Manufacturers of components in the machining process have delivered stronger cutting tools, better machine tools, more effective coolant, better toolholders, and superior workholding systems, and machining productivity has increased as a result. Toolpath technology, however, has not kept pace. CAM software developers have focused on streamlining the NC programming process with considerable advances. However, the tool paths themselves can have a tremendously positive impact on the machining process—the actual cutting of the metal—if designed and generated properly. Because CAM software generates the tool paths that drive the machines, it can be argued that, of all the components and technology involved in the milling process, CAM software may have the biggest impact.

The industry needs a toolpath engine that leverages the capabilities of numerically controlled milling machines to drive cutting tools along a path that is not restricted by manual milling techniques. Doing so would provide precise control of the cutting forces, enabling the use of much more aggressive machining parameters. Thus would in turn result in reduced machining time.

Such a toolpath engine now exists. Because the increased performance of these new tool paths is the result of reduced stress on the machining components, cutting tools are lasting several times longer than before. Evidence suggests that the reduced machining stress will extend the useful life of the other hardware components, including the machine tools themselves.

The Fundamental Challenge

The fundamental challenge in milling is controlling the radial engagement of the cutting tool with the material. If the radial engagement isn’t controlled, then the cutting forces cannot be controlled. If the cutting forces aren’t controlled, compromises must be made in the machining parameters, extending machining time and thereby reducing productivity.

Figure 1. A 70 percent stepover produces a total engagement angle (TEA) of 113.58 degrees.

Traditional toolpath strategies are based on design conventions that are holdovers from the days of crank handles, but are unnecessary with numerically controlled machines. They are based on a constant stepover between cuts and/or are driven by the shape of the area being machined. Following these conventions makes it impossible to control the tool’s radial engagement with the material, or tool engagement angle (TEA).

There is a relationship between a stepover value and a tool’s engagement angle with the material. A stepover value of 50 percent of the cutter diameter equates to 90 degrees of the periphery of the tool being engaged with the material.  A 30 percent stepover equates to a TEA of 66.42 degrees. A 70 percent stepover is a 113.58-degree TEA (Figure 1). For any given stepover value, there is one and only one corresponding TEA. However, this is true only when cutting along 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 percent stepover (113.58-degree TEA) encounters a 135 degree-concave corner, the TEA increases by 45 degrees (180 degrees – 135 degrees = 45 degrees) to 158.58 degrees (Figure 2).

Figure 2. Tool engagement increases substantially when the tool encounters a concave corner.

Consequently, a tool reaches full engagement (180 degrees of TEA) when the angle of the sharp, concave corner equals the straight-line TEA. Thus, a tool programmed at a 70 percent stepover reaches full engagement whenever it encounters a sharp, concave corner of 113.58 degrees or less (Figure 3). These increases in TEA cause significant increases in machining load. A tool machining a rectangular pocket with a 50 percent stepover value reaches full engagement every time it makes a turn. As it enters the corner, the tool is rapidly overloaded, increasing the “push” away from its natural attitude (parallel to the spindle. It then quickly comes to a stop, is rapidly unloaded and attempts to “spring” back toward its natural attitude. It then rapidly reloaded, this time to its expected level, as it exits the corner. This dynamic produces the groaning and screeching commonly heard while milling. This adverse machining condition is not only tolerated, but also generally accepted as normal. NC programmers compensate for this by compromising the machining parameters (for example, some combination of slower spindle speeds, slower feed rates, smaller stepovers, or shallower depths-of-cut) which increases machining time.

Figure 3. A tool machining a rectangular pocket reaches full engagement every time it makes a turn.

These sharp corners result when the tool path is driven by the shape of the part to be machined. Using the example of a simple pocket, traditional tool paths fill the area either with parallel, straight-line cuts (equally spaced by the stepover value), which are traversed in either a “lace” or “non-lace” mode, or, more typically, with equally spaced, nested offsets of the pocket geometry. The straight-line method requires sharp-corner turns to get from one cut to the next. With rare exceptions, perhaps with circular or oval shapes, the offset method does, tool (and even with such shapes, getting from one cut to the next presents a challenge.) In almost all other cases, any corner radii in the geometry will “collapse out” in just a few offsets – commonly on the first offset – leaving these sharp corners in the tool path. In each such corner the TEA, and therefore the machining load, increases. The more acute the angle of the corner, the higher this increase will be. These corners represent the worst-case machining conditions for any tool path. Cutting parameters must be set low enough for the tool to survive these conditions, causing the tool to be used inefficiently when not overloaded, thus yielding material removal rates that are far below the machining hardware’s capabilities.

With offset tool paths, each nested cut produces a shape that is a smaller version of the finished shape, clear evidence that the boundary geometry dictates the path of the tool. Using this principle, no method of effectively controlling the TEA is possible.

Treating The Symptoms

            A variety of specialized tool paths have been developed by the CAM industry. In some cases, these specialized tool paths have performed better than offset tool paths. However, none adequately address the inability to effectively control the TEA in the general case, as can be seen by examining a few of these specialized tool paths.      

Figure 4. Trochoidal milling uses a looping motion to prevent the TEA from reaching 180 degrees.

Trochoidal milling.  This milling technique employs a sort of “constant looping” motion in an attempt to avoid fully loading the cutting tool and thereby allowing higher feed rates. Essentially, this toolpath strategy modifies the offset machining method by adjusting the spacing of the offsets to account for the wider “tool kerf” that results from the constant looping. Although this method (Figure 4) can prevent the TEA from reaching 180 degrees, it does so at a steep price. By definition, this machining method causes the tool to be completely disengaged from the material for a significant portion of the overall toolpath length, most often for the majority of the toolpath length. Machining at a TEA of zero degrees is commonly referred to in the shop as “cutting air,” and it is obviously unproductive. This constant looping occurs even in portions of the tool path where tool overload is not an issue.

Similar to the sharp corner scenario discussed above, for a given radial depth-of-cut (or stepover), the TEA also increases whenever a tool transitions from cutting in a straight line to cutting a concave arc, as a function of the cutter radius and the toolpath radius. This occurs even if that transition is smooth and tangential. The smaller that concave radius is, the greater the TEA becomes. In trochoidal milling, the tool traverses a connected set of constant radius arcs spaced by a fixed distance. For reasons of practicality, the loop radius employed should be no larger than the radius of the cutting tool in use. If the loop-radius is equal to the tool radius, and the spacing between loops is equal to the toolpath stepover. For a stepover value of 50 percent, for example, the TEA increases from 90 degrees to 120 degrees, an increase of one-third. Using a smaller loop radius causes an even greater increase in TEA. The only way to prevent the TEA from increasing beyond 90 degrees is to reduce the spacing between loops, which of course further increases the toolpath length.

Figure 5. Partially trochoidal tool paths offer shorter tool paths and less air cutting than standard trochoidal milling.

The results of all this looping are tool paths that are many times longer than standard ones. Thus, the feed rate for these paths must be many times faster to maintain the same productivity level. Unfortunately, significantly increasing the programmed feed rate is problematic. When a tool traverses a concave corner radius, as it continually does in trochoidal milling, the periphery of the tool, where the chips are shorn from the material (assuming a climb milling direction), is feeding faster than the center of the tool. The difference in speed is a function of the radius of the tool and the toolpath radius. For a toolpath radius that is equal to that of the cutting tool, the effective feed rate at the periphery of the tool is double that of the programmed feed rate. If the toolpath radius is half that of the cutting tool radius, then the effective feed is triple the programmed feedrate. The larger the difference between these radii, the greater is the feed rate disparity. So, in the example just described, the effective feed rate in the loops is already twice the programmed rate.

Increasing the programmed rate significantly enough to compensate for the excess toolpath length causes the peripheral feed rate to rise even higher, introducing chip-clearance problems that can result in tool failure. It is difficult to imagine a case where the feed rate can be increased sufficiently to overcome the extended toolpath length.

Figure 6. In a morphing tool path, cuts are “pulled apart” in wider areas of the workpiece and “squeezed together” in narrower parts.

Partially trochoidal tool paths. This method seeks to improve on the standard trochoidal motion by identifying the problem areas of a tool path and applying the constant looping in those areas only (Figure 5). This produces a somewhat shorter tool path and less “air cutting” than standard trochoidal milling, and it is therefore an improvement over that method. However, it is limited by the other characteristics inherent to the algorithm: the TEA and peripheral feed rates still increase in the loops, limiting any feed rate increases that might be used to offset the extended toolpath length. In addition, many other areas of the tool path where the TEA naturally increases, such as in larger concave radii that are not tight corners, remain predominantly untreated. The detection of areas where the looping should be applied can also be prone to error. If feed rates are increased enough to reduce cycle times with this method and a problem area goes undetected, then severe tool overload and possible tool breakage can occur. The method relies on detection and adjustment, rather than avoidance by design.

Morphing Tool Paths. This milling method alters the path of the tool as it moves from one boundary to another. In Figure 6, the morphing occurs between the island and the outer boundary of the pocket. While the cuts are clearly not equally spaced, they are clearly driven by the shape of the area being machined, much more so than a standard, offset tool path. With a standard, offset tool path, not every cut is required to traverse the entire boundary--the innermost cuts are often “collapsed out” from certain areas. The typical morphing algorithm, however, requires all cuts to trace, or at least be influenced by, all of the boundary elements. To facilitate this, the cuts are essentially “pulled apart” in wider areas of the part and “squeezed together” in narrower areas.

On the surface, there appear to be two possible benefits to this approach. First, the number of truly sharp corners is significantly reduced. Second, it has the potential to enable the use of a stepover of greater than 50 percent of the cutter diameter without leaving uncut stands of material. However, the method introduces other problems that aren’t present with standard offset tool paths, likely negating potential benefits.

Figure 7. The TEA varies during every cut in a morphing tool path.

Note that this approach inevitably varies the TEA, rather than attempting to manage it, thus exacerbating the fundamental milling problem. As can be seen from a quick visual examination of the tool path, the amount of tool engagement varies widely and continually throughout. Instead of the TEA increasing only in the sharp corners, morphing causes the TEA to vary during virtually every cut. Figure 7 shows that a tool programmed at a 70 percent stepover (113.58 degrees TEA) in this open-sided region reaches a TEA of 145.03 degrees immediately upon entering the material. The TEA associated with the user-specified stepover isn’t considered. Figure 8 shows that, by the end of this straight-line cut, the TEA has reached 175.12 degrees, almost completely burying the cutter.

This variance in the TEA during a morphing tool path occurs even in those cuts that traverse straight lines. (One positive attribute of a standard offset tool path is that it maintains a constant TEA when cutting in a straight line; a morphing algorithm misses that benefit.) The machining parameters must, of course, be limited to values that can survive the areas of highest engagement, meaning that the tool is being used inefficiently in all but those areas. This is especially true in the many areas of the tool path where the cuts are compressed together.

Figure 8. A morphing tool path does not maintain a constant TEA, even in straight-line cuts.

The small radius in the toolpath corner prevents the tool from reaching 180 degrees TEA, but only by a negligible amount, as illustrated in Figure 8. Likewise, the introduction of this radius causes the peripheral feed rate to rise significantly in the corner, requiring further reductions in the machining parameters.

Moreover, this method does not completely avoid the instances in which the tool is fully buried, especially when islands are present. Referring again to the tool path in Figure 6, the tool would be engaged at 180 degrees during the cut around the island. If the island were not conveniently located at the center of the pocket, then the cuts on the smaller side of the island would be compressed. This is much like the cuts above and below the island and it further reduces machining efficiency. The presence of multiple islands or convex corners magnifies the inefficiency.

Corner Looping. This strategy is designed to address the problem of uncut material in corners when larger stepovers are used. It does so by adding self-intersecting loops where sharp directional changes occur in a standard offset tool path. The loops are added where necessary, and the size of each loop is established so that when the tool approaches the same area on the next offset, no material will be left behind. An example of this type of tool path is shown in Figure 9.

Figure 9. Corner looping is designed to prevent leaving behind uncut material.

Unfortunately, rather than minimizing the length of time that the tool is over-engaged, it extends that time; the tool must bury itself deeper into each corner to facilitate the looping motion. Feeds and speeds must be set low enough for such occurrences. However, the most detrimental characteristic of this strategy is that the cutting direction is reversed (from climb to conventional in this case) each time the apex of one of these loops is reached and the exit from the loop begins. Thus, in treating one toolpath problem, this strategy introduces two new problems, either of which is arguably more serious than the one being addressed. Combine the increased peripheral feed rates inherent in the small-radius loops to the reversal in cutting direction, and one of the most unfavorable machining conditions is established. This is hard on the cutting tool, the machine tool and every other component of the machining environment.

Feed Rate Optimization. Because the TEA, and therefore the machining load, cannot be controlled with the toolpath strategies discussed so far, feed rate optimizers have been applied to compensate. The load on the tool varies greatly and frequently within a tool path—whether generated by traditional means or with one of the above methods—making it virtually impossible to select a single, ideal feed rate for the entire toolpath. To avoid tool breakage, feed rates are typically programmed for the worst-case condition within a given tool path. This causes the tool to feed slower than necessary when it is not overloaded, resulting in slower material-removal rates. Feed rate optimizers attempt to analyze these changing load conditions and make the appropriate adjustments. Such optimizers post-process the tool path and adjust feed rates downward where more material is detected and upward where less material is detected.

For these optimizers to be effective, a considerable amount of setup and maintenance effort may be required by the end user. Feed rate ranges need to be established for various amounts of material that are encountered. These ranges can vary depending on the type of cutting tool used, its diameter, length, material, number of flutes and the workpiece material. Other factors, including the machine tool in use, the relative rigidity of the workholding setup and simple user-preference, all have an impact. This is a lot of data to consider and manage. The feed rate changes may tend to be abrupt jumps from one value to another rather than smooth transitions. Because the spindle speed is not correspondingly adjusted, the effective chip load, in feed per tooth, does not remain constant, which is a less than ideal characteristic. The cost of these optimizers must also be considered.

These optimizers typically rely on an in-process stock model from a material-removal simulation process to determine where excess material may or may not exist. Though such simulators are fairly accurate within a tolerance (or pixel) range, the possibility for error does exist. If the feed rates are pushed aggressively enough, then even a single miscalculation can cause problems at the machine.

Beyond Detect-And-Adjust

The above-mentioned approaches are a few of the many that are available. Because these approaches tend to be detect-and-adjust solutions, they cannot work in the general case. Toolpath algorithms designed specifically for high speed milling (HSM) also fall into this category. They are based on a constant stepover, are driven by the boundary geometry and are detect-and-adjust approaches. Therefore, they suffer from limitations similar to those discussed above. The result is a multitude of toolpath strategies that NC programmers must consider in hopes of selecting the proper strategy for a given situation. Most CAM software developers offer multiple ways to machine a pocket, for example; some systems feature more than ten. The truth is that if any one of those multiple methods actually worked in the general case, the others would be unnecessary.

Engagement-Controlled Milling

One solution to the fundamental milling problem is to generate toolpath motion that does not over-engage the cutting tool. This concept enables the use of more aggressive machining parameters in a safe and predictable manner.
The toolpath engine called TrueMill, available in SurfCAM Velocity from Surfware, Inc. (Westlake Village, California) takes such an approach. There are no constant stepovers in tool paths generated by this software. The tool path is not driven by the boundary geometry; the geometry contains the tool path, but it does not dictate its flow. By removing these restrictions, the tool’s engagement angle with the material can be controlled. Controlling the TEA enables the machining load to be managed, which, in turn, enables the use of more aggressive machining parameters than might otherwise be possible. As a result, machining times are reduced and there is significantly less stress on the hardware components in the machining environment, even at the more aggressive machining parameters. This helps extend cutting tool life.

Fig. 10—Using a constant TEA creates distinctive tool paths that contain no sharp corners.

Figure 10 shows that a TrueMill tool path is different from a tool path generated by other means. As discussed above, the highest increase in TEA occurs in a sharp corner. Therefore, this tool path contains no sharp corners. The next highest engagement values occur when cutting concave arcs. Because it is not feasible to construct tool paths that are free from concave arcs, there is no attempt to do so. Rather, these tool paths are constructed almost entirely of concave arcs, but the TEA is controlled in those arcs. If there are no sharp corners present, and the TEA is controlled in the concave arcs, then it is inherently controlled everywhere else.

Because the tool paths are not driven by the boundary geometry, each cut of the path is able to perform two functions rather than one. In a traditional tool path, each cut merely removes material as it traverses an offset of the boundary geometry. With a controlled TEA, each cut of the tool path removes material as well, but it does so in a manner that prepares the constantly evolving in-process material boundary so that the TEA will be automatically controlled during the next pass of the tool. This is not possible when traversing offsets of the boundary geometry. Using this new method, the shape of the area being machined is not apparent until the final passes of the tool. Although the tool paths may look haphazard at first glance, they are precisely planned and controlled.

The result is that machine tools and cutting tools can be used to the limits of their capabilities. The tool paths themselves do not limit the material-removal rates by forcing the machining hardware to perform under adverse machining conditions. In some cases, the machine will reach its maximum feeding capabilities and/or horsepower peak before the cutting tool is in danger. On stronger, faster machines, the cutting tool will reach its limits before the machine begins to become overtaxed.

The increases in machining parameters and resulting reductions in cycle time are considerable. For example, one customer substituted these TEA-controlled tool paths for the roughing tool paths previously used. The roughing time for the part dropped from 17 minutes and 11 seconds to 2 minutes and 54 seconds, a reduction of 83 percent. The same amount of material was removed approximately six times faster than with the traditional tool paths.

The only characteristic that these tool paths share with the detect-and-adjust tool paths previously described is that they are longer than traditional offset tool paths. However, machining parameters can be increased to more than compensate for that extra length. In this case, the user was able to nearly quadruple the programmed feed rate over the previous tool paths, triple the axial depth-of-cut and increase the programmed stepover from 44 percent of the tool diameter to 75 percent. If the machine tool in use had a faster spindle and/or a higher maximum cutting feed rate, then the time reductions would have been greater. Another user reported a roughing time reduction from 27 minutes to 5 minutes on one part. Another realized a reduction from 1 hour to less than 8 minutes.

The machining parameters required to achieve this level of performance are beyond the usual recommendations. Current cutting tool manufacturer-recommended values are too low for these tool paths. For example, one shop machined a part from 4140 steel, with a solid carbide, four-flute, 0.5 inch diameter end mill, at 12,000 rpm and a programmed feed rate of 1,000 ipm. The surface speed (nearly 1,600 feet per minute) and chip load (slightly under 0.021 inches per tooth) are several times the recommended values. These speeds were not achieved by using light cuts. The axial depth-of-cut was 0.5 inch (equal to the tool diameter), and the programmed stepover was 0.140 inch (64 degrees TEA). This is faster than most shops have ever cut aluminum.

With these machining parameters, especially with the high surface speed number, one might expect the cutting tool to wear more quickly. In fact, after machining several parts at these parameters, the tool showed no visible signs of wear.

These observed results are not small, incremental productivity improvements resulting from tweaks to traditional milling methods. Such time savings have the potential to redefine the milling industry.

About the author. Glenn Coleman is vice president of product design at Surfware, Inc.