Reaming SFM (HSS vs carbide), feed IPR by diameter, and drill-stock allowance on diameter.
How to Use This Chart
Use ~½–⅔ of drilling SFM as a mental check; this chart mirrors the reaming calculator tables. Tool: reaming speed calculator. Guide: reaming guide. Convert SFM to RPM with RPM = SFM × 3.82 ÷ reamer diameter (inches), then pick IPR from the diameter table — do not run a reamer at drill RPM.
Why This Chart Mirrors the Drilling Speed Chart — and Why You Should Not Copy Drill RPM
A reamer is a finishing tool. It is designed to size and finish a hole that already exists, not to hog stock the way a twist drill does. That is why shop practice treats reaming SFM as roughly half to two-thirds of the drilling SFM for the same material and tool class. The drill speeds by material chart is the sibling table: same materials, higher surface speeds, different job. If you take a mild-steel HSS drill at 80–100 SFM and run the reamer at that same number, you will usually chatter, bell-mouth, or burn the margins.
The mental check is useful because it keeps you from treating this page as an isolated lookup. Drill the hole using the drill chart (or the drill speed calculator), leave the stock allowance in the table below, then drop SFM and use a steady feed so the reamer cuts a chip instead of rubbing. The two charts are a pair, not duplicates.
Why HSS and Carbide SFM Diverge
HSS reamers are tougher at the edge and more forgiving of interrupted cuts, misalignment, and hand-feed drill presses. They also lose hardness as soon as the margin gets hot. That is why HSS SFM sits in the 15–60 range for steels and only climbs for aluminum and brass. Carbide holds a hard, sharp edge at much higher surface speed, so the carbide column is typically 2–3× the HSS column. That is not a suggestion to “always run carbide.” Carbide reamers chip if the spindle has runout, if the pre-drilled hole is off-center, or if you tap the tool into a chuck that is not true. On a worn Bridgeport or a hand-held reamer in a tap handle, HSS at the low end of the band is the correct choice even if you own carbide.
Material still gates both columns. Stainless work-hardens if you rub; stay at the low end and keep feed up so the edge is cutting. Aluminum wants speed and chip evacuation so the flute does not pack. Cast iron is abrasive — carbide pays off on production counts, HSS is fine for a handful of holes. Do not average the two columns or split the difference as a “safe” SFM; pick the tool you actually have in the spindle.
Why Stock Allowance Matters for Tolerance and Chatter
Leave too little stock and the reamer rubs. Rubbing burnishes the hole, work-hardens stainless, and produces a shiny undersize or tapered bore that no amount of extra RPM will fix. Leave too much and the reamer is doing a drill’s job: heavy radial load, wandering, chatter, and an oversized hole. The allowance table is on diameter (twice the per-side number). A ½″ finished hole with 0.015–0.020″ on diameter means you drill about 0.480–0.485″, not 0.490″ “to be safe.”
Chatter on a reamer is often an allowance problem disguised as a speed problem. If the pre-drill is already at finished size minus a few thousandths, the flutes have nothing to cut and the tool vibrates on the margins. Opening the pre-drill is the wrong fix; leaving proper stock and slowing SFM while keeping IPR in the diameter band is the right one. For press-fit or H7-class holes, treat the allowance as a process variable you measure: log pre-drill size, reamer condition, and resulting bore until the combination is repeatable. The chart is the starting window, not the capability study.
Start Conservative, Then Adjust Up
Guessing high on SFM is how reamers die. A dull or chipped reamer cuts an oversized, out-of-round hole long before you notice the finish went bad. Start at the low end of the HSS or carbide band, use the mid IPR for that diameter, flood or through-coolant if you have it, and take one scrap hole. If the hole is to size, round, and quiet, you can add SFM in modest steps. If it chatters, drop speed before you drop feed — starving IPR while spinning faster is the classic “polishing” mistake.
Machine rigidity still wins. A reamer in a floating holder on a mill can often run closer to the chart than the same reamer in a worn drill-press chuck. Hand reaming is a different process entirely: the SFM table does not apply; you are controlling feel, not RPM. For CNC, lock RPM from this chart and let feed be in/min = IPR × RPM. Do not let CAM default to drill speeds because the tool is in a drill cycle.
SFM by Material
| Material | HSS SFM | Carbide SFM |
|---|---|---|
| Mild steel | 40–60 | 100–150 |
| Tool steel | 20–35 | 60–100 |
| Stainless | 15–30 | 50–90 |
| Cast iron | 40–60 | 100–150 |
| Aluminum | 100–150 | 250–400 |
| Brass | 80–120 | 200–300 |
| Copper | 50–80 | 150–250 |
| Plastic | 100–150 | 200–350 |
Feed IPR by Reamer Diameter
| Reamer diameter | IPR |
|---|---|
| Under 1/8″ | 0.001–0.003 |
| 1/8–1/4″ | 0.003–0.006 |
| 1/4–1/2″ | 0.006–0.010 |
| 1/2–1″ | 0.010–0.015 |
| Over 1″ | 0.015–0.025 |
IPR scales with diameter because a larger reamer has more teeth sharing the chip and needs enough feed so each tooth cuts. Tiny reamers look “slow” in in/min; that is correct. Forcing 0.015 IPR on a 1/8″ reamer is how you break it.
Stock Allowance on Diameter
| Finished hole Ø | On diameter | Per side |
|---|---|---|
| Under 1/4″ | 0.010–0.015 | 0.005–0.0075 |
| 1/4–1/2″ | 0.015–0.020 | 0.0075–0.010 |
| 1/2–1″ | 0.020–0.030 | 0.010–0.015 |
| Over 1″ | 0.030–0.040 | 0.015–0.020 |
Get SFM, RPM, feed, and pre-drill size
WeldKit — Welding Calculators Offline
MIG, TIG, Stick, speeds/feeds, and more on Android.