공구강 참조 데이터

Cutting Speeds for Tool Steels

High speed steel cutting speeds for the tool steel grades, by hardness, for turning, milling, drilling and reaming, with the factors that trade speed against 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: 냉간 작업, 뜨거운 작업 그리고 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.

등급	상태	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
오1, O2, O6, O7	175–225 Bhn	70	50	45	30
Cold work, high carbon high chromium
디2, 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
에이7	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
금형강
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, 엠2, 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.

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 gain in life costs about half the speed in face milling.

Factor tables as printed, all three feed columns shown; the chart plots the medium feed column.

Tool life, min	up to 300 Bhn: small	중간	large	over 300 Bhn: small	중간	large	mixed ceramics: small	중간	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 per cent of the tabulated speed.

Tool life, min	face milling: small	중간	large	end milling: small	중간	large	drilling: small	중간	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 that should be used 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 inch. For other feeds and depths the source carries a further 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 the drilling speed with the diameter factors of Table 22, and the life of drills, reamers and taps with 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 the UNC, UNF and metric threads are on the tap drill size chart, and the finish each operation leaves is on the surface roughness chart.
Machine the steel as it comes from the mill: the speeds change with the condition of the material. The machinability ratings compare the grades against a 100 per cent baseline, and the machining allowance chart covers the stock left on for the finishing cuts. Grade by grade, the properties chart lists the hardness each family is supplied in.

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 carries a higher speed, and worn holders, thin sections and long overhangs are the usual reasons a speed from the table has to come down.

The longer the tool life asked of the cut, the lower the speed that reaches it, and the two are linked by the line in the chart above rather than by a fixed percentage. See the note below for what those fits say about the tool steel classes.

Cutting Speeds for Tool Steels

Using the speeds

관련 참조 페이지