Starting surface speeds
Surface speed depends mainly on the material and the tool. Carbide tolerates much more heat than high-speed steel (HSS), so it runs about two to four times faster. The ranges below are starting points for milling and turning with a rigid setup; go to the low end for light machines, long tools, no coolant or interrupted cuts, and to the high end with coated carbide, flood coolant and a rigid machine.
| Material | HSS | Carbide |
|---|---|---|
| Aluminum alloys | 75 to 100 m/min (245 to 330 SFM) | 180 to 600 m/min (590 to 1970 SFM) |
| Brass (free-cutting) | 45 to 90 m/min (150 to 295 SFM) | 120 to 230 m/min (395 to 755 SFM) |
| Plastics (acetal, nylon, acrylic) | 60 to 150 m/min (195 to 490 SFM) | 150 to 300 m/min (490 to 985 SFM) |
| Mild steel (1018, A36) | 25 to 35 m/min (80 to 115 SFM) | 75 to 150 m/min (245 to 490 SFM) |
| Gray cast iron | 20 to 30 m/min (65 to 100 SFM) | 75 to 150 m/min (245 to 490 SFM) |
| Alloy steel, annealed (4140) | 15 to 25 m/min (50 to 80 SFM) | 60 to 120 m/min (195 to 395 SFM) |
| Stainless steel (304) | 15 to 25 m/min (50 to 80 SFM) | 60 to 120 m/min (195 to 395 SFM) |
| Titanium (Ti-6Al-4V) | 6 to 12 m/min (20 to 40 SFM) | 30 to 60 m/min (100 to 195 SFM) |
- Drills run at the lower end of the HSS range (see Drilling, Reaming, Tapping and Boring), taps at about a third to a half of that.
- Harder or tougher materials (stainless, titanium, hardened steel) need lower speeds; gummy materials (stainless, pure aluminum, copper) need sharp tools and enough feed to avoid rubbing.
- Convert to RPM with n = 1 000 Vc ÷ (π D) (see Cutting Speed, Spindle Speed and Feed Rate).
Starting chip loads
Chip load (feed per tooth) rises with the diameter, because a bigger tool is stiffer and has bigger flutes. The table is for solid carbide end mills with a rigid setup and a moderate radial depth (about half the diameter or more); correct for chip thinning when the stepover is smaller (see Chip Load, Chip Thinning and Engagement). For HSS use about 70 % of these values.
| Material | 3 mm tool | 6 mm tool | 10 mm tool | 12 mm tool | 20 mm tool |
|---|---|---|---|---|---|
| Aluminum | 0.025 mm (0.001 in) | 0.050 mm (0.002 in) | 0.080 mm (0.003 in) | 0.100 mm (0.004 in) | 0.130 mm (0.005 in) |
| Brass (free-cutting) | 0.025 mm (0.001 in) | 0.050 mm (0.002 in) | 0.080 mm (0.003 in) | 0.100 mm (0.004 in) | 0.120 mm (0.005 in) |
| Plastics (acetal, acrylic) | 0.040 mm (0.002 in) | 0.080 mm (0.003 in) | 0.120 mm (0.005 in) | 0.150 mm (0.006 in) | 0.200 mm (0.008 in) |
| Mild steel | 0.020 mm (0.001 in) | 0.040 mm (0.002 in) | 0.060 mm (0.002 in) | 0.070 mm (0.003 in) | 0.090 mm (0.004 in) |
| Alloy steel (4140) | 0.015 mm (0.001 in) | 0.030 mm (0.001 in) | 0.050 mm (0.002 in) | 0.060 mm (0.002 in) | 0.080 mm (0.003 in) |
| Stainless steel (304) | 0.013 mm (0.001 in) | 0.025 mm (0.001 in) | 0.040 mm (0.002 in) | 0.050 mm (0.002 in) | 0.070 mm (0.003 in) |
| Gray cast iron | 0.025 mm (0.001 in) | 0.050 mm (0.002 in) | 0.070 mm (0.003 in) | 0.080 mm (0.003 in) | 0.100 mm (0.004 in) |
| Titanium (Ti-6Al-4V) | 0.010 mm (0.000 in) | 0.020 mm (0.001 in) | 0.030 mm (0.001 in) | 0.040 mm (0.002 in) | 0.055 mm (0.002 in) |
| Hardwood | 0.060 mm (0.002 in) | 0.120 mm (0.005 in) | 0.180 mm (0.007 in) | 0.220 mm (0.009 in) | 0.300 mm (0.012 in) |
- Chip load grows more slowly than the diameter: doubling the diameter raises it by about 50 to 80 %.
- Stay at the middle of the range on a first cut and move up or down by 20 % steps while you watch the chips and listen.
- Short tools (stick-out under 3 × D) take these values; long reach needs a lower chip load (see below).
Adjusting for your setup
| Condition | Speed | Chip load | Reason |
|---|---|---|---|
| Long stick-out (L ÷ D = 4) | × 0.8 | × 0.8 | Deflection grows with L³ (see Cutting Force, Power and Torque) |
| Very long stick-out (L ÷ D = 6) | × 0.6 | × 0.6 | Chatter and breakage risk |
| No coolant | × 0.7 to 0.8 (steels) | × 1 | Heat has nowhere to go (see Coolant, Lubrication and Chip Evacuation) |
| Flood or through-tool coolant | × 1.1 to 1.3 | × 1 | Better heat removal and chip clearing |
| Coated carbide | × 1.2 to 1.4 against uncoated | × 1 | Coating insulates and resists wear (see Tool Materials, Coatings and Geometry) |
| Interrupted cut, casting skin, scale | × 0.7 | × 0.8 | Shock loads chip the edge |
| Light or old machine | × 0.5 to 0.7 | × 0.7 | Limited rigidity and power |
| Harder workpiece (30 HRC against annealed) | × 0.6 | × 0.8 | More heat and force |
| Finishing pass | × 1 to 1.3 | × 0.5 | Light cut for finish; small chip |
Worked example: 304 stainless with a 10 mm four-flute carbide end mill
- Carbide in 304 stainless runs at 60 to 120 m/min; take the middle, 90 m/min. RPM = 1 000 × 90 ÷ (π × 10) = 2 865 rpm. The chip load for a 10 mm tool is about 0.04 mm, so Vf = 2 865 × 4 × 0.04 = 458 mm/min.
- If the tool sticks out 4 diameters, apply the long-reach factor of 0.8 to both: 72 m/min (2 292 rpm) and 0.032 mm per tooth, giving 293 mm/min.
- Stainless work-hardens when the edge rubs, so never lower the feed to “be gentle”: keep the chip load, keep the tool moving, and use coolant.
Worked example: 20 mm three-flute carbide in aluminum on a slow spindle
- At 300 m/min the speed is 4 775 rpm; the machine’s spindle stops at 3 500 rpm, which is 220 m/min (73 % of the target): fine for aluminum.
- The ideal feed rate would be 4 775 × 3 × 0.12 = 1 719 mm/min; at the spindle limit with the same chip load it is 1 260 mm/min (see Cutting Speed, Spindle Speed and Feed Rate).
Worked example: HSS against carbide in mild steel
- An 8 mm two-flute HSS end mill runs at 30 m/min (1 194 rpm) with 0.03 mm per tooth: Vf = 72 mm/min.
- A four-flute carbide tool at 100 m/min (3 979 rpm) and 0.04 mm per tooth feeds at 637 mm/min, about 8.9 times as fast: the cost of the carbide tool is repaid in time on any production job.
Notes by material
| Material | What to watch | Tips |
|---|---|---|
| Aluminum alloys | Gummy chips weld to the edge (built-up edge); chips pack the flutes | Sharp, polished two- or three-flute tools; high speed; air or mist; free-cutting alloys (6061, 7075) cut best |
| Brass and bronze | Free-cutting brass is easy; unleaded and hard bronzes are tougher | Zero or slight negative rake to stop the tool digging in; run dry or with a little oil |
| Plastics | Melting at the edge, stress cracking, burrs | High RPM with a high feed so the chip carries the heat; single-flute O-flute tools; air blast, no coolant on some |
| Mild and alloy steels | Heat and wear at higher speeds | Coated carbide with coolant; avoid dwelling |
| Stainless steel | Work hardening, gummy, heat stays in the tool | Low speed, firm feed, sharp positive tools, coolant; never rub |
| Titanium | Low conductivity: heat stays in the tool; fire risk with fine chips | Low speed, light radial cuts, flood coolant, sharp tools; keep the tool moving |
| Cast iron | Abrasive, fine dust, hard skin | Run dry with air or extraction; cut below the skin |
| Wood and MDF | Burning at too low a feed, fuzzy grain, fine dust | High RPM with a brisk feed; compression or up-cut bits; extraction (see Dust, Fumes and Ventilation) |
| Composites (CFRP, GFRP) | Abrasive fibers, delamination, harmful dust | Diamond-coated or compression tools, sharp edges, extraction and a respirator |
How to use the numbers
- 1. Start from the tool maker’s chart for the exact tool, coating and material; use this page when you have no chart or to cross-check it.
- 2. Calculate the RPM from the surface speed and the diameter, and check it against the spindle limit.
- 3. Choose the chip load from the table, adjust it for the setup and for chip thinning, and calculate the feed rate.
- 4. Check the power (see Cutting Force, Power and Torque) and the tool life (see Tool Life, Wear and Cutting Economics).
- 5. Make the first cut at about 70 % of the feed, listen, look at the chips and the finish, then raise the feed in steps (see Dialling In: Chatter, Rigidity and Troubleshooting).
- 6. Write down what works for each material and tool so that the next job starts from a proven setting. The CNC Feeds and Speeds Calculator does the arithmetic for you.
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Chips weld to the tool (aluminum) | Speed too low, dull edge, not enough flute room | Raise the speed, use a polished sharp tool, add air or mist |
| Stainless work-hardens and the tool dies | Rubbing at a low chip load | Raise the feed, keep cutting, no dwell, use coolant |
| Plastic melts and sticks to the tool | Feed too low for the RPM | Raise the feed so that the chip carries the heat; use air |
| Wood burns | Feed too low, dull bit | Feed faster at the same RPM, sharpen or replace the bit |
| Tool wears out in minutes in steel | Speed too high for the tool material | Reduce the speed 20 to 30 %; use carbide with coating and coolant |
| Numbers from two charts disagree | Different tools, coatings and assumptions | Use the maker’s chart for your tool and begin conservatively |
Related
- Speeds and Feeds: the overview of this guide.
- Cutting Speed, Spindle Speed and Feed Rate: turning speeds into RPM and feeds.
- Tool Materials, Coatings and Geometry: what the tool is made of and coated with.
- CNC Feeds and Speeds Calculator and Machining Metals and Machining Plastics, Wood and Composites.
FAQ
What speed should I run carbide in steel?
About 75 to 150 m/min (250 to 500 SFM) for mild steel, lower for alloy and stainless steels (60 to 120 m/min); use the tool maker’s data for the exact value.
What chip load should I use for a 6 mm end mill?
About 0.05 mm per tooth in aluminum, 0.04 mm in mild steel and 0.025 mm in stainless, for carbide in a rigid setup; adjust for stepover and reach.
Why do charts differ?
Tool material, coating, geometry, coolant and machine rigidity all change the right numbers; charts are written for different conditions.
Should I run HSS faster than the chart if the machine allows?
No: HSS is limited by heat, not by the spindle; raising the speed shortens its life dramatically.
References
- Oberg, E., et al., Machinery’s Handbook (cutting speeds, feeds and recommended practice for each material).
- Tool makers’ catalogs (Harvey Tool, Sandvik Coromant, Kennametal, OSG) for chip loads and speeds of specific tools.
- Smith, G. T., Cutting Tool Technology, Springer (materials and their machinability).
Last reviewed: October 2026. All values are typical starting points; the maker’s data for your tool takes priority.