A NEW TOOL PATH STRATEGY TAPS THE TRUE POTENTIAL OF CNC MILLING MACHINES

Transcription

1 volume 9 issue 33

2 A NEW TOOL PATH STRATEGY TAPS THE TRUE POTENTIAL OF CNC MILLING MACHINES There s no denying that CNC milling machines represent a quantum leap in productivity over their manual brethren. Even so, numerically controlled milling machines still fall short of their true productivity potential. A bold statement, yes, but the limiting factor in material removal rates is not the machine tool itself, or the cutting tools. Rather, the limiting factor in the productivity of CNC milling machines is the input to the machines the tool paths that drive them. Tool paths force machine tools and cutting tools to perform under the worst possible conditions. Cutting tools are driven into corners where the machining load increases dramatically. Sharp directional changes require machine tools to come to complete stops, and to accelerate and decelerate rapidly and often. Feedrates are maintained at the center of the cutting tool, which does not control how fast the chips are removed, except when cutting in a straight line. Machine tool builders and cutting tool manufacturers have made many technological advances to better cope with these worst-case conditions, but until tool path logic is reinvented, these adverse conditions remain and machining productivity is limited. By Glenn Coleman, Vice President of Product Design, Surfware, Inc. 20

3 CNC MACHINING 21

4 Existing tool path generators maintain a constant stepover between cuts, and a constant feedrate at the center of the tool. These two core strategies, though unavoidable with manual milling, actually limit the utility of numerically controlled machines. NC machines have always been capable of running free of these restrictions, but the tool path engines developed by CAM software vendors and even the early computer-assisted programming languages, such as APT keep these strategies not only in play, but front and center. A brief look at these machining dynamics illustrates how a tremendous opportunity to increase productivity has been overlooked for many years. Constant Stepover There is a relationship between a stepover value and a tool s engagement angle with the material. A stepover value of 50% of the cutter diameter results in 90 of the periphery of the tool being engaged with the material. A 30% stepover equates to a tool engagement angle (TEA) of 66.42, and a 70% stepover yields a TEA of (Figure 1). For any given stepover value there is one, and only one, corresponding TEA. But this is true only when cutting in a straight line with a constant radial depth of cut. When traversing a sharp, concave corner, the TEA increases by the supplement of the angle of that corner. For example, when a tool programmed at a 70% stepover ( TEA) encounters a 135 concave angle, the TEA increases by 45 ( = 45 ) to (Figure 2). Consequently, a tool reaches full burial (180 of TEA) when the angle of the sharp, concave corner equals the original TEA. So a tool programmed at a 70% stepover reaches full engagement whenever it encounters a sharp, concave corner of or less (Figure 3). These significant increases in tool load are extremely common. A tool machining a rectangular pocket with a 50% stepover value reaches full engagement every time it makes a turn. Each such turn requires the machine to come to a complete stop, however briefly, in order to change directions, as evidenced by the circular dwell marks commonly left on the floor of a part. As the tool enters the corner, it is rapidly and significantly overloaded, increasing the push away from its natural attitude (parallel to the spindle). It then quickly comes to a stop, where it is rapidly unloaded and attempts to spring back toward its natural attitude. As the tool exits the turn, it is then rapidly reloaded, this time to its expected level. 22

5 Fig. 1 This cycle is what produces the groaning and screeching heard all day, every day, in every machine shop throughout the world. This obviously adverse machining condition is not only tolerated, but is accepted as normal. NC programmers compensate for this with some combination of slower spindle speeds, slower feedrates, smaller stepovers or shallower depths of cut, which, in all cases, cause increased machining time. Fig. 1 For 70% stepover, tool engagement angle (TEA) = when cutting in a straight line. Fig. 2 When the tool encounters a corner, the TEA is increased by 180 minus the angle of the corner. In this example, the corner angle = 135. Therefore, the TEA = ( ) = Fig. 3 Therefore, the tool is at maximum engagement (180 ) when the corner angle is straight line tool engagement angle. For 70% stepover, TEA = in a straight line. Fig. 2 Fig. 3 Constant Feedrate The other staple of existing tool path generators is to maintain a constant feedrate at the centerline of the cutter. But maintaining a constant feed at the tool s center causes a nonconstant feedrate at the periphery of the tool, where the chips are actually produced. A simple analogy can be found on a running track. An Olympic track has an inside running length of 400 meters. Most tracks have 85-meter straights, and turns that have a radius of meters. On the straights, a runner in lane 2 keeps pace with a runner in lane 1 (the inside lane) by running at the same speed. In the turns, however, the runner in lane 2 must run significantly faster to keep pace; he must cover a longer distance in the same amount of time. Now, move the runner in lane 2 to lane 8, and he must run dramatically faster to keep up, perhaps impossibly so. If the inside radius of the turn is reduced from meters to, say, 1 meter, the outside runner must now run even faster. The distance between lanes represents the radius of the endmill. The greater this value is, the greater the disparity in speed. (Imagine a track with many more lanes.) The inside radius of the track represents the tool path radius at the centerline of the tool. The smaller this value is, the greater the disparity in speed. The numbers are dramatic. For example, when a 1.00" diameter endmill, programmed at 100 ipm, traverses a concave tool path radius of 0.010", the effective feedrate at the periphery of the tool is 5,100 ipm. Reduce that tool path radius to 0.005", and the effective feedrate is 10,100 ipm. CNC MACHINING 23

6 In our track analogy, a runner in an outside lane simply falls behind under these circumstances. Clearly, the periphery of a cutting tool has no such option: The effective feed per tooth becomes tremendously out of sync with the spindle speed. As a result, the chips cannot clear, and the tool breaks. Recent tool path innovations that add small radius arcs to keep the machine from coming to a stop (most HSM algorithms), or small-radius circular moves to keep from fully burying the tool ( trochoidal milling), actually cause dramatic increases in stress and wear on the machine tool and the cutting tool. To compensate for this phenomenon, whether it is realized or not, NC programmers reduce the programmed feedrate, which, of course, slows the entire tool path. If feedrates aren t slowed enough, machine operators must diligently man the feed override control to slow the tool in the corners, which is an additional drain on productivity. Such tool path deficiencies force machine tool builders, cutting tool manufacturers and NC programmers to compensate for the CAM software industry s lack of vision. Efforts to develop software to automate the NC programming process, with the apparent goal of eliminating NC programmers (a bad idea), divert attention from where it should be. CAM software should leverage the tremendous capabilities of numerically controlled milling machines and modern cutting tools to reduce machine cycle time. This has finally happened. A True Revolution A completely new, patent-pending, tool path engine has been developed that maintains the tool s engagement angle with the material at or below a user-controlled threshold. This software completely disregards the stepover value, other than using it to calculate a TEA. Since the TEA is controlled, rather than the stepover, the tool paths look completely unlike the tool paths generated with traditional methods, with the shape of the machined feature not evident until the final cuts. The constant machining load on the tool enables the use of significantly more aggressive machining parameters. In addition, the system automatically manipulates the programmed feedrate to maintain an effective feedrate throughout the entire tool path. Every unique, concave radius in the tool path has a unique, appropriately adjusted feedrate. In the above example of the 1.00" diameter endmill traversing the 0.005" radius, the tool path engine adjusts the feedrate at the center of the tool to 0.99 ipm, which maintains the speed at the periphery of the tool at a constant and uninterrupted 24

7 Surfware, Inc ipm. Dramatically increased programmed feedrates can now be used. Tests reveal that the feeds and speeds recommended by cutting tool manufacturers are now obsolete. At the recent EASTEC show in Springfield, MA, this new tool path engine was used to drive a Haas VF-2SS a high-speed VMC with a 12,000-rpm spindle and 1,400-ipm rapids. Using a 0.500" diameter, 3-flute, solid carbide endmill, a freeform shape was milled from 6061 aluminum. The tool ran at 12,000 rpm, with a 0.500" depth of cut, 0.375" programmed stepover and a programmed feedrate of 756 ipm! This is triple the recommended feed per tooth for the tool, and the machining was so smooth as to be almost inaudible. Due to the much lower machining loads, the stress on the tool was drastically reduced. After three days of machining, the cutter still looked new. Since this new tool path engine precisely controls the TEA, the tool never encounters excess material. Therefore, the shape of the part is irrelevant. For a given tool in a given workpiece material, any combination of spindle speed, feedrate, depth of cut and stepover that yields the desired combination of material removal rates and cutting tool life when cutting in a straight line on the edge of a block can safely be used on any part, regardless of its shape. With this software, it is now possible to fully utilize the full capability of numerically controlled machines. Tool paths no longer limit material removal rates. Rather than force machine tools and cutting tools to operate under worst-case conditions, this new tool path engine turns all conditions into best-case conditions. This new patent-pending technology, called TrueMill, is only available in SURFCAM Velocity by Surfware, Inc. CNC MACHINING 25

8 RELENTLESS.