Honing Machining: Process, Tolerances, and Small-Bore Applications
Honing is the final sizing and finishing operation for precision bores — the step that turns a bored or reamed hole into a straight, round cylinder with a functional surface. Here is how the process works, what it can hold, and when to specify it, including small bores down to Ø3 mm.
IsoCNC Engineering Team
CNC Machining & DFM Engineers · Updated · 14 min read
On this page
Quick Answer
Honing is an abrasive finishing process that brings machined bores to their final size, geometry, and surface texture. Bonded stones on an expanding mandrel rotate and reciprocate inside the hole, removing a small, controlled allowance — typically 0.02–0.08 mm — and leaving the characteristic crosshatch pattern that retains lubricant. Typical results: size tolerances in the IT5–IT6 band, corrected roundness and taper, and finishes down to Ra 0.05–0.4 µm. At IsoCNC we hone small bores from Ø3 mm — including Ø4 mm bores up to 600 mm long — to ±0.002 mm and Ra 0.1 µm, in through holes and blind holes, across any machinable metal.
What Is Honing in Machining?
Honing is a low-speed abrasive process that finishes the inside of a hole using bonded stones mounted on an expanding mandrel. The mandrel rotates while stroking back and forth along the bore axis, and the stones press outward against the wall under controlled pressure. Because the tool floats — either the mandrel or the workpiece is free to align itself — honing follows the bore’s own centerline and averages away local errors with every stroke.
That behavior defines honing’s place in the hole-making chain: drill → bore or ream → hone. Drilling creates the hole, boring or reaming brings it close to size and establishes position, and honing takes the last few hundredths of a millimeter. It is the operation that fixes what the earlier steps cannot — out-of-roundness, taper, bell mouth, tool marks — while laying down a surface texture chosen for the part’s function, not just its appearance. If a drawing calls out a precision bore with a tight roundness or a specific finish, honing is usually how the shop gets there.
How the Honing Process Works
A honing tool carries two to a dozen abrasive sticks — conventional aluminum oxide or silicon carbide for most steels and cast irons, CBN or diamond superabrasives for hardened steels and carbides — set into a mandrel, often with hard guide shoes that stabilize the tool in the bore. A wedge mechanism inside the mandrel expands the stones radially, so cutting pressure is set mechanically rather than by the operator’s hand. Stock removal is deliberately slow: typically 0.02–0.08 mm on diameter, taken over many strokes. That slowness is the point — it is what makes the final size controllable to a few microns.
The combination of rotation and reciprocation produces honing’s signature: a crosshatch pattern, typically at a 20–60° included angle, set by the ratio of spindle speed to stroke speed. The valleys of that pattern hold oil; the plateaus carry the load. On sliding interfaces — hydraulic cylinders, valve bores, engine liners — this texture is a functional surface, not a cosmetic one. Honing oil floods the cut throughout, cooling the stones and flushing swarf so the finish stays consistent from one end of the bore to the other.
Machines come in two orientations. Vertical honing machines suit short bores and high-volume work — the classic automotive cylinder application. Horizontal honing machines support long parts and deep bores, where the stroke must travel many times the bore diameter without the tool whipping or the part sagging. A separate distinction is stroke honing versus single-pass honing, where a pre-sized diamond sleeve passes through the bore once — extremely fast and consistent for high volumes, but limited to through holes and modest stock removal.
What Honing Can — and Cannot — Achieve
Honing is the strongest hole-finishing process for geometry and the equal of any for size. The table below gives industry-typical results; every figure assumes a properly prepared bore with a sensible stock allowance. For how these numbers map to drawing callouts, see our reference on CNC machining tolerances.
| Characteristic | Typical Result | Notes |
|---|---|---|
| Size tolerance | IT5–IT6 band; ±0.002–0.01 mm is commonly achievable | The tightest sizing of any hole-finishing process; final op after boring or reaming |
| Roundness | Corrects out-of-round, lobing, and bell mouth from prior ops | Stones average the bore over many strokes — geometry improves every pass |
| Straightness / cylindricity | Corrects taper, bow, and barrel shape along the bore | Stroke length and stone wear are balanced to keep the bore parallel end to end |
| Surface finish | Ra 0.05–0.8 µm typical; plateau finishes on request | Crosshatch texture doubles as an oil-retention surface |
| Position / location | Cannot correct | The floating mandrel follows the existing bore axis — fix position upstream at boring |
| Perpendicularity to a face | Cannot correct | Datum faces must be squared before honing, or ground afterward |
The two "cannot" rows matter most at the design stage. Because the tool follows the bore, honing will faithfully perfect a hole that is in the wrong place. Position, perpendicularity, and true alignment between bores belong to the boring operation upstream — usually on a machining center or jig borer — and must be verified before honing starts. If your print carries a tight cylindricity callout alongside a tight position tolerance, that is a two-process feature by definition.
Honing vs Reaming vs Boring vs ID Grinding
These four processes overlap, and drawings often could be satisfied by more than one of them. The practical difference is what each one is for: boring establishes the hole, reaming sizes it quickly, grinding removes real stock from hard material, and honing perfects geometry and texture. Our guides to reaming and CNC grinding go deeper on each; this table is the selection view. For how the first three processes in the chain divide their work, see the drilling vs boring vs reaming guide.
| Process | Stock Removed | Size Tolerance (Typ.) | Finish (Typ.) | Best Role |
|---|---|---|---|---|
| Boring | Heavy — millimeters | IT7–IT8 | Ra 0.8–3.2 µm | Establishes size, position, and alignment; the op honing follows |
| Reaming | Light — 0.1–0.5 mm | IT6–IT7 | Ra 0.4–1.6 µm | Fast, accurate sizing of drilled holes at production rates |
| ID grinding | Moderate | IT5–IT6 | Ra 0.1–0.8 µm | Hard materials and interrupted cuts; removes stock honing cannot |
| Honing | Very light — 0.02–0.08 mm | IT5–IT6 | Ra 0.05–0.8 µm | Final geometry, size, and crosshatch texture on precision bores |
A few rules of thumb. If the hole needs only an accurate diameter at production speed, reaming wins on cycle time. If the material is hard and more than a few hundredths must come out, grind first — honing that much stock is slow and wears stones unevenly. If the drawing asks for roundness, cylindricity, a controlled finish, or an oil-bearing texture, hone last. Many precision bores use three of the four in sequence, and that is normal engineering, not indecision.
Small-Bore and Deep-Hole Honing
Most honing content is written about engine cylinders — bores measured in inches. Small-bore honing is a different discipline. Mandrels slim enough for a Ø3–6 mm hole are delicate, stone wear shows up as taper over a long stroke, and measuring the result takes bore gauges and air gauging rather than a quick pass with a pin gauge. Blind holes add another constraint: the stones reverse stroke inside the bore without exiting, so the bottom of the hole sees different abrasions than the mouth — keeping that bore parallel end to end is the craft.
This is the work our horizontal honing machines do every day. IsoCNC hones small bores from Ø3 mm, including Ø4 mm bores up to 600 mm long — a 150:1 length-to-diameter ratio that demands rigid horizontal support and disciplined stroke control. On small bores we hold size tolerance to ±0.002 mm and surface finish to Ra 0.1 µm, in through holes and blind holes alike. Material is not a constraint: aluminum, stainless, hardened steels, and other machinable metals are all honed by matching the stone, grit, and tooling to the workpiece. Because honing runs in-house as the finishing step for the parts we machine, the bore never leaves our workflow — the same team that bores the hole hones it, and verifies it with bore gauges, a roughness tester, and CMM before it ships.
Where Honed Bores Earn Their Keep
Honing earns its cost wherever a bore is a working surface rather than a clearance hole. The recurring applications:
- Hydraulic and pneumatic valve bores — spool-to-sleeve clearance measured in microns, where roundness directly controls internal leakage and response.
- Fuel injection components — nozzle and plunger bores where fit and finish decide spray behavior and sealing.
- Cylinders and pump bodies — the crosshatch texture retains oil and seats piston rings or seals during break-in.
- Gear and bearing bores — controlled size and roundness for press or slip fits that must stay consistent across a lot; see our guide to engineering fits for the fit system behind these callouts.
- Connecting rods and actuator components — big-end and small-end bores finished to size with a load-bearing surface texture.
- Medical and instrumentation parts — small precision bores in stainless and titanium where finish affects cleaning and function.
What these share is a bore that interacts with something — a spool, a seal, a ring, a pin. If the hole merely passes a bolt, honing is overkill; if the hole works, honing is usually the cheapest way to make it work reliably.
Specifying Honing on Your Drawing
You rarely need to write "hone" on a print — a good shop reads the requirements and chooses the process. What the drawing must carry is the end state: the size and tolerance, the surface finish (Ra), any geometry callouts such as roundness or cylindricity, and a note if the crosshatch itself is functional. A bore specified at Ø12 H6 with Ra 0.2 and a roundness callout will be honed by any shop that takes the print seriously.
Three practical points sharpen the quote. First, leave the right stock allowance: honing typically removes 0.02–0.08 mm on diameter, so the preceding bore or ream should land consistently inside that window — too much stock wastes time, too little cannot clean up the bore. Second, hone only the bores that need it: tightening every hole on the print to honing-level requirements multiplies cost without buying function, the same DFM logic covered in our DFM design guide. Third, state material and hardness — parts hardened after machining are honed after heat treatment, and the stone selection changes with the alloy. Send the drawing with those three things settled and the quote comes back without questions.
FAQ: Honing Machining
What is honing in machining?
Honing is an abrasive finishing process for holes. Bonded abrasive stones mounted on a mandrel rotate and reciprocate inside a bore while expanding outward under controlled pressure, removing a small, predictable amount of stock — typically 0.02 to 0.08 mm on diameter. The result is a hole brought to final size with corrected roundness, straightness, and a controlled surface texture. Honing is always a finishing operation: the hole is drilled and bored or reamed first, and honing takes it the last few hundredths of a millimeter to its final dimension.
What is the difference between honing and grinding?
Both are abrasive processes, but they solve different problems. ID grinding uses a small wheel at high speed to remove stock and can bring a hardened bore to size from a rough state. Honing uses multiple stones at low speed with a reciprocating stroke, removes far less material per pass, generates less heat, and excels at the last stage: correcting roundness and taper, hitting a tight size band, and laying down a crosshatch surface texture. In practice, grinding is chosen when real stock must come out of a hard bore; honing is chosen when geometry, size control, and surface function matter most.
How much material does honing remove?
Very little by design — typically 0.02 to 0.08 mm on diameter, sometimes up to 0.1 mm when a bore needs more cleanup. Honing is not a roughing process, and feeding it too much stock wastes cycle time and wears stones unevenly, which shows up as taper. The upstream boring or reaming operation should leave a consistent, small allowance. If a bore needs more than about a tenth of a millimeter removed, it goes back to boring or to ID grinding first.
Can honing correct the position of a hole?
No. The honing mandrel floats and follows the bore's existing axis, so it improves everything about the hole itself — size, roundness, straightness, taper, surface — but it cannot move the hole or change its angle. Position, perpendicularity to a datum face, and alignment between multiple bores must be established at the boring stage. This is the single most common misconception about honing, and it is worth remembering when you decide which process fixes which drawing requirement.
What is the crosshatch pattern from honing for?
The intersecting scratch pattern — typically laid at a 20–60° included angle, set by the ratio of rotation speed to stroke speed — acts as a network of microscopic oil reservoirs. On sliding or rotating interfaces such as hydraulic cylinders, valve bores, and engine liners, the valleys retain lubricant while the plateaus carry the load, which reduces wear and prevents scuffing during break-in. Where sealing matters, the crosshatch angle and depth are functional requirements, not cosmetics, and can be called out on the drawing.
Can small holes and blind holes be honed?
Yes, with dedicated tooling. Small-bore honing uses slim mandrels and fine-grit stones, and blind holes are honed by reversing the stroke inside the bore without the stones exiting — stroke control at the bottom is what keeps the bore parallel. At IsoCNC, our horizontal honing machines finish small bores from Ø3 mm, including Ø4 mm bores up to 600 mm long, holding ±0.002 mm and Ra 0.1 µm in through holes and blind holes alike, across any machinable metal.
Related Resources
What Is CNC Machining?
What is CNC machining? A plain-English guide to how it works, the main process types, materials, tolerances, and…
How Does CNC Machining Work? A Step-by-Step Look at the Process
How does CNC machining work? Follow a part from CAD to CAM, setup, machining, inspection, and shipping — and see…
Types of CNC Machining: Every Process and When to Use It
The main types of CNC machining explained: 3/4/5-axis milling, turning, mill-turn, Swiss machining, EDM, grinding —…
How to Outsource CNC Machining to China, Step by Step
How to outsource CNC machining to China, step by step: vet suppliers, compare landed cost, control quality remotely,…
Precision Bores on Your Drawing? Send It In.
IsoCNC machines and hones precision-bore parts in one workflow — small bores from Ø3 mm, deep bores to 600 mm, held to ±0.002 mm and Ra 0.1 µm, through holes and blind holes in any machinable metal. Every lot is verified with bore gauges, roughness testing, and CMM inspection before shipment. An engineer reviews every RFQ, typically within 1–2 business days.