Machinery's Handbook, 31st Edition
1132 SPEEDS AND FEEDS FOR DRILLING, REAMING, THREADING Indexable Insert Drilling: The feed/speed data for indexable insert drilling are based on a tool with two cutting edges, an insert nose radius of 3 ∕ 64 inch (1.2 mm), a 10-degree lead angle, and diameter D = 1 inch (2.54 mm). Adjustments to cutting speed for feed and depth of cut are made using Table 5a on page 1103 (Adjustment Factors) using a depth of cut of D ⁄2, or one-half the drill diameter. Expected tool life at the given speeds and feeds is approximately 15 minutes for short hole drilling (i.e., where maximum hole depth is about 2 D or less). Speed adjustment factors to increase tool life are found in Table 5b. Tapping and Threading: The data in this column are intended for use with thread chasers and for tapping. The feed used for tapping and threading must be equal to the lead (feed = lead = pitch) of the thread being cut. The two feed/speed pairs given for each material, therefore, are representative speeds for two thread pitches, 12 and 50 threads per inch (1 ∕ 0.083 = 12, and 1 ∕ 0.020 = 50). Tool life is expected to be approximately 45 minutes at the given speeds and feeds. When cutting fewer than 12 threads per inch (pitch ≥ 0.08 inch or 2.1 mm), use the lower ( optimum ) speed; for cutting more than 50 threads per inch (pitch ≤ 0.02 inch or 0.51 mm), use the larger ( average ) speed; and, in the intermediate range between 12 and 50 threads per inch, interpolate between the given average and optimum speeds. The combined feed/speed data in this table are based on tool grades (identified in Table 16) as follows: coated carbide = 10. Example 2, Drilling: If the 1120 steel of Example 1 is to be drilled with a 0.60-inch drill at a feed of 0.012 in/rev, what is the cutting speed in ft/min? Also, what spindle rpm of the drilling machine is required to obtain this cutting speed? To find the feed factor F d in Table 22, calculate the ratio of the desired feed to the opti mum feed and the ratio of the two cutting speeds given in the speed tables. The desired feed is 0.012 in/rev and the optimum feed, as explained above is 0.016 in/rev, therefore, feed/ f opt = 0.012 ∕ 0.016 = 0.75 and V avg / V opt = 95 ∕ 50 = 1.9, approximately 2. The feed factor F f is found at the intersection of the feed ratio row and the speed ratio column. F f = 1.40 corresponds to about halfway between 1.31 and 1.50, which are the feed factors that correspond to V avg / V opt = 2.0 and feed/ f opt ratios of 0.7 and 0.8, respectively. F d , the diameter factor, is found on the same row as the feed factor (halfway between the 0.7 and 0.8 rows, for this example) under the column for drill diameter = 0.60 inch. Because the speed table values are based on a 0.60-inch drill diameter, F d = 1.0 for this example, and the cutting speed is V = V opt 3 F f 3 F d = 50 3 1.4 3 1.0 = 70 ft/min. The spindle speed in rpm is N = 12 3 V /( π 3 D ) = 12 3 70/(3.14 3 0.6) = 445 rpm. Example 3, Drilling: Using the same material and feed as in the previous example, what cutting speeds are required for 0.079-inch and 4-inch diameter drills? What machine rpm is required for each? Because the feed is the same as in the previous example, the feed factor is F f = 1.40 and does not need to be recalculated. The diameter factors are found in Table 22 on the same row as the feed factor for the previous example (about halfway between the diameter fac tors corresponding to feed/ f opt values of 0.7 and 0.8) in the column corresponding to drill diameters 0.079 and 4.0 inches, respectively. Results of the calculations are summarized below. Drill diameter = 0.079 inch Drill diameter = 4.0 inches F f = 1.40 F f = 1.40 F d = (0.34 + 0.38)⁄2 = 0.36 F d = (1.95 + 1.73)⁄2 = 1.85 V = 50 3 1.4 3 0.36 = 25.2 fpm V = 50 3 1.4 3 1.85 = 129.5 fpm 12 3 25.2/(3.14 3 0.079) = 1219 rpm 12 3 129.5/(3.14 3 4) = 124 rpm
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online