How to Choose a Tool for Interior Holes: 5 Checks Before You Cut
Interior holes are machined semi-closed. You cannot see the chips leave, and the bar is long and thin. This guide shows how to pick a tool for interior holes by length-to-diameter ratio, diameter range, tolerance and surface finish, and when boring should stop and reaming or interpolation should take over.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
Why a tool for interior holes behaves differently
An interior hole is cut in a semi-closed state. The tool enters from one side, the chips have to travel back along the same path, and nobody can watch the cutting edge. On an outside profile a bad insert shows up as a mark you can see from the aisle. Inside a Ø30 mm hole, 180 mm deep, the first visible sign of trouble is usually a chirp in the sound or a size drift on the gauge.
The second difference is stiffness. A boring bar is a cantilever. Every extra 10 mm of overhang adds deflection faster than the bar diameter can compensate for it. That is why the length-to-diameter ratio, not the insert grade, is the first number to check when you choose a tool for interior holes.
The third difference is chip removal. A blind hole leaves the tool sitting in a pile of chips at the bottom, and re-cutting turns them into a fine powder that packs the flutes. Deep holes in aluminium and low-carbon steel need either through-spindle coolant above 20 bar, or a retract cycle that lifts the tool clear every 1–2 mm of feed at the bottom of the cut. Neither option is free. Both are cheaper than scrapping a part at the final bore.
So the choice is never one tool. It is a short sequence: drill or helical-plunge to open the hole, then bore, ream or interpolate based on the tolerance band and the depth you actually need.
Length-to-diameter ratio: the first cut-off
Measure the real overhang: the distance from the spindle nose or holder face to the tip of the cutting edge, not the length of the hole. A Ø20 mm bar hanging 60 mm out sits at 3:1 and will bore cleanly in steel. The same bar at 140 mm is 7:1, and chatter becomes the limiting factor before tool life is.
A practical working band for steel and stainless: keep L/D under 4:1 for a standard steel boring bar, and under 3:1 if you are chasing Ra 0.8 μm or better. Tungsten carbide bars with a heavy shank extend that to roughly 6:1, and tuned anti-vibration bars with a built-in damper can reach 8:1 to 10:1. Those bars cost more and need a dialled-in speed. They do not fix a weak setup.
In aluminium and brass the bar is stiffer relative to the cut, so 6:1 is often workable with carbide and a modest depth of cut. In titanium and Inconel the same ratio will burn the insert, because the material pushes back harder and the bar has no margin left to absorb it.
If the ratio goes past what the bar can hold, do not buy a longer bar. Change the operation: helical interpolation with a smaller end mill spreads the load and shortens the overhang, or you can open the hole from both ends on a mill-turn center.
Matching the boring, reaming and interpolation routes
Drilling gets you a hole. It does not get you a tolerance. A twist drill in steel typically lands within IT12–IT13 and often wanders 0.05–0.15 mm off position over a deep hole. That is a starting point, not a finished feature.
Reaming is the fast route to a round, on-size hole: IT7 is normal, IT6 with a good floating holder and a rigid setup. Reamers cut on the chamfer only, so they straighten a slightly bent hole but they cannot correct position. Leave 0.1–0.3 mm of radial stock for a hand reamer and about 1 percent of the diameter for a machine reamer.
Fine boring is the route when you need both position and size, and it lets you correct the hole in one or two passes without changing tools. With a rigid setup we hold ±0.005 mm on bore diameters and Ra 0.8–1.6 μm as a standard machined finish, down to Ra 0.2–0.8 μm when the bore is finished with a wiper insert and a light spring pass.
Interpolation sits between them. It is slower than reaming but it handles odd diameters, interrupted bores and stepped holes with one tool, and it lets you dial the size in by adjusting cutter compensation. Choose it when the hole count is low or the diameter changes between parts.
Setup mistakes that show up as a bad bore
Runout is the quiet one. A reamer held 0.02 mm off centre cuts oversize on one side and undersize on the other, and the hole looks acceptable on a plug gauge while failing on a roundness check. Indicate every boring and reaming tool within 0.01 mm TIR, and re-check after a tool change.
Chip packing is the loud one. In blind holes, chips collect at the bottom and the bar starts rubbing instead of cutting. Add a retract cycle, increase coolant pressure, or switch to a tool with internal coolant holes. In aluminium, a polished flute and a higher helix angle help the chip leave without smearing.
Thermal drift is the slow one. A production run of 200 bores will grow 0.01–0.02 mm across the first hour as the spindle and part warm up. Cut three warm-up parts, gauge them, and only then lock the offset. If the tolerance is tight, keep a gauge on the machine and check every 20 parts.
Tool wear is the expensive one. A worn boring insert cuts undersize, so the operator nudges the offset, and the next fresh insert cuts oversize. Log the offset change per insert and replace on a count, not on a hunch.
Step by step: choosing and running the tool
Five steps from drawing to first good bore
- 11. Read the drawing for the real requirementWrite down diameter, depth, tolerance class, surface finish and position tolerance. A Ø12 H7 hole 40 mm deep and a Ø12 clearance hole 40 mm deep are two different jobs. Note whether the hole is through or blind.
- 22. Pick the opening operationCentre drill or spot drill 90° for location, then drill 0.5–1.0 mm under the finished diameter for a reamed hole, or 0.2–0.5 mm under for a bored hole. Use a peck cycle for depth beyond 3× diameter.
- 33. Check the boring bar L/D and pick the barDivide real overhang by bar diameter. Under 4:1 use a standard steel bar. 4:1 to 6:1 use a carbide bar. Beyond 6:1 use a tuned anti-vibration bar and reduce depth of cut to 0.2–0.5 mm per side.
- 44. Set speeds, feeds and coolant before the first cutAluminium: 200–350 m/min, 0.08–0.15 mm/rev. Steel 1045: 120–180 m/min, 0.05–0.12 mm/rev. Stainless 316: 80–120 m/min, 0.05–0.10 mm/rev. Titanium: 40–60 m/min, 0.05–0.08 mm/rev. Use through-coolant where the tool allows it.
- 55. Measure runout, then cut and gauge the first partIndicate the boring bar or reamer within 0.01 mm TIR. Take a 0.3 mm test cut, measure, and correct the offset before the finishing pass. Check roundness in two directions, not one.
Tool and process comparison for interior holes
Pick the row that matches your tolerance and depth
| Process | Typical tolerance | Depth limit | Best for |
|---|---|---|---|
| Twist drilling | IT12–IT13 | Up to 5× diameter with peck | Opening the hole, clearance bores |
| Helical interpolation | IT8–IT9 | Up to 4× diameter | Odd diameters, low volume, stepped bores |
| Reaming | IT7 (IT6 with float holder) | Up to 5× diameter | On-size rounds in one pass |
| Fine boring | IT6–IT7, ±0.005 mm | 3:1–4:1 steel bar, 8:1 damped bar | Position plus size, correction passes |
| Boring with damped bar | IT7–IT8 | 6:1 to 10:1 | Deep bores where reaming cannot reach |
Frequently asked questions
How deep can I bore before I need a special bar?
Past 4:1 for a standard steel boring bar, chatter usually appears before the insert wears out. Carbide bars push that to about 6:1, and tuned anti-vibration bars with an internal damper reach 8:1 to 10:1. The number that matters is real overhang from the holder face to the cutting edge, not hole depth.
When should I ream instead of bore?
Ream when the hole is round, the position is already correct from the drilling or boring step, and you need IT7 quickly in one pass. Bore when you need to correct position, hold a tight size across a range of parts, or the diameter is not a standard reamer size.
What stock should I leave for the finishing pass?
About 0.1–0.3 mm radial stock for a hand reamer, roughly 1 percent of diameter for a machine reamer, and 0.2–0.5 mm per side for a fine boring pass. Less than 0.1 mm often rubs instead of cutting, which smears the surface and ruins the size.
Why does my bore come out tapered?
Usually tool deflection at the bottom of a deep cut, or a bar that is too long for its diameter. Reduce depth of cut to 0.2–0.3 mm per side, shorten the overhang if the geometry allows, or switch to a damped bar. A worn insert with a large nose radius can also push the taper.
Can I hold ±0.005 mm in a deep hole?
Depth works against you. At 3:1 to 4:1 with a rigid setup, a carbide bar and temperature control, ±0.005 mm is realistic. Beyond 6:1, expect the achievable band to widen unless you use a damped bar, a warm-up cycle and in-process gauging.
How do I keep chips out of a blind hole?
Use through-spindle coolant where the tool allows it, add a retract cycle that lifts the tool every 1–2 mm of feed near the bottom, and prefer inserts with a positive rake that curls the chip tightly. In aluminium, higher helix and polished flutes keep the chip moving.
Send the drawing, get a boring plan
Upload your part and we will come back with a tooling route, tolerance check and DFM notes for the interior holes within 12 hours.
12-hour quote100% inspectionNo minimum order quantity
More CNC machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
