Keyseat Miller Feeds & Speeds — Operating Guide
Getting feeds and speeds right on a keyseat miller is one of the most common questions we hear from both new and experienced users. Run too fast and you’ll chatter, overheat the cutter, or lose tolerance. Run too slow and you’ll rub instead of cut, work-harden the bore wall, and wear out the tool prematurely. The right parameters depend on your miller model number, your material, and your setup.
This page covers NMT’s recommended spindle speeds and feed rates for all keyseat miller models, plus context on how to apply those numbers and what to watch for in the cut.
How to Read This Chart
Keyseat Miller Number refers to your NMT model designation. This is stamped or labeled on your tool. The letter suffixes (A, B, S, C) denote configuration variants — pilot size, slot width, or special application — but the operating parameters are the same within each numbered group.
Pin Drive refers to the number of driving pins used to engage the cutter. Pin drive 2 vs. 3 vs. 4 affects torque transmission and is fixed by the tool design — you don’t select it, it’s how the tool is built.
Spindle Speed (RPM) is given as a range. Use the lower end of the range when starting on a new application, in harder materials, or when the bore is deep relative to diameter. Move toward the upper end when conditions are confirmed good — chip formation is clean, no chatter, and the tool is running freely.
Hard Steel RPM is a single value rather than a range because the operating window in hard material is narrower. Stay close to the listed value and reduce feed rate if you see poor chip formation or heat buildup.
Feed Rate is in inches per minute and represents the axial feed — how fast you’re advancing the tool into the bore. Cast iron feeds faster because the material is brittle and chips cleanly; steel requires a slower, more controlled feed to prevent chip packing and tool loading.
Feeds & Speeds Reference Table — Keyseat Millers
| Keyseat Miller # | Pin Drive | RPM Cast Iron | RPM Mild Steel | RPM Hard Steel | Feed/Min Cast Iron (in) | Feed/Min Steel (in) |
|---|---|---|---|---|---|---|
| 0-B | 2 | 1600–1900 | 1000–1300 | 840 | 1½ | ⅜ |
| 0-BS | 2 | 1600–1900 | 1000–1300 | 840 | 1½ | ⅜ |
| 0-A | 2 | 1600–1900 | 1000–1300 | 840 | 1½ | ⅜ |
| 0-AS | 2 | 1600–1900 | 1000–1300 | 840 | 1½ | ⅜ |
| 0 | 3 | 1500–1800 | 910–1250 | 840 | 1½ | ⅜ |
| 0-S | 2 | 1400–1650 | 910–1200 | 740 | 1½ | ⅜ |
| 1 | 3 | 1000–1200 | 700–840 | 560 | 2 | ½ |
| 1-S | 2 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 2-B | 3 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 2-A | 3 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 2 | 3 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 2-½B | 3 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 2-½A | 3 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 2-½AS | 2 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 2-½ | 3 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 2-½S | 2 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 3-C | 2 | 900–1080 | 650–780 | 520 | 2 | ½ |
| 3-B | 3 | 750–900 | 650–780 | 500 | 2 | ½ |
| 3-A | 3 | 750–900 | 650–780 | 500 | 2 | ½ |
| 3-AS | 2 | 750–900 | 650–780 | 500 | 2 | ½ |
| 3 | 3 | 750–900 | 650–780 | 500 | 2 | ½ |
| 3-S | 2 | 750–900 | 650–780 | 500 | 2 | ½ |
| 4-C | 3 | 650–780 | 420–500 | 380 | 2 | ½ |
| 4-B | 3 | 650–780 | 420–500 | 380 | 2 | ½ |
| 4-A (4) | 3 | 650–780 | 420–500 | 380 | 2 | ½ |
| 4-A (4) | 4 | 600–720 | 400–500 | 340 | 2 | ½ |
| 5-A (5) | 3 | 400–480 | 260–320 | 205 | 2 | ⅜ |
| 5-A (5) | 4 | 420–480 | 260–320 | 205 | 2 | ⅜ |
| 6-A (6) | 3 | 400–480 | 240–320 | 190 | 2 | ⅜ |
| 6-A (6) | 4 | 420–480 | 240–320 | 190 | 2 | ⅜ |
| 7-A (7) | 3 | 350–420 | 220–320 | 180 | 2 | ⅜ |
| 7-A (7) | 4 | 350–420 | 220–320 | 180 | 2 | ⅜ |
Oil Grooving Millers (separate series):
| Miller # | Pin Drive | RPM Cast Iron | RPM Mild Steel | RPM Hard Steel | Feed/Min Cast Iron (in) | Feed/Min Steel (in) |
|---|---|---|---|---|---|---|
| 0 | 3 | 1600–1900 | 1000–1250 | 840 | 1½ | ⅝ |
| 1 | 3 | 1000–1200 | 700–840 | 560 | 2 | ⅝ |
| 2 | 3 | 900–1080 | 650–780 | 520 | 2 | ⅝ |
| 3 | 3 | 750–900 | 620–780 | 500 | 2 | ⅝ |
| 4 | 3 | 750–900 | 600–780 | 500 | 2 | ⅝ |
Applying These Parameters — What to Watch For
The table gives you the starting point. Here’s how to dial it in for your specific setup:
Starting a New Application
Always begin at the lower end of the RPM range and at or below the listed feed rate. Run a short test cut — a few inches of axial travel — and evaluate before committing to the full depth or length. What you’re looking for:
Good cut indicators:
- Chips are forming cleanly and evacuating freely from the bore
- No chatter or vibration felt through the machine
- No unusual heat buildup at the cutter or bore entry
- Keyway walls are clean with no tearing or built-up edge on the cutter
Adjust up (increase RPM toward the top of the range, increase feed slightly) if the cut feels sluggish, chips are thick and heavy, or the tool is rubbing rather than cutting.
Adjust down (reduce RPM, reduce feed) if you hear chatter, feel vibration, see chip packing in the bore, or notice heat at the cutter.
Material-Specific Notes
Cast iron: Cast iron is brittle and chips cleanly, which is why feed rates are higher. The material doesn’t work-harden under the cutter, so you have more margin in feed rate. Keep the bore and cutter dry — coolant is generally not needed and can cause cast iron to crack on thermal cycling in deep cuts.
Mild steel (1018, 1045, and similar): Steel requires a controlled feed to prevent chip packing, especially in blind bores where chips have nowhere to go. Use the lower end of the RPM range for deeper keyways. A light cutting oil or coolant applied at the bore entry helps chip evacuation significantly.
Hard steel (4140, 4340, and other alloys): The single RPM value for hard steel reflects the narrower operating window in tougher material. Don’t exceed it — running too fast in hard steel generates heat that dulls the cutter rapidly. Run at the listed RPM, reduce feed rate 20–30% from the steel column value, and use cutting oil. Watch chip color — if chips are turning blue or brown, you’re generating too much heat.
Stainless steel: Not listed in the table because it varies widely by alloy. For austenitic stainless (304, 316), use the hard steel RPM values and reduce feed rate by approximately 30% from the mild steel column. Stainless work-hardens rapidly — maintain a positive feed at all times, never dwell in the cut. For 17-4 PH and other precipitation-hardening grades, contact NMT for specific recommendations.
Aluminum and bronze: Not listed in the table — these materials are softer than cast iron and can be run at the upper end of the cast iron RPM range. Feed rates can be increased beyond the cast iron values. Use cutting fluid to prevent chip welding on aluminum.
Titanium and nickel alloys (Inconel, Hastelloy): Reduce RPM to approximately 60–70% of the hard steel value. Reduce feed rate to approximately 50% of the steel column value. Use cutting oil, maintain consistent feed — never dwell in the cut. Contact NMT when ordering tooling for these materials so the cutter geometry can be specified appropriately.
Setup Tips That Affect Feeds and Speeds
The parameters in the table assume a properly set up tool and machine. If your results don’t match the expected cut quality, check setup before adjusting feeds and speeds:
Spindle runout: Excessive runout in the drill press or milling machine spindle translates directly to keyway width variation and poor surface finish. Check with a test indicator before running a precision application.
Pilot fit: The tool pilot should be a close sliding fit in the bore — loose enough to enter smoothly, tight enough that there’s no lateral play. A sloppy pilot fit causes the cutter to drift off centerline, producing a wide, off-center keyway regardless of how good the feeds and speeds are.
Pin drive engagement: Confirm the driving pins are fully seated in the cutter slots before starting the cut. Partially engaged pins transmit torque unevenly and can cause the cutter to slip or chatter.
Bore condition: A rough or out-of-round bore will cause the tool to hunt as it feeds, producing chatter marks in the keyway. For precision applications, the bore should be finished before the keyway is cut.
Quill or Z-axis feed: On a manual drill press, feed rate is controlled by hand pressure on the quill. Maintain smooth, consistent feed pressure — hesitation in the feed produces chatter marks; surging produces overload. On a CNC machining center, program the feed rate per the table values.
Troubleshooting Common Feeds and Speeds Problems
Chatter marks on keyway walls: Most common cause: RPM too high or feed rate too slow. Try reducing RPM 10–15% and increasing feed rate slightly. Also check pilot fit and driving pin engagement.
Rapid cutter wear: Most common cause: RPM too high in hard materials, or cutting dry when coolant is needed. Reduce RPM to the hard steel value, apply cutting oil, and check that chips are evacuating rather than being re-cut.
Keyway oversized in width: Most common cause: spindle runout, loose pilot fit, or driving pins not fully engaged. These are setup issues, not feeds and speeds problems. Correct the setup before adjusting parameters.
Chip packing in blind bore: Most common cause: feed rate too high in steel, or lack of cutting oil. Reduce feed rate, apply cutting oil at the bore entry, and retract periodically to clear chips in deep applications.
Tool stalling or machine tripping: Most common cause: feed rate too high for material, or cutter dull from running at excessive speed. Check cutter condition first. Reduce feed rate and confirm RPM is within the listed range.
When to Contact NMT
The parameters in this table apply to standard NMT keyseat millers in the materials listed. If you’re running an application not covered here — exotic alloys, very deep keyways, small bore applications under ½”, or non-standard geometries — contact us directly. Our engineers can provide specific recommendations for your application and confirm whether the tooling is specified correctly for your material.
Call: 513-541-6682 Email: nationalmachinetoolco@gmail.com
National Machine Tool Co. — Cincinnati, OH — Over 100 years manufacturing custom keyseat millers.