Cutting Speeds for Tool Steels
High-speed steel cutting speeds for tool steel grades, by hardness, for turning, milling, drilling, and reaming, with factors that trade speed for tool life. Speeds are in feet per minute (fpm), as published in the Handbook speed and feed tables.
High speed steel cutting speeds by grade
A working set of high-speed steel speeds for the common tool steel families: cold work, hot work, and high-speed grades, from the traditional speed columns of the Handbook turning, milling, and drilling tables, brought into one comparison. The carbide speeds for the same grades run several times higher in the source tables.
| Grade | Condition | Turning, fpm | Milling, fpm | Drilling, fpm | Reaming, fpm |
|---|---|---|---|---|---|
| Water hardening | |||||
| W1, W2, W5 | 150–200 Bhn | 100 | 85 | 85 | 55 |
| Shock resisting | |||||
| S1, S2, S5, S6, S7 | 175–225 Bhn | 70 | 55 | 50 | 35 |
| Cold work, oil hardening | |||||
| O1, O2, O6, O7 | 175–225 Bhn | 70 | 50 | 45 | 30 |
| Cold work, high carbon high chromium | |||||
| D2, D3, D4, D5, D7 | 200–250 Bhn | 45 | 40 | 30 | 20 |
| Cold work, air hardening | |||||
| A2, A3, A8, A9, A10 | 200–250 Bhn | 70 | 50 | 50 | 35 |
| A4, A6 | 200–250 Bhn | 55 | 45 | 45 | 30 |
| A7 | 225–275 Bhn | 45 | 40 | 30 | 20 |
| Hot work, chromium type | |||||
| H10, H11, H12, H13, H14, H19 | 150–200 Bhn | 80 | 60 | 60 | 40 |
| 200–250 Bhn | 65 | 50 | 50 | 30 | |
| 325–375 Bhn | 50 | 30 | 30 | 20 | |
| 48–50 HRC | 20 | n/a | n/a | n/a | |
| 50–52 HRC | 10 | n/a | n/a | n/a | |
| 52–56 HRC | n/a | n/a | n/a | n/a | |
| Hot work, tungsten type | |||||
| H21, H22, H23, H24, H25, H26 | 150–200 Bhn | 60 | 55 | 55 | 35 |
| 200–250 Bhn | 50 | 45 | 40 | 25 | |
| Hot work, molybdenum type | |||||
| H41, H42, H43 | 150–200 Bhn | 55 | 55 | 45 | 30 |
| 200–250 Bhn | 45 | 45 | 35 | 20 | |
| Low alloy, special purpose | |||||
| L2, L3, L6 | 150–200 Bhn | 75 | 65 | 60 | 40 |
| Mold steels | |||||
| P2, P3, P4, P5, P6, P21, P26 | 100–150 Bhn | 90 | 75 | 75 | 50 |
| 150–200 Bhn | 80 | 60 | 60 | 40 | |
| High speed steels | |||||
| M1, M2, M6, M10, T1, T2, T6 | 200–250 Bhn | 65 | 50 | 45 | 30 |
| M3-1, M4, M7, M30, M33, M34, M36, M41, M42, M43, M44, M46, M47, T5, T8 | 225–275 Bhn | 55 | 40 | 35 | 20 |
| T15, M3-2 | 225–275 Bhn | 45 | 30 | 25 | 15 |
Reaming runs at roughly two-thirds of the drilling speed; threading in these grades is done at the lowest speed of all, as noted on the tap drill chart below. n/a means the source gives no speed for that condition, because those hardnesses are worked by grinding or EDM instead.
Cutting speeds reference card, printable PDF
Two A4 pages with cutting speeds for common tool steel families, tool life factors for turning, milling, and drilling, and our contact details.
Adjusting the speed for a longer tool life
The table speeds carry one tool life: about 15 minutes of cutting for the turning tables and about 45 minutes for milling and drilling. To trade speed for a longer life, multiply the tabulated speed by the factor for the life you want: at 45 minutes the turning speed falls to about four-fifths, and at 180 minutes to about two-thirds. Milling loses speed faster, so the same life gain costs about half the speed in face milling.
Turning, base 15 min multiply the tabulated speed, carbide up to 300 Bhn small feed medium feed large feed 15 45 90 180 0.5 0.6 0.7 0.8 0.9 1 tool life, minutes (log scale) factor from Table 5b, the factor table below Milling and drilling, base 45 min multiply the tabulated speed, coated carbide face milling end milling drilling 15 45 90 180 0.5 0.75 1 1.25 1.5 1.75 tool life, minutes (log scale) factor from Table 15e, the factor table below Values as printed in Machinery’s Handbook, Tables 5b and 15e, medium feed column. The lines are drawn through the four tabulated tool lives.
Factor tables as printed, all three feed columns shown; the chart plots the medium feed column.
| Tool life, min | up to 300 Bhn: small | medium | large | over 300 Bhn: small | medium | large | mixed ceramics: small | medium | large |
|---|---|---|---|---|---|---|---|---|---|
| 15 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 |
| 45 | 0.86 | 0.81 | 0.76 | 0.80 | 0.75 | 0.70 | 0.89 | 0.87 | 0.84 |
| 90 | 0.78 | 0.71 | 0.64 | 0.70 | 0.63 | 0.56 | 0.82 | 0.79 | 0.75 |
| 180 | 0.71 | 0.63 | 0.54 | 0.61 | 0.53 | 0.45 | 0.76 | 0.72 | 0.67 |
Tool life factors for turning, Table 5b. The base speed is the tabulated turning speed for the grade (15-minute tool life), so the factor at 45 minutes, 0.81, should be read as 81 percent of the tabulated speed.
| Tool life, min | face milling: small | medium | large | end milling: small | medium | large | drilling: small | medium | large |
|---|---|---|---|---|---|---|---|---|---|
| 15 | 1.69 | 1.78 | 1.87 | 1.10 | 1.23 | 1.35 | 1.11 | 1.21 | 1.30 |
| 45 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 | 1.00 |
| 90 | 0.72 | 0.70 | 0.67 | 0.94 | 0.89 | 0.83 | 0.93 | 0.89 | 0.85 |
| 180 | 0.51 | 0.48 | 0.45 | 0.69 | 0.69 | 0.69 | 0.87 | 0.80 | 0.72 |
Tool life factors for milling and drilling, Table 15e. Here, the base speed is the tabulated speed for the operation (45-minute tool life), so the factor at 180 minutes (0.48 for face milling) is the speed you should use to reach that life.
- The turning speeds for high-speed steel tools assume a feed of 0.012 in./rev and a depth of cut of 0.125 in. For other feeds and depths, the source includes an additional factor table, Table 5c.
- Milling speeds are based on a tool life of about 45 minutes for all tabulated values; the end milling data assume a 3-tooth cutter of 1 inch diameter, and the face milling data a 10-tooth, 8 inch face mill. Adjust for other cutter feeds and depths with Tables 15b and 15c.
- Drilling and reaming speeds also carry a tool life of about 45 minutes. For other drill diameters and feeds, the source adjusts drilling speed using the diameter factors in Table 22 and the life of drills, reamers, and taps in Table 15e, as tabulated above.
- The Handbook pairs each speed column with an optimum feed for the cut, in combined feed and speed sets given as fractions such as 16/50, feed over speed. This page carries the traditional speed columns; for the combined sets use the source tables directly.
- Tapping runs at the lowest speed of any of these operations because the tap is fully engaged in the cut. Tap drill sizes for UNC, UNF, and metric threads are in the tap drill size chart, and the finish each operation leaves is in the surface roughness chart.
- Machine the steel as it comes from the mill: speeds change with the material condition. The machinability ratings compare the grades against a 100 percent baseline, and the machining allowance chart covers the stock left on for the finishing cuts. Grade by grade, the properties chart lists the hardness in which each family is supplied.
Using the speeds
A speed from a table is a starting value. Run it, watch the chip and the finish, and move from there: a heavier, more rigid machine can take a higher speed, and worn holders, thin sections, and long overhangs usually require reducing the table speed.
The longer the tool life required for the cut, the lower the speed that reaches it, and the chart above links the two rather than a fixed percentage. See the note below for what those fits say about the tool steel classes.
Related reference pages
- D2 tool steel machining guide
- H13 tool steel machinability
- Selection guide for high speed steel cutting tools
- Tapping tool steel by hardness
- Drilling hardened tool steel
- Tool steel band sawing speeds
Source: Machinery’s Handbook 28th Edition (Industrial Press), Speeds and Feeds section: traditional HSS speed columns of the turning tables (Tables 1 to 9), the milling tables (Tables 10 to 14), and the drilling and reaming tables (Tables 17 to 23), with the tool life adjustment factors of Table 5b and Table 15e. Speeds are in feet per minute (fpm).