A machinist needs a 0.5000" finished hole and asks the obvious question: why not just drill it with a 1/2" drill? Because making a hole and finishing a hole are two different operations. A drill enters solid material, centers itself, makes chips, and evacuates them, all at once. A reamer starts with a hole that already exists and takes a controlled sliver off the wall. Here is where the line falls, and—the part most articles skip—how much material to leave, according to the people who actually build the tools.
A drilled hole is not the same as a reamed hole.
A drill has a difficult job. It must enter solid material, center itself, generate chips, evacuate them, and create the hole, all at the same time. Because of those cutting forces, the finished hole may not reproduce the drill's nominal diameter to the precision the print demands.
A reamer starts from an existing hole. Instead of removing the entire core, its cutting edges take a controlled amount off the wall. Think of it in two steps: drilling creates the hole, and reaming finishes it.
For general holemaking, start with solid carbide jobber-length drills. Where rigidity matters and you want less deflection, the screw-machine-length drills are shorter and stiffer for the same diameter.
What a drill can — and cannot — control
The diameter stamped on a drill is its nominal cutting diameter. It is not a guarantee of the diameter of the hole it will produce. Several things move the result:
- Runout lets the cutting edges sweep a larger effective circle than the tool measures.
- Tool deflection affects hole location and straightness.
- Workpiece material changes cutting forces, chip formation, and the tendency to build up on the edge.
- Drill geometry and condition decide how cleanly the tool enters and cuts.
- Machine and workholding rigidity govern vibration and positional accuracy.
- Speeds, feeds, and coolant delivery drive chip evacuation, heat, and wear.
For plenty of work, a drilled hole is entirely adequate. When diameter, roundness, straightness, or surface finish becomes a critical feature on the print, a finishing operation earns its place. That is where the reamer comes in.
How much stock to leave: the published numbers
This is the most misunderstood question in reaming, and the honest answer is that the industry does not agree on one number. What follows is what tool manufacturers actually publish, side by side, so you can see the spread rather than trust a single chart.
Approach 1—a fixed scale by diameter. Three published tables, unaltered:
| Finished hole | Gammons Hoaglund | ICS Cutting Tools | Alvord-Polk |
|---|---|---|---|
| Up to 1/16" | .003–.006" (to 1/8") | .003–.005" | .003–.006" (to 3/32") |
| 1/16" – 1/8" | .003–.006" | .004–.008" | .008–.010" (3/32"–1/4") |
| 1/8" – 1/4" | .005–.009" | .006–.012" | .008–.010" |
| 1/4" – 3/8" | .007–.012" | .008–.014" | .012–.015" (1/4"–1/2") |
| 3/8" – 1/2" | .010–.015" | .010–.015" | .012–.015" |
| 1/2" – 3/4" | .015–.031" | .012–.018" | .017–.020" (1/2"–1") |
| 3/4" – 1" | .031" | — | .017–.020" |
| 1" – 2" | — | — | .020–.025" |
| Over 2" | — | — | .030–.035" |
Sources as published: Gammons Hoaglund, Stock Allowance for Machine Reaming; ICS Cutting Tools, Reaming Recommendations; Alvord-Polk, quoted in Cutting Tool Engineering. None of the three separates HSS from carbide. Where a source's band does not line up with the row, its own range is noted in grey.
Approach 2—a percentage of the finished diameter. Carbide reamer makers tend to publish a rule instead of a table:
| Source | Rule | On a 0.500" hole | Tool |
|---|---|---|---|
| Hannibal Carbide | 2–3% of reamer diameter finish reaming; up to 5% rough reaming. 2% steels and tough alloys, 3% non-ferrous and cast iron | .010–.015" | Carbide & carbide-tipped |
| Super Tool | 2–3% of finished hole size—multiply the finished diameter by 0.98 and 0.97 to bracket the pre-drill | .010–.015" | Carbide & carbide-tipped |
| Harvey Performance | Pre-drilled hole = 90–94% of final diameter, i.e., 6–10% stock—for miniature reamers | .030–.050" | Solid carbide, miniature |
| Gammons Hoaglund | ≈3% of hole diameter; below 1/2" ream only .006–.008"; hand reaming .001–.003" | .015" | Not specified |
Harvey's figure is for miniature reamers and is two to three times the others. It is here because it is published, not because it transfers to a 1/2" hole. Alvord-Polk rejects the percentage approach outright: "It's a sliding scale. It doesn't even work out as a percentage."
Approach 3—metric, and adjusted for hardness. Guhring publishes the recommended stock allowance in millimeters on the diameter and is the only source that reduces the allowance as the workpiece gets harder:
| Hole diameter | All materials | Hardened steel ≤48 HRC | Hardened steel ≤63 HRC |
|---|---|---|---|
| up to Ø6 mm | 0.1–0.2 mm | 0.1–0.2 mm | 0.1 mm |
| up to Ø10 mm | 0.2 mm | 0.2 mm | 0.1 mm |
| up to Ø16 mm | 0.2–0.3 mm | 0.2 mm | 0.1–0.2 mm |
| up to Ø25 mm | 0.3 mm | 0.2 mm | 0.2 mm |
| up to Ø40 mm | 0.3–0.4 mm | 0.3 mm | 0.2 mm |
| above Ø40 mm | 0.4–0.5 mm | 0.3 mm | 0.2 mm |
Guhring, Reamers, countersinks, and deburring catalogue. Ø10 mm ≈ 0.394"; 0.2 mm ≈ .008"—which puts Guhring squarely on top of the inch tables for the same size.
Too little stock is its own failure mode.
Leaving too much material is the mistake everyone anticipates. Leaving too little is the one that quietly ruins holes, and the manufacturers are blunt about it.
Hannibal Carbide: "Solid carbide & carbide-tipped reamers must have adequate stock to remove, or they will rub in the hole and generate excessive heat, which leads to premature tool wear." M.A. Ford puts both failures in one sentence: "If the hole is too close to the finish size, the reamer will tend to burnish the hole, and excessive tool wear will occur. If too much material is left, chips can clog the flutes of the reamer, resulting in a poor finish, poor size control, and possible tool breakage."
A reamer that rubs instead of cutting work-hardens the surface it is supposed to finish, and the next pass has a harder skin to get through than the one before it. Gammons makes the same point about feed: too low a feed can "glaze" the hole, with the same work-hardening result.
Why you shouldn't use a reamer to drill the hole
A reamer is not a drill. It is built to follow an existing hole and take a small amount off the wall. Push it to remove excessive material, and cutting forces rise, tool life drops, finish suffers, and the tool can fail outright.
The sequence is drill the undersized hole, then ream to the finished diameter. Drills and reamers are complementary tools, not competing ones—which is why a holemaking process is specified as a pair, not as a single tool.
Carbide or HSS?
Both have legitimate applications. High-speed steel brings toughness, which suits less rigid setups, lower cutting speeds, and jobs where tool cost dominates. Solid carbide brings substantially greater rigidity and wear resistance and supports higher productivity when the machine, the setup, and the application allow it.
That makes carbide the natural choice for CNC production, abrasive materials, repetitive holemaking, and anywhere dimensional consistency across a long run matters more than the price of the tool. It also changes the stock allowance conversation: the sources that publish a 2–3% rule are, without exception, the ones talking about carbide.
Four flutes or six? The catalogue is already decided.
Flute count is the one reamer variable a buyer actually chooses, and it is a straight trade between two things that both matter.
More flutes mean more cutting edges in contact with the wall. The tool is better supported, each edge takes a smaller bite at the same feed rate, and roundness and finish benefit. Fewer flutes means more room in each gullet for the chip to form and leave. In a blind hole that room is not a luxury: a chip that has nowhere to go gets dragged between a cutting edge and a wall you have just finished, and that is a scratched bore.
Below a certain diameter the argument settles itself, because six flutes in a small tool leave gullets too shallow to clear anything. Which is why the reamer line here splits cleanly and without overlap:
| Diameter | Flutes | References in stock | Why |
|---|---|---|---|
| .0280" – .2495" | 4 | 452 | Chip Room wins. At these diameters there is no space for six usable gullets. |
| .2500" – .7510" | 6 | 331 | Support wins. The gullets are large enough, so the extra edges buy roundness and finish. |
What that leaves you to think about is the hole, not the tool. In a through hole, chips have somewhere to go, and the decision is made for you. In a blind hole, plan the chip evacuation before you plan the cut: coolant pressure and volume, peck strategy if the depth calls for it, and enough room at the bottom that the last chips are not being recut against the finished wall. All 783 diameters are here, one reference per diameter.
Speeds and feeds
There is no universal reaming speed. The right parameters depend on workpiece material, reamer diameter, carbide or HSS construction, coating, flute geometry, hole depth, coolant strategy, and machine rigidity.
The common mistake is lifting a generic reaming speed off a chart and applying it to every tool. Start from the manufacturer's cutting data for that specific tool in that specific material, then read the evidence: tool wear, surface finish, chip formation, and the measured hole. The goal is not to make the reamer survive. It is to produce the required hole consistently, part after part.
Seven reasons a reamed hole comes out oversize or rough
When the hole is wrong, the reamer is the last thing to blame, not the first.
- Excessive runout. If the reamer is not running concentrically, the cutting edges sweep an oversized path. This is the most common cause and the least often checked.
- Too much stock. Excess material raises cutting forces, packs the flutes, and costs you both accuracy and finish.
- Too little stock. The tool rubs instead of cutting, generates heat, and work-hardens the surface.
- Wrong cutting speed. Too fast generates heat and accelerates wear; too slow can stop the tool cutting cleanly.
- Wrong feed. Feeding too lightly encourages rubbing; too heavily overloads the edges and degrades finish.
- Worn or damaged edges. A chipped edge or one carrying built-up material cannot produce a precision surface, whatever the parameters.
- Poor coolant delivery or chip recutting. Heat and trapped chips damage the finished wall and the cutting edges together.
Before you change tools, look at the whole system: tool, holder, runout, the pre-hole itself, parameters, coolant, workholding, and machine condition.
Drill or reamer? Start with the print.
If the print asks for a nominal hole with an open tolerance, drilling may be all you need. If it asks for tighter dimensional control, better roundness, or a better surface finish, drilling followed by reaming is the process.
So go back to the 0.5000" hole. The question is not "which 1/2" drill should I buy?" The question runs backwards from the print:
For that 0.5000" hole: a 0.5000" reamer, .010–.015" of stock on the diameter, and therefore a pre-drill somewhere around .485"–.490". The drill creates the hole. The reamer turns it into a precision feature.
FAQ
How much material should I leave for reaming?
It depends on diameter, material, and whether the reamer is HSS or carbide, and published recommendations genuinely disagree. Around a 1/2" hole, four independent manufacturers converge on .010" to .015" on the diameter. Below 1/8", .003" to .006". Carbide reamer makers often publish it as 2–3% of the finished diameter instead of a table. Always start from the recommendation for the specific tool you are using.
Is the reaming allowance measured on the diameter or per side?
Almost all published charts give it on the diameter—the total material removed across the hole. A few sources quote depth of cut per side instead. Confusing the two doubles or halves your allowance, so check which basis a chart uses before you set the pre-drill size.
Can I just drill a hole to size instead of reaming it?
For a nominal hole with an open tolerance, often yes. A drill's stamped diameter is its nominal cutting diameter, not a guarantee of the hole it produces—runout, deflection, material, and rigidity all move the result. When diameter, roundness, straightness, or finish are critical features on the print, a reaming pass is what controls them.
Why is my reamed hole oversize?
Check runout first: a reamer that is not concentric sweeps an oversized path regardless of how good the tool is. After that, look at stock allowance in both directions, speed and feed, edge condition, and coolant and chip evacuation.
Should I use a 4-flute or a 6-flute reamer?
Diameter decides it. Below 1/4", there is no room for six usable chip gullets, so small reamers are 4-flute; from 1/4" up, the gullets are large enough that the extra cutting edges buy better support, roundness, and finish. In the FM Carbide line the split is exactly at .2500", with no overlap: 452 four-flute references below it and 331 six-flute references above.
What happens if I leave too little stock for the reamer?
The tool rubs or burnishes instead of cutting. That generates heat, accelerates wear, and work-hardens the surface you were trying to finish, which makes the next pass harder than the last. Carbide reamer manufacturers warn about this explicitly.
Build the process, not just the hole.
517 solid carbide jobber-length drills across 145 diameters, 2- and 3-flute, coated and uncoated; 138 screw-machine-length drills, shorter and stiffer, 135° point; 783 solid carbide reamers, one for every diameter from .0280" to .7510", 4- and 6-flute.
Shop Jobber Drills → Shop Screw Machine Drills → Shop Reamers →Tools when you need them. Knowledge when you need it. · Stock allowance figures reproduced as published by Gammons Hoaglund, ICS Cutting Tools, Alvord-Polk (via Cutting Tool Engineering), Hannibal Carbide, Super Tool, Harvey Performance Company, and Guhring and M.A. Ford. They are starting points, not specifications: the recommendation for the tool in your hand always takes precedence.
Comments (0)