Machinery's Handbook, 31st Edition
SPEEDS AND FEEDS FOR MILLING 1109 be large enough to allow each cutting edge on the cutter to penetrate below the work- hardened layer produced by the previous cutting edge. The heavy feeds recommended for face milling cutters are to be used primarily with larger cutters on milling machines having an adequate amount of power. For smaller face milling cutters, start with smaller feeds and increase as indicated by the performance of the cutter and the machine. When planning a milling operation that requires a high cutting speed and a fast feed, always check to determine if the power required to take the cut is within the capacity of the milling machine. Excessive power requirements are often encountered when milling with cemented carbide cutters. The large metal removal rates that can be attained require a high horsepower output. An example of this type of calculation is given in the section on Machining Power that follows this section. If the size of the cut must be reduced in order to stay within the power capacity of the machine, start by reducing the cutting speed rather than the feed in inches per tooth. The formula for calculating the table feed rate, when the feed in inches per tooth is known, is as follows: f f nN m t t = where f m = milling machine table feed rate in inches per minute (ipm) f t = feed in inch per tooth (ipt) n t = number of teeth in the milling cutter N = spindle speed of the milling machine in revolutions per minute (rpm) Example: Calculate the feed rate for milling a piece of AISI 1040 steel having a hardness of 180 BHN. The cutter is a 3-inch diameter high-speed steel plain or slab milling cutter with 8 teeth. The width of the cut is 2 inches, the depth of cut is 0.062 inch, and the cutting speed from Table 11 is 85 fpm. From Table 15a, the feed rate selected is 0.008 inch per tooth. . . N D V f f n N 12 314 3 12 85 108 0008 8 108 # # # # = rpm m t t = Example 1, Face Milling: Determine the cutting speed and machine operating speed for face milling an aluminum die casting (alloy 413) using a 4-inch polycrystalline diamond cutter, a 3-inch width of cut, a 0.10-inch depth of cut, and a feed of 0.006 inch/tooth. Table 10 gives the speeds and feeds for milling aluminum alloys. The feed/speed pairs for face milling die-cast alloy 413 with polycrystalline diamond (PCD) are 8 ∕ 2320 (0.008 in/tooth feed at 2320 fpm) and 4 ∕ 4755 (0.004 in/tooth feed at 4755 fpm). These speeds are based on an axial depth of cut of 0.10 inch, an 8-inch cutter diameter D , a 6-inch radial depth (width) of cut ar , with the cutter approximately centered above the workpiece, i.e., eccentricity is low, as shown in Fig. 3. If the preceding conditions apply, the given speeds and feeds can be used without adjustment for a 45-minute tool life. The given speeds are valid for all cutter diameters if a radial depth of cut to cutter diameter ratio ( ar / D ) of 3 ∕ 4 is maintained (i.e., 6 ∕ 8 = 3 ∕ 4 ). However, if a different feed or axial depth of cut is required, or if the ar / D ratio is not equal to 3 ∕ 4 , the cutting speed must be adjusted for the conditions. The adjusted cutting speed V is calculated from V = V opt 3 F f 3 F d 3 F ar , where V opt is the lower of the two speeds given in the speed table, and F f , F d , and F ar are adjustment factors for feed, axial depth of cut, and radial depth of cut, respectively, obtained from Table 15d(face milling); except, when cutting near the end or edge of the workpiece as in Fig. 4, Table 15c (side milling) is used to obtain F f . 7 ipm (approximately) = π = = =
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online