Speed & Feed Recommendations
Severance RPM chart for Midget Mills, countersink speeds and feeds, and the RPM formula
The RPM Formula
The correct spindle speed for any rotary cutting tool is calculated from the recommended Surface Feet per Minute (SFM) and the tool diameter:
RPM = SFM × 3.82 ÷ Tool Diameter (inches)
Where 3.82 is the constant derived from 12 / π (converting feet to inches and accounting for circumference). This formula applies to all rotary cutting tools including Midget Mills, Junior Mills, Lab Mills, countersinks, and Carbo-Mills.
Important: These are starting recommendations. Adjust based on your specific setup, rigidity, coolant availability, and desired finish. When in doubt, start slower and increase speed gradually.
Quick Reference
- Carbide Midget Mills: 1/4″ at 7,500 RPM in steel, 30,000 in aluminum (chart)
- HSS Midget Mills: about half the carbide speed
- HSS Countersinks: 70-100 SFM in mild steel
- Carbide Countersinks: 80-170 SFM in mild steel
- Countersinks in other materials: see the catalog countersink chart
Rotary File Speeds
Recommended Operating Speeds for Carbide Midget Mills®
No hard and fast rule can be laid down: operating conditions vary greatly, and experience must guide the operator to the most economical speed for their skill and technique. For abrasive conditions, reduce speed. These figures are given only as a general guide.
| Cutter Dia. | Aluminum, Magnesium, Brass (RPM) | Cast Iron (RPM) | Steel (RPM) |
|---|---|---|---|
| 1/8" | 40,000 | 15,000 | 10,000 |
| 1/4" | 30,000 | 11,200 | 7,500 |
| 3/8" | 25,000 | 9,300 | 6,200 |
| 1/2" | 20,000 | 7,400 | 5,000 |
| 3/4" | 15,000 | 5,500 | 3,700 |
| 1" | 10,000 | 3,600 | 2,500 |
HSS Midget Mills: reduce these speeds by about half. For example, a 1/4″ HSS Midget Mill in steel runs at about 3,750 RPM. For other carbide rotary files, or a recommendation on a specific job, contact Severance.
High Speed Steel
HSS rotary files are better for less rigid, hand operations where some chatter is likely, and they take more shock than carbide. Run them at about half the speed of a carbide tool of the same diameter.
Carbide
Carbide rotary files are for rigid setups where chatter is minimized and tool control is high. The catalog says carbide may be operated at many times the speed of steel tools and generally yields as much as five to ten times the service life.
Which Tool for Which Material
The catalog matches each tooth pattern to the materials it cuts best:
| Tool | Tooth Pattern | Works Best On |
|---|---|---|
| HSS Midget Mills® | Right hand spiral with a light chipbreaker | Non-work hardening materials: M2, M42, cold and hot rolled steels, aluminum, cast iron and bronze |
| Carbide Midget Mills® | Right hand spiral with deep radial flutes, mainly for machine use | Carbon steels, cast steels, gray irons, some stainless steels, tungsten and nickel alloys |
| Carbo-Mills™ | Double cut, for substantial stock removal with a rough to medium finish | Ferrous, non-work hardening materials: steels, aluminum, cast iron and bronze |
| Sever-Cuts™ | Super coarse cut that removes material without loading up, for hand or machine use | Nonferrous materials: aluminum, copper, bronze, nickel and magnesium |
Bore Mills™ are the one rotary file with a stated speed: they are run at the same speeds and feeds as the mounted grinding wheels they replace.
Recommended Countersink Speeds and Feeds
Countersinks run slower than rotary files to keep control and leave a clean, chatter-free seat. This chart is from page 87 of the Severance catalog and covers HSS and carbide countersinks in 19 workpiece materials.
| Material | Feed per Tooth (FPT) | HSS Speed (SFM) | Carbide Speed (SFM) |
|---|---|---|---|
| Aluminum / Aluminum Alloys | .001-.002 | 150-250 | 300-500 |
| Brass / Bronze | .001-.002 | 75-125 | 150-250 |
| Iron, Cast (Soft) | .001-.002 | 75-125 | 125-225 |
| Iron, Cast (Medium Hard) | .001-.002 | 50-100 | 100-175 |
| Iron, Malleable | .001-.002 | 80-90 | 90-150 |
| Magnesium / Magnesium Alloys | .001-.002 | 125-250 | 250-400 |
| High Nickel Steel | .001-.002 | 30-50 | 50-75 |
| Plastic, Bakelite | .001-.002 | 100-250 | 250-400 |
| Steel, Mild | .001-.002 | 70-100 | 80-170 |
| Steel, Tool | .001-.002 | 50-60 | 60-100 |
| Steel, Forgings | .001-.002 | 40-50 | 50-80 |
| Steel, Alloy (300-400 Brinell) | .001-.002 | 20-30 | 30-50 |
| Steel, High Tensile (35-45 Rc) | .001-.002 | 25-40 | 35-60 |
| Steel, High Tensile (45-50 Rc) | .001-.002 | 15-25 | 25-40 |
| Steel, High Tensile (50-55 Rc) | .001-.002 | 7-15 | 15-20 |
| Stainless Steel (Free Machining) | .001-.002 | 30-80 | 80-125 |
| Stainless Steel (Work Hardening) | .001-.002 | 15-50 | 50-75 |
| Inconel Alloy, Hastelloy Wrought | .001-.002 | 15-20 | 25-35 |
| Hastelloy (Cast) | .001-.002 | 5-7 | 7-15 |
RPM = SFM × 3.82 ÷ Cutter O.D.
IPR = FPT × Number of Teeth
IPM = IPR × RPM
IPR = FPT × Number of Teeth
IPM = IPR × RPM
These surface speeds are a guide. Good quality cutting fluid is recommended. For help with a specific job, call 989-777-5500.
Countersink RPM by Body Diameter
RPM worked out from the chart above for the most common materials, rounded to the nearest 10. For any other size or material, use the RPM formula with the catalog surface speed.
| Body Diameter | Mild Steel | Aluminum | Stainless, Free Machining |
Stainless, Work Hardening |
Cast Iron, Soft |
|---|---|---|---|---|---|
| 1/4" (0.250") | HSS 1,070-1,530 Carbide 1,220-2,600 |
HSS 2,290-3,820 Carbide 4,580-7,640 |
HSS 460-1,220 Carbide 1,220-1,910 |
HSS 230-760 Carbide 760-1,150 |
HSS 1,150-1,910 Carbide 1,910-3,440 |
| 3/8" (0.375") | HSS 710-1,020 Carbide 810-1,730 |
HSS 1,530-2,550 Carbide 3,060-5,090 |
HSS 310-810 Carbide 810-1,270 |
HSS 150-510 Carbide 510-760 |
HSS 760-1,270 Carbide 1,270-2,290 |
| 1/2" (0.500") | HSS 530-760 Carbide 610-1,300 |
HSS 1,150-1,910 Carbide 2,290-3,820 |
HSS 230-610 Carbide 610-960 |
HSS 110-380 Carbide 380-570 |
HSS 570-960 Carbide 960-1,720 |
| 5/8" (0.625") | HSS 430-610 Carbide 490-1,040 |
HSS 920-1,530 Carbide 1,830-3,060 |
HSS 180-490 Carbide 490-760 |
HSS 90-310 Carbide 310-460 |
HSS 460-760 Carbide 760-1,380 |
| 3/4" (0.750") | HSS 360-510 Carbide 410-870 |
HSS 760-1,270 Carbide 1,530-2,550 |
HSS 150-410 Carbide 410-640 |
HSS 80-250 Carbide 250-380 |
HSS 380-640 Carbide 640-1,150 |
| 1" (1.000") | HSS 270-380 Carbide 310-650 |
HSS 570-960 Carbide 1,150-1,910 |
HSS 110-310 Carbide 310-480 |
HSS 60-190 Carbide 190-290 |
HSS 290-480 Carbide 480-860 |
Feed Rate Guidelines
Rotary Files (Hand-Held / Die Grinder)
When using rotary files in a hand-held die grinder or flexible shaft tool, feed is controlled by the operator's hand pressure. Follow these principles:
- Let the tool do the work. Excessive pressure causes premature dulling, overheating, and poor finish.
- Use a brushing motion. Move the tool across the workpiece rather than pressing it into one spot.
- Maintain consistent movement. Dwelling in one area causes localized overheating and uneven stock removal.
- Listen to the tool. A high-pitched whine means too much pressure. A smooth, consistent hum indicates proper feed.
Countersinks (Machine / Drill Press)
When using countersinks in a drill press or CNC machine, use these feed rate starting points:
- Hand feed (drill press): Slow, steady advancement. Let the tool cut without forcing.
- CNC feed: 0.001-0.002" per tooth in every material on the catalog chart. Multiply by the number of flutes for feed per revolution (IPR), then by RPM for inches per minute (IPM). A 1/2" six-flute HSS countersink in mild steel at 70 SFM turns about 530 RPM, feeds 0.006-0.012" per revolution, and advances about 3.2-6.4 inches per minute.
- Peck cycle: For deep countersinks, use a peck cycle to clear chips and reduce heat.
- Chatterless advantage: Severance Chatterless Countersinks can run at higher feeds than conventional countersinks due to their 6-flute unequal-spacing design.
CNC-K™ Countersink Programming
CNC-K™ Precision Countersinks are made for NC, CNC, and preset machine tools. They have Chatterless™ tooth geometry, and tight tolerances on angle, diameter, and length make them accurate to set. They come in 30°, 41°, 45°, 50°, 55°, and 60° centerline angles (60°, 82°, 90°, 100°, 110°, and 120° included). Other angles and sizes are available on request.
At any depth, the countersink diameter grows in direct ratio to the depth. As the tool travels in the (A) direction along its axis, (X) grows by the tangent of the centerline angle (K), so tan K = X ÷ A. The angle opens on both sides of the drilled hole, so the ratio (R) is 2 × tan K.
| Angle (K) | Included | Ratio (R) |
|---|---|---|
| 30° | 60° | 1.15 |
| 41° | 82° | 1.74 |
| 45° | 90° | 2.00 |
| 50° | 100° | 2.38 |
| 55° | 110° | 2.86 |
| 60° | 120° | 3.46 |
Calculations
- Cut diameter: C = H + (R × A)
- Depth of cut: A = (C − H) ÷ R
- Stroke: S = (C − D) ÷ R
- Wall width: X = (C − H) ÷ 2
Example: countersink a 0.500" hole to a 0.875" cut diameter at 41° (82° included) with a CNC-K-1 (1" body, 0.203" nose). Depth of cut A = (0.875 − 0.500) ÷ 1.74 = 0.216". Stroke S = (0.875 − 0.203) ÷ 1.74 = 0.386".
Tips for Maximum Tool Life
Do
- Run at the recommended RPM for your tool diameter and material.
- Use cutting fluid on steel, stainless, and titanium.
- Keep the tool moving across the work surface.
- Select the right tool material (HSS or Carbide) for the job.
- Inspect tools regularly for wear, chipping, or loading.
- Store tools properly to protect cutting edges.
- Send worn tools for regrinding rather than discarding them.
Don't
- Don't exceed the maximum recommended RPM—it generates excessive heat.
- Don't use excessive pressure—it dulls tools prematurely.
- Don't dwell in one spot—it causes overheating and work hardening.
- Don't use HSS on hardened steels above Rc 45—switch to Carbide.
- Don't run Carbide at low speeds with interrupted cuts—it causes chipping.
- Don't use water-based coolant on cast iron (use dry or air blast).
- Don't use a worn tool thinking you'll save money—it produces poor results and damages workpieces.
When to Use Cutting Fluid
| Material | Cutting Fluid? | Recommended Type |
|---|---|---|
| Aluminum | Optional (helps prevent loading) | Wax stick, light oil, or WD-40 |
| Mild Steel | Recommended | Soluble oil, cutting oil, or sulfurized oil |
| Stainless Steel | Required | Heavy-duty cutting oil or sulfurized/chlorinated oil |
| Cast Iron | Not recommended | Dry cutting or air blast preferred |
| Brass / Bronze | Optional | Light oil or dry |
| Tool Steel | Required | Heavy-duty cutting oil |
| Titanium | Required (flood) | Water-soluble coolant at high flow |
| Plastics | Not recommended | Dry or air blast (fluid may damage some plastics) |