Machinery's Handbook, 31st Edition
MACHINING MONEL AND NICKEL ALLOYS 1259 300 BHN, a grade of straight tungsten carbide will often work best, although some crater resistant grades will also work well. A sulfurized oil or a water-soluble oil is recommended for rough and finish turning. A sulfurized oil is also recommended for milling, threading, tapping, reaming, and broach ing. Recommended cutting speeds for Monel and the softer nickel alloys are 70 to 100 fpm (20–30 m/min) for high-speed steel tools and 200 to 300 fpm (60–90 m/min) for cemented carbide tools. For the harder nickel alloys, the recommended speed for high-speed steel is 40 to 70 fpm (12–21 m/min) for a hardness up to 300 BHN and for a higher hardness, 10 to 20 fpm (3–6 m/min); for cemented carbides, 175 to 225 fpm (55–70 m/min) when the hard ness is less than 300 BHN and for a higher hardness, 30 to 70 fpm (9–21 m/min). Nickel alloys have a high tendency to work harden. To minimize work hardening caused by machining, the cutting tools should be provided with adequate relief angles and positive rake angles. Furthermore, the cutting edges should be kept sharp and replaced when dull to prevent burnishing of the work surface. The depth of cut and feed should be sufficiently large to ensure that the tool penetrates the work without rubbing. Machining Copper Alloys.— Copper alloys can be machined by tooling and methods similar to those used for steel, but at higher surface speeds. Machinability of copper alloys is discussed in Table 2 on page 512 and Table 3 on page 516. Machinability is based on a rating of 100 percent for the free-cutting alloy C35000, which machines with small, easily broken chips. As with steels, copper alloys containing lead have the best machin- ing properties, with alloys containing tin and lead having machinability ratings of 80 and 70 percent. Tellurium and sulphur are added to copper alloys to increase machinability with minimum effect on conductivity. Lead additions are made to facilitate machining, as their effect is to produce easily broken chips. Copper alloys containing silicon, aluminum, manganese and nickel become progres sively more difficult to machine, and produce long, stringy chips, the latter alloys having only 20 percent of the machinability of the free-cutting alloys. Although copper is fre quently machined dry, a cooling compound is recommended. Other lubricants that have been used include tallow for drilling, gasoline for turning, and beeswax for threading. Machining Non-Metals Machining Hard Rubber.— Tools suitable for steel may be used for hard rubber, with no top or side rake angles and 10 to 20 degree clearance angles, of high-speed steel or tungsten carbide. Without coolant, surface speeds of about 200 ft/min (60m/min) are recommended for turning, boring and facing; with coolant, increase up to 300 surface ft/ min (90 m/min). Drilling of hard rubber requires high-speed steel drills of 35 to 40 degree helix angle to obtain maximum cutting speeds and drill life. Feed rates for drilling range up to 0.015 in/rev (0.38 mm/rev). Deep-fluted taps are best for threading hard rubber, and should be 0.002 to 0.005 inch (0.05-0.13 mm) oversize if close tolerances are to be held. Machine oil is used for a lubricant. Hard rubber may be sawn with band saws having 5 to 10 teeth per inch (2–4 teeth/cm), running at about 3000 ft/min (914 m/min) or cut with abrasive wheels. Use of coolant in grinding rubber gives a smoother finish. Piercing and blanking of sheet rubber is best performed with the rubber or dies heated. Straightening of the often-distorted blanks may be carried out by dropping them into a pan of hot water. Formica Machining.— Blanks can be cut from sheets of “Formica” either by a band saw or by trepanning tools in a boring mill or a drill press. To saw blanks, first describe a circle as a guide line, then use a 21-gage 3 1 ∕ 2 -point saw running at a speed of 5000 ft/min (1525 m/min). The saw should be sharp, with a 1 ∕ 64 -inch (0.4 mm) set on both sides. In drilling, use an ordinary high-speed drill whose point is ground to an included angle of 55 to 60 degrees. Another method is to grind the drill point slightly off center. The feed
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online