Reaming After Drilling: How to Hit H7 Tolerance Every Time

A drill produces a hole. A reamer produces a bore. The distinction matters when you're working to tolerance. A standard jobber-length HSS drill held to ±0.003" on a good day. An H7 reamed bore holds ±0.0005" routinely. For bearings, pins, bushings, and precision fits, drilling is just the first step — reaming is where the tolerance is made.

Here's the full process: what H7 means, how to set up the drill-to-ream sequence, and the variables that will either hit the tolerance or miss it.

What H7 Means

H7 is an ISO hole tolerance designation. The "H" means the hole's lower deviation is zero — the hole starts at the nominal dimension and goes only in the oversize direction. The "7" is the tolerance grade. For a 25mm hole, H7 means the hole must be between 25.000mm and 25.021mm. For a 1" bore, the equivalent is approximately +0.0000" to +0.0008".

H7 is the standard fit grade for most sliding and clearance fits — bearing inner races, dowel pins, ground shafts. It's tight enough to require controlled drilling and reaming, but achievable in a normal machine shop without exotic tooling.

Tighter grades (H6, H5) are used for interference and transition fits and require precision boring or lapping in addition to reaming on most equipment.

The Three-Step Sequence

Step 1: Drill Undersize

Never drill to the reamer's final diameter and then ream. Leave stock for the reamer to remove. The reamer needs material to work — if the pre-drilled hole is already at or near final size, the reamer will rub rather than cut, generating heat and oversizing the hole rather than refining it.

Standard stock allowance for machine reaming:

• Under 1/4": leave 0.005"–0.008" under nominal
• 1/4" to 1/2": leave 0.008"–0.015" under nominal
• 1/2" to 1": leave 0.015"–0.020" under nominal
• Over 1": leave 0.020"–0.030" under nominal

For H7 work, stay at the lower end of these ranges. Too much stock means the reamer takes a heavier cut than intended and may deflect, producing an oversize or tapered bore. Too little stock and the reamer doesn't cut enough to produce a consistent finish.

Step 2: Bore or Semi-Finish (Optional)

For critical bores or when the drill hole is suspected to be off-center, a single boring pass before reaming cleans up the geometry. The boring tool removes eccentric error from the drill hole and leaves a round, straight wall for the reamer to follow. This step adds time but significantly improves the final result when your drill press has runout or when positional accuracy matters as much as diameter tolerance.

Step 3: Ream to Size

Use a machine reamer — straight-flute or spiral-flute, depending on material. For through holes in most metals, a straight-flute reamer works well. For blind holes or materials that produce stringy chips, a spiral-flute reamer's helical cutting action pulls chips out more reliably.

Reaming speed should be roughly half the drilling speed for the same diameter and material. Stainless and hard alloys: slow down further. Feed per revolution should be consistent and moderate — erratic feed produces chatter marks on the bore wall.

Use cutting fluid on everything except cast iron. A dry reamer in steel will wear faster and heat enough to cause dimensional errors from thermal expansion. Flood coolant in CNC, cutting oil applied liberally by hand on manual setups.

Never reverse a reamer while it's in the hole. Machine reamers cut on the forward stroke only. Reversing a reamer in the hole rolls the chips backward under the flute margins, scoring the bore wall and damaging the cutting edges. Back it out forward at reduced feed, then stop spindle rotation outside the hole.

Variables That Kill Tolerance

Spindle Runout

A reamer running with measurable runout will produce an oversized hole. The reamer effectively becomes a boring tool, orbiting around the center and cutting on only one side. Measure your spindle TIR before precision reaming. Anything over 0.0003" TIR requires collet toolholding or a floating reamer holder (which allows the reamer to follow the existing hole rather than the spindle axis).

Chip Buildup in Flutes

Chips that pack in the flute grooves and re-contact the bore wall will scratch and oversized it. Clear chips frequently, especially on deeper holes. On production runs, program a chip-clear retract every 1.5–2 diameters of depth.

Wrong Stock Allowance

Leaving too much stock is the most common error on first attempts at precision reaming. When in doubt, err toward less stock rather than more. A hole that needs a second reaming pass because stock was insufficient is fixable. A hole that was opened oversize by a reamer taking too heavy a cut is usually a scrapped part.

Worn Reamer

A reamer that has cut a few hundred holes in steel is not the same tool it was when new. The margins at the flute land wear and the reamer begins to rub rather than size. Check reamers with a micrometer across the cutting lands periodically. Any detectable wear relative to nominal should trigger a resharpen or replacement before precision work.

---

H7 is achievable consistently with clean equipment, correct stock allowance, proper cutting fluid, and a reamer that's actually sharp. Every variable in the process is controllable. Master the sequence once and it becomes routine.