machines.
| Boring bar | Boring head | |
|---|---|---|
| Machine | Lathe (workpiece rotates) | Mill or drill press (tool rotates) |
| Form factor | Long bar with cutting tip at one end, held in lathe tool post | Compact adjustable head with a slide carrying a small cutting bar; mounts in mill spindle via R8/CAT/BT/Morse taper |
| Adjustment | Cross-slide of the lathe controls the bore diameter | Built-in graduated dial on the head adjusts the cutter offset |
| Cutter | Insert (or brazed tip) at the end of the bar itself | Small boring bar inserted radially into the head |
| Best for | Through bores, blind bores, tapered bores, precise sizing on lathe | Boring on parts that can't be turned (large/awkward) on the mill, drill press or VMC spindle |
A boring HEAD uses small boring bars (or boring tools) — the tool slides into the head, and the head adjusts the cutter offset from the spindle axis. A boring BAR is the cutting tool on a lathe, where the workpiece rotates and the bar stays still.
This guide is about boring bars — lathe operation. For mill spindle work, you'd reach for a boring head with smaller boring tools mounted in it; the principles below (insert geometry, centre height, L:D ratio, chatter control) all transfer, but the holder is different.
Indexable, brazed and solid carbide — three eras of boring bar tech
Boring bars come in three fundamental constructions, reflecting three generations of cutting-tool technology.
| Indexable insert bars | Brazed-tip bars | Solid carbide bars | |
|---|---|---|---|
| Construction | Steel shank with replaceable carbide insert clamped or screwed in | HSS or steel shank with carbide tip brazed to one end | Single piece of solid carbide, ground to shape |
| Replacement | Replace the insert (cents to dollars) when worn | Re-grind the brazed tip, or replace the whole bar | Re-grind only by specialist; usually replaced |
| Cost (per bar) | $50–$500 holder + $5–$30 per insert | $15–$100 each | $200–$2,000+ |
| Stiffness (Young's modulus) | Steel shank: ~210 GPa | Steel shank: ~210 GPa | Tungsten carbide: ~600 GPa (3× steel) |
| Max practical L:D ratio | 4:1 (steel shank) | 4:1 (steel shank) | 8:1 (carbide shank) |
| Best for | Production work, repeatability, common bore sizes | Hobby use, one-offs, custom geometries, light cuts | Long stick-out, hard-to-reach bores, vibration-sensitive work |
| AIMS supply | Seco range — 391 products in indexable turning toolholders | Maxigear Double End Boring Bar set (6 sizes) | Sourced on request — Sandvik, Iscar, Mitsubishi premium |
For commercial workshop work, indexable insert bars dominate. Replace the insert in 30 seconds when it wears, no re-grind, predictable performance from one insert to the next. Brazed-tip bars survive in hobby and one-off use because they're cheap and easy to re-grind for a custom geometry. Solid carbide is the answer when stick-out is unavoidable and chatter must be eliminated — three times the stiffness of a steel bar means twice the practical reach.
Boring bar anatomy
An indexable boring bar has six functional features:
- Shank — the cylindrical (or with flats) main body, sized to fit a standard tool holder. Common AU sizes: 8, 10, 12, 16, 20, 25, 32 mm. Imperial: 3/8", 1/2", 5/8", 3/4", 1", 1-1/4".
- Head — the cutting end that carries the insert pocket. Reduced diameter compared to the shank to fit inside the bore.
- Insert pocket — the seat that locates the insert. Geometry of the pocket determines what insert shape will fit.
- Lock system — how the insert is secured. Screw lock (most common), pin lock (Seco), clamp lock, multiple lock. Determines insert change speed and rigidity.
- Coolant outlet (optional) — for coolant-through bars, an outlet at the head delivers coolant to the cutting edge. Critical for blind hole boring.
- Lead angle / approach angle — the angle the cutting edge makes with the bar axis. 90° is dominant for general boring; 95° gives slightly stronger insert support; 91–93° is the typical "negative rake" geometry.
Reading the ISO designation code
Every indexable boring bar has a stamped designation that decodes the bar's specifications. The ISO 5610 code looks intimidating but breaks into 7 characters that each mean something specific.
Example: S20R-SCLCR12 on a Seco bar.
| Position | Code | Meaning |
|---|---|---|
| 1 | S | Shank type — S = solid steel; A = steel with carbide insert pocket; E = solid carbide; F = solid steel for adapters |
| 2–3 | 20 | Shank diameter in mm — 20 mm here. (06 = 6 mm; 25 = 25 mm; 32 = 32 mm) |
| 4 | R | Shank length in mm divided by 25 — R = 200 mm length. Lengths: M=125, N=150, P=170, Q=180, R=200, S=250, T=300 |
| 5 | S | Insert clamping system — S = screw clamp; M = multiple clamping; P = pin lock; D = clamp on top |
| 6 | C | Insert shape — C = 80° rhombic (CCMT); D = 55° rhombic (DCMT); T = triangle (TCMT/TPMT); V = 35° rhombic (VCMT); W = trigon (WNMG) |
| 7 | L | Insert clearance angle — L = 0°; A = 3°; B = 5°; etc. |
| 8 | C | Tool style — direction of approach |
| 9 | R | Cutting direction — R = right hand; L = left hand; N = neutral |
| 10–11 | 12 | Insert size code — 12 mm cutting edge |
So S20R-SCLCR12 = 20 mm solid steel shank, 200 mm long, screw-clamp, CCMT insert (80° rhombic, 0° clearance), right-hand cutting, 12 mm insert. That's a typical mid-size general-purpose internal turning toolholder.
Knowing the code is non-negotiable for ordering — supplier websites are organised by it. Get one digit wrong and you'll receive a bar that won't accept your inserts.
Insert geometry by application
The insert is the actual cutting edge — the consumable that wears. Pick the wrong geometry and even a perfect bar will perform badly. The 7 common shapes:
| Insert | Shape | Edge angle | Cutting edges | Best for | Min bore typical |
|---|---|---|---|---|---|
| CCMT | 80° rhombic | 80° | 2 (positive rake) | General-purpose boring, finishing | ~10–12 mm on 6 mm shank |
| CCGT / CPMT | 80° rhombic, ground | 80° | 2 (positive rake, sharp) | Aluminium, copper, finish boring | Smaller — to ~8 mm |
| DCMT | 55° rhombic | 55° | 2 (positive rake) | Profiling, contouring, smaller bores | Smaller than CCMT — sharper point |
| TCMT | Triangle (60°) | 60° | 3 (positive rake) | Roughing, deeper cuts, more economical (3 edges) | ~12 mm on small shank |
| TPMT | Triangle (60°), positive geom | 60° | 3 (positive rake, sharp) | Smaller bores than TCMT, lighter cuts | ~10 mm on small shank |
| VCMT / VBMT | 35° rhombic | 35° | 2 (positive rake) | Tight-radius profile boring, contouring | Sharp point — small radius work |
| WNMG | Trigon | 80° | 6 (negative rake) | Heavy roughing, larger bores, economy (6 edges) | Larger bores only — ~25 mm+ |
For Australian general workshop use, the standard kit is:
- CCMT for general boring — most versatile, two edges per insert, 80° provides good balance of strength and access
- DCMT for tight bores and profiling — 55° narrower point gives clearance for radii and steps
- TPMT for very small bores — when you need to bore down to 10 mm or below
Sizing the bar — diameter and L:D ratio
The single most important rule in boring: biggest diameter that fits, shortest stick-out you can manage. Rigidity of a cantilevered bar scales as diameter to the fourth power, divided by length cubed. Every millimetre of extra stick-out costs disproportionately.
The L:D ratio (length-to-diameter ratio) is the practical chatter-prevention rule:
| Bar construction | Max L:D ratio | Practical reach (e.g. for 16 mm bar) |
|---|---|---|
| Steel shank (indexable or brazed) | 4:1 | 64 mm stick-out |
| Heavy-metal shank (tungsten alloy) | 6:1 | 96 mm stick-out |
| Solid carbide shank | 8:1 | 128 mm stick-out |
| Anti-vibration / dampened | 10–14:1 | 160–224 mm stick-out |
Beyond these ratios you're guaranteed chatter regardless of skill. Below, you have a fighting chance — with correct centre height, sharp insert, appropriate cutting parameters and good workholding rigidity.
Every increase in diameter buys you disproportionate rigidity. A 25 mm bar at 100 mm stick-out is dramatically more stable than a 16 mm bar at 64 mm stick-out, even though both are at the same 4:1 ratio.
Minimum bore diameter — what each combo can actually do
The minimum bore a tool can produce is determined by the bar shank diameter PLUS the insert clearance to the wall PLUS the insert nose radius and clearance. Manufacturers publish minimum bore data per holder — but the rules of thumb:
| Shank diameter | Min bore — CCMT (typical) | Min bore — CPMT/TPMT (positive geom) |
|---|---|---|
| 6 mm | ~10 mm | ~8 mm |
| 8 mm | ~12 mm | ~10 mm |
| 10 mm | ~14 mm | ~12 mm |
| 12 mm | ~16 mm | ~14 mm |
| 16 mm | ~22 mm | ~18 mm |
| 20 mm | ~27 mm | ~24 mm |
| 25 mm | ~33 mm | ~30 mm |
| 32 mm | ~42 mm | ~38 mm |
For bores below 10 mm, you're outside indexable territory — solid carbide micro boring bars or specialised brazed-tip tools take over. AIMS sources Sandvik CoroBore and equivalent micro-boring tools on request.
Centre height setup and parallel alignment
The single most common boring bar setup mistake is incorrect centre height. The cutting edge of the insert must sit on the workpiece centreline — not above, not below — for a standard general-purpose setup.
The standard procedure:
- Measure tailstock centre height first. Bring up a known accurate centre in the tailstock. Use a 6" rule held vertically against the tailstock centre and the cutting edge of the boring bar. They should align exactly.
- Use a height gauge or shim stack. Workshop technique: place the insert tip against a small bubble level on top of the workpiece. Adjust shims under the bar until the level reads dead centre.
- For QCTP holders: use the height-adjustment knob. The bar position is repeatable once set.
- For lantern post / 4-way: use a packer / shim stack under the bar. Slow but accurate.
- Verify with a test cut. Take a light cut on a test piece. Measure the bore. If the surface finish is rough or the dimensions don't match the dial, recheck centre height.
Parallel alignment — the bar must be parallel to the lathe bed (Z-axis), not skewed. Misalignment causes the cutter to dig in deeper as it advances, producing a tapered bore. Check by traversing the bar along the bed without engaging cut and watching for any change in the gap between bar and workpiece.
Speeds, feeds and depth of cut for boring
Boring speeds and feeds follow the same fundamentals as external turning, but with two adjustments: lower speeds (typically 70–80% of external turning) and lighter depth of cut.
| Material | Cutting speed (Vc, m/min) | Feed (mm/rev) | DOC (depth per side) |
|---|---|---|---|
| Mild steel (1018, 1020) | 120–180 | 0.10–0.20 | 0.5–1.5 mm rough; 0.05–0.20 mm finish |
| Free-machining steel (12L14) | 180–250 | 0.10–0.25 | 0.5–2.0 mm |
| Alloy steel (4140, 4340) | 80–120 | 0.10–0.20 | 0.5–1.0 mm |
| Stainless 304/316 | 50–90 | 0.10–0.18 | 0.5–1.0 mm — heavier feed cures work-hardening |
| Aluminium 6061 | 200–500 | 0.10–0.30 | 0.5–2.0 mm |
| Brass / bronze | 150–250 | 0.10–0.20 | 0.5–1.5 mm |
| Cast iron (grey) | 80–130 | 0.10–0.30 | 0.5–1.5 mm — dry cutting fine |
| Tool steel (annealed) | 40–80 | 0.05–0.15 | 0.3–0.8 mm |
Convert Vc to spindle RPM using the formula N = (1000 × Vc) ÷ (π × D), where D is the bore diameter in mm. For the full RPM derivation, worked examples and CSS / G96 considerations, see our Lathe RPM Formula Guide. For broader cutting speed and feed reference across milling, drilling and turning, the Cutting Speeds & Feeds Chart covers the wider context.
Light-machine modification: on hobby and small bench lathes (Optimum, Sieg, Boxford), reduce the depth of cut to 0.1–0.3 mm per side and increase feed slightly. Light DOC + faster feed is the classic chatter-prevention combination.
Chatter control — six fixes ranked
Chatter — the high-pitched ringing sound and ribbed surface finish that haunts every machinist. The cause is always the same: the system (bar + holder + workpiece + machine) has insufficient dynamic stiffness for the cutting force, and starts oscillating at its natural frequency. The fixes, ranked by what to try first:
- Reduce stick-out. The single highest-leverage fix. Halving the stick-out increases rigidity by 8×. Re-mount the bar to put the holder closer to the work face if at all possible.
- Use a bigger diameter bar. Doubling the bar diameter increases rigidity by 16×. If a 12 mm bar is chattering and a 20 mm fits, swap immediately.
- Switch to solid carbide. Carbide is 3× the Young's modulus of steel — equivalent to a steel bar of larger diameter. The Practical Machinist consensus on solid carbide is "night and day" for chatter on long reaches.
- Reduce the depth of cut, increase the feed. Lighter cut means less force; faster feed means the chip is thicker (better breaking) and the cutting edge spends less time per revolution under load. Counter-intuitive but works.
- Sharpen / replace the insert. A worn or dull insert generates higher cutting forces. Many "chatter problems" are actually "the insert needs replacing." Hone the cutting edge for stainless work — fresh inserts come with a tiny edge prep that helps prevent built-up edge but can chatter on light cuts.
- Increase positive rake / change geometry. Switch from CCMT (neutral) to CPMT (positive rake) — sharper, lighter cutting force. For aluminium, use polished aluminium-specific inserts.
If you've exhausted the six fixes and chatter persists, you've hit the limit of an unaided steel bar. Either redesign the part to allow a shorter setup, or move to anti-vibration / dampened bars (Sandvik Silent Tools, Kennametal Romicron) — these have an internal mass-spring-damper that absorbs vibration energy and can run 10:1+ L:D ratios. AIMS sources these on request — premium pricing ($800–$3,000+ per bar) but transformative on long-reach work.
Chip evacuation, coolant-through and blind hole strategy
Boring is fundamentally limited by chip evacuation. Unlike external turning where chips fall away under gravity, internal turning has nowhere for chips to go except back along the bar — past the cutting edge, where they can re-cut, weld to the insert, or jam between the bar and bore wall.
The evacuation rules:
- Through-hole boring — chips can be pushed out the back. Use a helical chip-breaking insert geometry and feed in continuously. This is the easy case.
- Blind-hole boring — chips have nowhere to go. They pile up at the bottom, then re-cut into the next pass. The standard fixes: peck-feed (back the bar out periodically to clear chips), high-pressure coolant (typically 30+ bar to flush chips out), or coolant-through bars with the outlet directing flow back along the bar to push chips up.
- Stainless and titanium — these materials produce stringy chips that wrap around the bar. Use a chipbreaker insert geometry (M, MM, MR breakers) and step the cuts to force chip breaks. Run with flooded coolant.
- Aluminium — chips can weld to the insert (built-up edge). Use polished, sharp ground geometry (CPMT/CCGT — the "GT" indicates a polished aluminium-specific edge). Kerosene or aluminium-specific cutting fluid.
Coolant-through bars deliver coolant through internal passages to the cutting edge — the gold standard for blind-hole work. Worth the premium when you're doing repeat blind-hole production. AIMS Seco range includes coolant-through variants on request.
For the broader cutting fluid selection by material, see our Cutting Fluids Guide.
Boring different materials
Each material has its own boring strategy. The five common ones:
Mild steel — the easy case. CCMT general-purpose insert, standard speeds and feeds, soluble oil flood. Chips break cleanly, bar runs predictably. This is what indexable boring bars were designed for.
Stainless 304/316 — the hardest common material. Work-hardens in seconds, demands continuous cutting (no peck-feeding), heavy feed to keep cutting under the work-hardened layer, sharp inserts (hone the edge before first cut), heavy sulphurised coolant. Switch to CPMT positive geometry; the standard CCMT will smear instead of cut. Solid carbide bars give substantial improvement.
Aluminium 6061 / 2011 — runs fast (200–500 m/min Vc), but chip welding is the failure mode. Polished aluminium-specific insert (CCGT/CPMT with polished face), kerosene flood. Chips build up if speeds are too low, so push the RPM as high as the lathe allows.
Cast iron (grey) — runs dry. CCMT or WNMG insert. Cast iron produces a powdery chip rather than continuous swarf, which makes chip evacuation a non-issue but a cleanup nightmare. Use a vacuum or air blast rather than coolant flood.
Hardened steel (above 45 HRC) — outside standard carbide insert territory. Use CBN (cubic boron nitride) inserts or specialty hard-turning grades. AIMS sources Seco hard-turning inserts on request. Standard CCMT/DCMT inserts will fail in seconds on hardened material.
AIMS Seco and Maxigear range
AIMS stocks two tiers of boring tooling:
Seco Internal Turning Toolholders — the production / commercial tier. Comprehensive range covering shank sizes from S04 (4 mm) through A32 (32 mm), in steel-shank construction, with multiple lock systems (Multiple Lock for heavy roughing, Pin Lock for production speed, Screw Lock for general use, Clamp Lock for high-grip). Insert geometries include T (triangle), C (80° rhombic), D (55° rhombic), V (35° rhombic). Both left-hand and right-hand variants. Duratomic-coated inserts available.
Total range: part of the indexable turning tool holders collection (391 products covering both internal and external turning). Pricing typically $200–$465 per holder.
Maxigear Double End Boring Bar With Holder — the hobby / one-off tier. Traditional brazed-tip boring bar with a versatile double-ended head, sized 3/8" through 1-3/16". Strong supply for occasional or one-off work where the cost of a Seco indexable bar isn't justified. Six size variants from $30 to $110.
Inserts — AIMS stocks 838 turning inserts in the turning inserts collection, covering all common ISO geometries (CCMT, DCMT, TCMT, TPMT, VCMT, CPMT, WNMG) with various coatings and grades for steel, stainless, aluminium and cast iron applications.
Lathe HSS tool bits — for traditional grind-your-own boring tool work, the lathe tool bits collection stocks 15 HSS bit options.
Premium tier on order: Sandvik (CoroBore, Silent Tools), Kennametal (Romicron anti-vibration), Iscar Cham-IQ, Mitsubishi solid carbide micro-boring. Sourced via AIMS on request — typical lead time 5–10 working days.
Need help selecting the right bar and insert combination for your application? Browse the Seco indexable turning toolholder range, the turning inserts collection, or contact the AIMS team on (02) 9773 0122 — happy to talk through bore size, material and stick-out for your job.
Common boring bar mistakes
| Mistake | Result | Fix |
|---|---|---|
| Smallest bar that fits | Excess deflection, chatter, poor finish | Use the biggest diameter that fits — every mm of diameter matters |
| Stick-out too long | Chatter, taper in bore, poor finish | Mount holder closer to work; reduce stick-out to 4:1 (steel) / 8:1 (carbide) |
| Wrong centre height | Below centre = digs in, chatters; above centre on a normal cut = poor finish | Set on centre exactly using tailstock centre as reference (or 0.1–0.3 mm above for long reaches) |
| Bar not parallel to bed | Tapered bore | Square the bar to the spindle axis before cutting |
| Wrong insert for material | Smearing (stainless), built-up edge (aluminium), chipping (hardened) | Match insert geometry and grade to material |
| Worn insert pushed beyond service life | Chatter, oversize bores, poor finish, broken edges | Index or replace at first sign of wear — they're consumables |
| Pre-drill same size as target bore | Skim cut, no material to actually engage, chatter | Pre-drill at least 0.5–1 mm undersize to leave material for the boring bar to cut |
| Skipping spring cuts at finish | Bore comes out 0.02–0.05 mm under target | At final dimension, run a second pass without changing the dial — cuts the spring-back |
| Chips not evacuating in blind hole | Re-cutting, broken inserts, jammed bar | Peck-feed, high-pressure coolant, or coolant-through bar |
| Loose toolholder or workpiece | Chatter independent of bar setup | Verify QCTP locked, workpiece firmly chucked, no daylight in setup |
Frequently Asked Questions
What is a boring bar and what is it used for?
A boring bar is a single-point cutting tool used on a lathe to enlarge and finish an existing hole. It's used to size a hole accurately (±0.01 mm achievable), produce non-standard hole sizes (e.g. a 27.5 mm hole that no drill bit makes), improve surface finish on drilled holes, bore castings and forgings that have no pre-drilled hole, and produce tapered or stepped bores. The standard sequence for a precision lathe-bored hole is drill → bore → ream.
What's the difference between a boring bar and a boring head?
A boring bar is the cutting tool used on a lathe — workpiece rotates, tool stays still. A boring head is an adjustable holder used on a mill or drill press — tool rotates, workpiece stays still. Boring heads contain small boring bars (sometimes called boring tools) that are inserted radially. The cutter offset on a head is adjusted via a graduated dial; on a lathe, the cross-slide controls the bore diameter. The cutting principles are identical but the tool form factor and the machine are different.
What's the difference between boring, drilling, and reaming?
Drilling makes a hole from solid stock, with typical tolerance of ±0.05 to ±0.2 mm. Boring enlarges an existing hole to high accuracy (±0.01 mm achievable) using a single-point cutting tool. Reaming finishes a hole to an exact reamer diameter, typically H7 or H8 standard, with surface finish Ra 0.4–1.6 µm. The standard precision-hole sequence on a lathe is drill (rough hole) → bore (accuracy and concentricity) → ream (final size and finish).
How do I read a boring bar designation code like S20R-SCLCR12?
The ISO 5610 code breaks down: S = solid steel shank, 20 = 20 mm shank diameter, R = 200 mm shank length (M=125, N=150, P=170, Q=180, R=200, S=250, T=300), S = screw clamp, C = CCMT 80° rhombic insert shape, L = 0° insert clearance, C = tool style, R = right-hand cutting, 12 = 12 mm insert size code. So S20R-SCLCR12 is a 20 mm steel shank, 200 mm long, screw-clamped CCMT-style right-hand boring bar for 12 mm inserts.
What's the maximum stick-out I can have on a boring bar?
The L:D ratio (length-to-diameter) rule: 4:1 maximum for steel shanks, 6:1 for heavy-metal (tungsten alloy) shanks, 8:1 for solid carbide shanks, 10–14:1 for anti-vibration / dampened bars. So a 16 mm steel bar can stick out 64 mm before chatter is guaranteed, while the same bar in solid carbide can reach 128 mm. Beyond these ratios you're guaranteed chatter regardless of skill or technique. Below them you have a fighting chance with correct setup.
What insert should I use — CCMT vs DCMT vs TPMT?
CCMT (80° rhombic) is the general-purpose default — most versatile, two cutting edges, good balance of strength and access for typical bores. DCMT (55° rhombic) has a sharper point, better for tight radius profiling and steps. TCMT (60° triangle) gives three edges for economy on roughing. TPMT is the positive-geometry version of TCMT — sharper, lighter cutting force, smaller minimum bore than TCMT. CPMT and CCGT are the polished, ground versions of CCMT for aluminium and finish work. Standard kit: CCMT for general boring, DCMT for tight bores, TPMT or CPMT when you need to bore down to ~10 mm or smaller.
What's the minimum bore diameter I can achieve?
Depends on shank diameter and insert geometry. Rough rules of thumb: 6 mm shank with CCMT — about 10 mm minimum bore; 12 mm shank with CCMT — about 16 mm; 20 mm shank — about 27 mm; 32 mm shank — about 42 mm. Switch to PMT-style positive-geometry inserts (TPMT, DPMT, CPMT) on the same shank for ~15–20% smaller minimum bore due to extra clearance. For bores below 10 mm, you need solid carbide micro-boring bars rather than indexable.
What RPM and feed should I use when boring?
Use the same surface-speed (Vc) values as external turning, then drop 20–30% for the lighter setup of internal work. Mild steel: Vc 120–180 m/min, feed 0.10–0.20 mm/rev. Stainless 304/316: Vc 50–90 m/min, feed 0.10–0.18 mm/rev (heavier feed to cut under work-hardening). Aluminium 6061: Vc 200–500 m/min, feed 0.10–0.30 mm/rev. Convert to RPM with N = (1000 × Vc) ÷ (π × D). On hobby/light machines, drop the depth of cut to 0.1–0.3 mm per side.
How do I set the boring bar at the correct centre height?
The cutting edge of the insert must sit on the workpiece centreline (spindle axis). Use a tailstock centre as a reference — bring it up, hold a 6" rule vertically against the centre and the cutting edge, they should align exactly. For QCTP holders, use the height-adjustment knob; for lantern-post or 4-way, use shims under the bar. Verify with a test cut. For long stick-outs where chatter is a problem, set the bar 0.1–0.3 mm ABOVE centre — when the cutting force deflects the bar downward, the cut becomes lighter rather than digging in deeper.
Why is my boring bar chattering and how do I fix it?
Six fixes ranked by what to try first: reduce stick-out (halving stick-out gives 8× the rigidity); use a bigger diameter bar (doubling diameter gives 16× rigidity); switch to solid carbide (3× stiffness of steel); reduce depth of cut and increase feed (lighter, faster cuts have less time under load per revolution); replace the insert (worn inserts cause higher cutting forces); switch to positive-rake geometry (CCMT to CPMT) for sharper cutting. The cheap counterintuitive trick: loosen all but the front set screw on the toolholder block — the bar can self-damp slightly. Forum-validated as "100% fixed" in stubborn cases.
When should I switch from a steel boring bar to solid carbide?
When the L:D ratio of your job exceeds 4:1 (or you're getting chatter at lower ratios that you can't fix any other way). Solid carbide has 3× the Young's modulus of steel — equivalent to a steel bar of ~1.4× the diameter. Practical Machinist consensus on the upgrade is "night and day" for chatter on long reaches. The cost is significant — a 25 mm solid carbide bar runs $400–$800 versus $50–$200 for a steel equivalent — but it's transformative when stick-out is unavoidable.
What is an anti-vibration / dampened boring bar and when do I need one?
Anti-vibration bars (Sandvik Silent Tools, Kennametal Romicron, Iscar Cham-IQ) have an internal mass-spring-damper system that absorbs vibration energy as the bar tries to oscillate. Allows L:D ratios of 10–14:1 versus 4:1 steel and 8:1 carbide. When you need them: deep blind bores beyond 4× bar diameter, very long-reach line boring, hard-to-reach internal features. Premium pricing ($800–$3,000+ per bar). AIMS sources these on request — typical lead time 5–10 working days.
Can I use a boring bar without coolant?
For cast iron and brass, dry boring is fine and standard practice. For steel, soluble-oil flood coolant is highly recommended — keeps the cutting edge cool, flushes chips, prevents work-hardening on the bore wall. For stainless 304/316, heavy sulphurised coolant is mandatory — dry stainless boring causes immediate work-hardening and insert smearing. For aluminium, kerosene or aluminium-specific cutting fluid prevents chip welding to the insert. For blind holes in any material, coolant flow is critical for chip evacuation, ideally via a coolant-through bar.
How do I bore stainless steel without work-hardening?
Five rules: slow RPM (Vc 50–90 m/min), heavy feed (0.10–0.18 mm/rev — light feed lets stainless harden faster than you can cut it), sharp insert with honed edge, heavy sulphurised cutting oil flooded, no peck-feeding (continuous cut keeps cutting under the hardened layer). Switch to CPMT positive-geometry insert rather than CCMT — sharper edge cuts cleanly through the work-hardened surface. Solid carbide bar gives noticeable improvement on long reaches because the lighter chatter prevents the work-hardening cycle from compounding.
How do I take a finish pass to hit a precise bore diameter?
The "spring cut" technique: at final dimension on the cross-slide dial, run a second pass without changing the dial setting. Tool deflection on the first pass leaves the bore slightly undersize from the dial reading; the spring cut lets the tool re-engage at the same depth setting and remove the spring-back. For very precise bores (±0.01 mm), measure between passes with telescopic gauges and a micrometer, or with a dial bore gauge — see our Bore Gauge Types Guide for measurement options. Aim for the lower limit of your tolerance band on roughing, then walk to nominal with light spring cuts.
