Many wear parts are made from mechanical plastics. Common ones include bearings, gears, material-handling parts and machine components such as spacers and positioning mounts where the reduction of vibration is essential. Traditionally, these types of parts have been fabricated from metal. But mechanical plastics are beginning to replace metal because of their increased durability, excellent machinability, and exceptional mechanical and electrical properties. Common mechanical plastics include acrylonitrile butadiene styrene (ABS), Acetal, Delrin, Hydex, nylon, polycarbonate, polyurethane and polyethylene terephtalate (PET).     Cutting Tool Geometry Router bits for cutting mechanical plastics have traditionally been run on CNC routers at high spindle speeds and feed rates. Extensive testing and years of field experience have shown that a tool with a high rake and low clearance performs exceptionally well. It machines mechanical plastics more productively than tools with other geometries and imparts a finer surface finish (Figure 1). This kind of free-cutting geometry is rarely used by shops to machine mechanical plastics. Most use endmills running on CNC milling machines.    Tool Selection Mechanical plastics are characterized as either soft or hard. By looking at the chip produced, a machinist can easily determine the flexibility or rigidity of the material being cut. Soft plastic produces a curled chip, while hard plastic produces a splintered wedge. Generally, O-flute tools are applied to soft plastic, while V-flute tools are used with hard plastic (Figure 2). Most wear plastics are made from soft plastic. Consequently, O-flute tools are recommended for machining most mechanical plastics.     O-flute tools are manufactured in straight- or spiral-flute configurations. The choice depends on which direction the user wants the chips to flow. Straight tools have a neutral effect, while spiral tools can influence the chips either upward or downward. (For purposes of clarification, a downcut spiral is a lefthand spiral, while an upcut spiral is a right-hand spiral.) For the most part, routers with upcut, or right-hand, spirals are applied because they effectively evacuate chips. Downcut, or lefthand, spirals tend to recut chips, which is not advantageous when cutting mechanical plastics where chip welding may be a problem. However, for part hold-down considerations and through-cuts, left-hand spirals are a standard item.     The O-flute spirals are available as single- and double-edge tools in diameters ranging from 1.16" to 3.4". When machining mechanical plastics, the single- edge O-flute spirals impart a finer finish than multiple-flute endmills. When small tool diameters are necessary, the single-edge design, with its more open flute, accentuates chip evacuation. In terms of balance, a maximum cutting-edge diameter of 3.8" is recommended for single-edge tools. If cutting tool balance is an issue or a deeper cut is required, double edge O-flute spirals and 3-flute finishing tools are logical selections. Both of these types of tools can machine materials up to 31.8" thick. Excellent finishes can be achieved when deep cuts of two to four times the cutting- edge diameter are made at aggressive feed rates. The double-edge O- flutes are available with a low- or high helix angle to accommodate a range of horsepower requirements. Also, high helix cutting tools are advantageous in materials over 1" thick.   Chip Load Once the correct tool geometry is chosen, the proper chip load is the next consideration. In mechanical-plastics machining, the recommended chip load range is 0.004 to 0.012 ipt, which results in an excellent finish and acceptable productivity rates (Figure 3). This narrow range imparts the finest finish through the continuous generation of properly sized or curled chips. Inadequate chip load can lead to knife marks, which adversely affect the finish. O-flute tools with a high rake and low clearance help eliminate knife marks by slightly rubbing the part during machining.   Machining Ways Today’s CNC milling machines are more than adequate to achieve the proper feeds and speeds for router tools. Spindle speeds of 10,000 rpm and higher, with feed rates in excess of 600 ipm, are not uncommon. However, when these kinds of capabilities are not available or feasible, router tools toleranced for machining mechanical plastics can perform at spindle speeds of 6,000 rpm and proportionately higher feed rates. The key is maintaining proper chip load to enhance productivity and part finish.