Machinery's Handbook, 31st Edition
1094 SPEEDS AND FEEDS FOR TURNING Speeds and Feeds Tables for Turning.— Speeds for HSS (high-speed steel) tools are based on a feed of 0.012 inch/rev and a depth of cut of 0.125 inch; use Table 5c to adjust the given speeds for other feeds and depths of cut. The combined feed/speed data in the remaining columns are based on a depth of cut of 0.1 inch, lead angle of 15 degrees, and nose radius of 3 ∕ 64 inch. Use Table 5a to adjust given speeds for other feeds, depths of cut, and lead angles; use Table 5b to adjust given speeds for increased tool life up to 180 min utes. Examples are given in the text. Examples Using the Speeds and Feeds Tables for Turning: The examples that follow give instructions for determining cutting speeds for turning. In general, the same methods are also used to find cutting speeds for milling, drilling, reaming, and threading, so reading through these examples may bring some additional insight to those other metalworking processes as well. The first step in determining cutting speeds is to locate the work material in the left column of the appropriate table for turning, milling, or drilling, reaming, and threading. Example 1, Turning: Find the cutting speed for turning SAE 1074 plain carbon steel of 225 to 275 BHN (Brinell Hardness Number), using an uncoated carbide insert, a feed of 0.015 in/rev, and a depth of cut of 0.1 inch. In Table 1, speed and feed data for two types of uncoated carbide tools are given, one for hard tool grades, the other for tough tool grades. In general, use the speed data from the tool category that most closely matches the tool to be used because there are often significant differences in the speeds and feeds for different tool grades. From the uncoated carbide hard grade values, the optimum and average feed/speed data given in Table 1 are 17 ∕ 615 and 8 ∕ 815, or 0.017 in/rev at 615 ft/min and 0.008 in/rev at 815 ft/min. Because the selected feed (0.015 in/rev) is different from either of the feeds given in the table, the cutting speed must be adjusted to match the feed. The other cutting parameters to be used must also be compared with the general tool and cutting parameters given in the speed tables to determine if adjustments need to be made for these parameters as well. The general tool and cutting parameters for turning, given in the footnote to Table 1, are depth of cut = 0.1 inch, lead angle = 15 ° , and tool nose radius = 3 ∕ 64 inch. Table 5a is used to adjust the cutting speeds for turning (from Table 1 through Table 9) for changes in feed, depth of cut, and lead angle. The new cutting speed V is found from V = V opt 3 F f 3 F d , where V opt is the optimum speed from the table (always the lower of the two speeds given), and F f and F d are the adjustment factors from Table 5a for feed and depth of cut, respectively. To determine the two factors F f and F d , calculate the ratio of the selected feed to the optimum feed, 0.015 ∕ 0.017 = 0.9, and the ratio of the two given speeds V avg and V opt , 815 ∕ 615 = 1.35 (approximately). The feed factor F f = 1.07 is found in Table 5a at the intersection of the feed ratio row and the speed ratio column. The depth-of-cut factor F d = 1.0 is found in the same row as the feed factor in the column for depth of cut = 0.1 inch and lead angle = 15 ° , or for a tool with a 45 ° lead angle, F d = 1.18. The final cutting speed for a 15 ° lead angle is V = V opt 3 F f 3 F d = 615 3 1.07 3 1.0 = 658 fpm. Notice that increasing the lead angle tends to permit higher cutting speeds; such an increase is also the general effect of increasing the tool nose radius, although nose radius correction factors are not included in this table. Increasing lead angle also increases the radial pressure exerted by the cutting tool on the workpiece, which may cause unfavorable results on long, slender workpieces. Example 2, Turning: For the same material and feed as the previous example, what is the cutting speed for a 0.4-inch depth of cut and a 45 ° lead angle? As before, the feed is 0.015 in/rev, so F f is 1.07, but F d = 1.03 for depth of cut equal to 0.4 inch and a 45 ° lead angle. Therefore, V = 615 3 1.07 3 1.03 = 676 fpm. Increasing the lead angle from 15 ° to 45 ° permits a much greater (four times) depth of cut, at the same feed and nearly constant speed. Tool life remains constant at 15 minutes. (Continued on page 1104)
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online