Machinery's Handbook, 31st Edition
1128 SPEEDS AND FEEDS FOR DRILLING, REAMING, THREADING Using the Speeds and Feeds Tables for Drilling, Reaming, and Threading.— The first two speed columns in Table 17 through Table 23 give traditional Handbook speeds for drilling and reaming. The following material can be used for selecting feeds for use with the traditional speeds. The remaining columns in Table 17 through Table 23 contain combined feed/speed data for drilling, reaming, and threading, organized in the same manner as in the turning and milling tables. Operating at the given speeds and feeds is expected to result in a tool life of approximately 45 minutes, except for indexable insert drills, which have an expected tool life of approximately 15 minutes per edge. Examples of using this data follow. Adjustments to HSS drilling speeds for feed and diameter are made using Table 22; Table 5a is used for adjustments to indexable insert drilling speeds, where one-half the drill diameter D is used for the depth of cut. Tool life for HSS drills, reamers, and thread chasers and taps may be adjusted using Table 15e and for indexable insert drills using Table 5b. The feed for drilling is governed primarily by the size of the drill and by the material to be drilled. Other factors that also affect selection of the feed are the workpiece configuration, the rigidity of the machine tool and the workpiece setup, and the length of the chisel edge. A chisel edge that is too long will result in a very significant increase in the thrust force, which may cause large deflections to occur on the machine tool and drill breakage. For ordinary twist drills, the feed rate used is given in the table that follows. For addi tional information also see the table Approximate Cutting Speeds and Feeds for Standard Automatic Screw Machine Tools—Brown and Sharpe on page 1235. Feet Rate for Twist Drills Drill Size, inch (mm) Feed Rate, inch/rev (mm/rev) smaller than 1 ∕ 8 inch (3.175 mm) 0.001 to 0.003 in/rev (0.025–0.08 mm/rev) from 1 ∕ 8 - to 1 ∕ 4 -inch (3.175–6.35 mm) 0.002 to 0.006 in/rev (0.05–0.15 mm/rev) from 1 ∕ 4 - to 1 ∕ 2 -inch (6.35–12.7 mm) 0.004 to 0.010 in/rev (0.10–0.25 mm/rev) from 1 ∕ 2 - to 1-inch (12.7–25.4 mm) 0.007 to 0.015 in/rev (0.18–0.38 mm/rev) larger than 1 inch (25.4 mm) 0.010 to 0.025 in/rev (0.25–0.64 mm/rev) The lower values in the feed ranges should be used for hard materials such as tool steels, super alloys, and work-hardening stainless steels; the higher values in the feed ranges should be used to drill soft materials such as aluminum and brass. Example 1, Drilling: Determine the cutting speed and feed for use with HSS drills in drilling 1120 steel. Table 17 gives two sets of speed and feed parameters for drilling 1120 steel with HSS drills. These sets are 16 ∕ 50 and 8 ∕ 95, i.e., 0.016 in/rev feed at 50 ft/min and 0.008 in/rev at 95 fpm, respectively. These feed/speed sets are based on a 0.6-inch diameter drill. Tool life for either of the given feed/speed settings is expected to be approximately 45 minutes. For different feeds or drill diameters, the cutting speeds must be adjusted and can be determined from V = V opt 3 F f 3 F d , where V opt is the minimum speed for this material given in the speed table (50 fpm in this example) and F f and F d are the adjustment factors for feed and diameter, respectively, found in Table 22.
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online