The evolution of toolpath development has taken two routes, according to Ben Mund, senior market analyst for CNC Software Inc., Tolland, Conn. One developed from a traditional machining approach that applied a 50 percent stepover as a rule of thumb to today’s dynamic machining. In dynamic machining, he explained, CAM developers started with radial chip thinning principles and created software that constantly adjusted the toolpath, axial depth of cut, and/or removal rate to maintain constant engagement and consistent chips. When it’s done right, shops get excellent tool life and high material removal rates. And it will work with virtually any tool on any machine.
Conversely, the other route marries CAM software to a specific cutting tool to achieve accelerated machining. “Both are equally powerful,” said Mund, “but have very different evolutions.” Which do you choose? Do you need to choose? And is there more you can do to improve performance between generating a toolpath and pressing “go” on the machine?
Dynamic machining is so close to a universally applicable solution that all the major CAM providers have their own version of it. In CNC Software’s Mastercam product it’s called Dynamic Motion. Open Mind Technologies USA, Needham, Mass., calls its high-performance package hyperMILL MAXX Machining. Vyncent Paradise, director of product development for NX CAM at Siemens Digital Industries Software, Plano, Texas, said its package is designated Adaptive Milling. He also explained that there are add-on modules from partners that offer optimized roughing.
Whatever it’s called, dynamic machining produces a radically different cutting path compared to traditional machining. The traditional toolpath follows the desired profile at a predetermined offset and works its way down into the material in an orderly fashion. CNC Software’s Mund explained that dynamic machining is most effective when allowed to use as much of the tool’s cutting length (maximum axial depth of cut) as possible in one continuous path. And in calculating the most efficient route to cutting material out of the space, Siemen’s Paradise added that the software typically produces “lots of crescent shaped paths that go from one end to the other and then back again, with varying radii.” The result can look chaotic compared to a simple offset approach.
Dynamic machining software also uses a shallower radial depth of cut while varying the stepover or the feed rate (depending on the vendor) to “control the engagement level in the material cutting so you can ensure consistent cutting forces are applied to the tool during machining,” said Paradise. This maximizes tool life, because, according to Mund, “this type of cut makes heat management dramatically more efficient, and heat is a prime cause of tool wear.” It also maximizes tool life by eliminating peak loads, which can break the tool before wear becomes the problem. And although the radial depth of cut is smaller than a traditional path, the material removal rate is higher because the dynamic path is in constant contact with the material, using a deeper axial cut and a theoretically optimal engagement.
So, are there significant differences among the CAM providers? It’s hard to say and the players acknowledge it’s a very competitive field. One area of distinction is taking the technique into five-axis machining. Paradise said it’s a big push for Siemens. Open Mind has built its reputation on five-axis machining software, according to Managing Director Alan Levine. One interesting example he cited is creatively using five-axis capability to perform operations like drilling that are traditionally thought of as strictly one-axis, up-and- down moves. Levine explained that sometimes Open Mind considers helical drilling (in which an end mill cuts a hole larger than its diameter by moving in both the vertical and horizontal axes), “but rather than pushing down vertically and mashing the chips on themselves, we use a five-axis mode such that the cutter is tilted forward and there’s room for the chips to flush out on the backside.”
Levine also pointed to Open Mind’s Smooth Overlap function for when multiple operations occur adjacent to each other, or different cutting tools or different cutting angles are used in adjacent areas. “The physics of such situations are complex,” he said. “Any error in tool measurement, or degradation of the cutter that changes how it cuts, or temperature changes over the course of a day, can lead to mismatches and visual problems on a part. Smooth Overlap tries to solve that with a small lift at the transition point, rather than just a simple overlap with a double cut in the area. The software presents the customer with the option to use the feature with a single button, sometimes two buttons. There’s no need to redraw toolpaths and no upfront CAD work, yet we’re still covering the material and the blends are fantastic.”
A related topic is Open Mind’s High Precision mode. Levine explained that almost the entire CAM industry machines to “some sort of mesh on top of surfaces, because the CAD models can come from many different types of software, with many different topologies and lots of patchy surfaces. Using a mesh simplifies the CAM challenge.” He added that although the mesh can be very accurate, machining to a mesh in areas with a high radius of curvature can create a surface that looks faceted. “You may still be within the machining tolerance of two tenths or whatever, but these parts may not be visually perfect. So the High Precision mode gets really close with the standard technique, then we push the cutter to the actual designed surfaces. Because when we’re that close to the actual surface patches, we can move the cutter on the surface with high reliability and the quality of the machined result goes way up,” said Levine.
Siemens has added what it calls “guiding curves” as “a different way to control toolpaths on complex shapes,” said Paradise. “It’s particularly relevant for five-axis machining where you’re trying to get a smooth path over a complex shape. It enables us to create paths that might, for example, automatically adjust and vary the step-over between different boundaries. You can select two edges and it will morph and create a smooth, flowing toolpath on that complex surface between the selected boundaries, almost like water flowing through a surface.”
Paradise said another area of improvement is the ability to predict and then adjust for what would otherwise be thin walls or pillars when roughing out an area using new high-speed cutting methods. “If you don’t see the creation of a thin pillar coming, it can wrap around and break the tool as it goes around. Or if you collapse the toolpath towards the middle and create a thin wall, that wall can tip over with the side force of the cutter and then wrap into the cutter and break it. NX automatically detects these cases and uses a helical engagement from the top down to mill the pillar out as opposed to wrapping around it with the tool,” he said.
Open Mind’s Levine added that CAM providers tend to focus on milling, but with the popularity of mill/turn machines and the prevalence of at least some turning in most shops, it’s essential to offer turning routines. “If you can solve it, they’re happy,” he said, “but if we had milling and no turning, a large amount of our business wouldn’t happen. Even if turning is only five percent of a customer’s usage, without software for it you’d get none of it.” Mund said Mastercam has expanded its Dynamic Motion engine into this area with Dynamic Turning. “Lathe button inserts offer the ability to cut in both directions, speeding the cutting process,” he said. “Dynamic Turning makes this even more efficient by adjusting the insert motion to maintain a consistent load on the cutter, just as it does with milling.” The resulting cutter path is not a series of even or linear cuts like a traditional turning path because the motion changes based on tool load. And just as it does with its milling counterpart, “the dynamic turning path yields a faster cut time and more even wear on the tool. And it can be used with any insert,” said Mund.
To some extent, these new capabilities rely on recent advances in computing power. Levine explained that all CAM developments are in response to customer needs, but they also have to be practical given the available technology. “Ten years ago, a computer may not have been fast enough to do all of the necessary steps that are happening in the background in some of these new techniques, so you would solve problems in a different way based on the environment. Timeliness of calculation is always a factor. If it takes two days to get a perfect calculation, most people still don’t want it.” This also points to the “black box” nature of all software. Most of us on the outside will never understand how it works.
When asked how and why CNC Software develops its solution, Mund pointed to the company’s three-pronged approach: “Our internal math engine, which is rock solid; practical testing in our manufacturing lab; and direct contact with the tool manufacturer to make sure that whatever ideal they had for this tool can be met in practicality with our software.” But all the major vendors truthfully make the same argument. Levine’s answer regarding software development was simple: It takes “a bunch of good mathematicians,” he said.
The second route of toolpath improvement is the development of routines that take advantage of specific cutting tool designs. Perhaps the prime example, which Manufacturing Engineering has covered in several recent articles, are end mills with side end profiles that follow a large radius, the center of which is well outside the center of the tool. Such tools have a barrel, lens, or oval shape, among other terms. Generally speaking, the odd profile of the tool does not match the profile of the part it is used to cut. Instead, as Mund explained, they are tilted in such a way that their “big, broad oval shape on the edge acts like a huge ball end mill.” That requires five-axis moves and software that “simulates a tool that can’t exist.” This also limits the areas such tools can reach, but for surfaces that can be accessed the results are “tremendous” both in terms of finish quality and material removal rates.
However, this example is not so much one of software taking advantage of a special cutting tool as clever software engineers driving the creation of a special tool. Levine recounted the history. “We have a department called ‘Innovation.’ This team really thinks differently from the rest of our company. They didn’t start with a strange-shaped cutter, or the desire to make a strange-shaped cutter. They started with the observation that finishing time felt longer than it used to because the industry had gotten so good at reducing roughing time. So, they asked the question ’How can we get better at finishing?’ [They then] designed a concept for a new style of barrel cutter, and took that idea to Emuge Corp. to prove it out.” Levine also said that although Open Mind has a “great sampling of customers that serve as sounding boards” and provide development suggestions, the company doesn’t always follow customer requests literally. “We prefer to develop something that solves the customer’s problem while also having broader applications, sometimes considering multiple vantage points,” Levine said. “And the toolpaths for the future developed by our Innovation department don’t always come from a customer. They sometimes come from our own observations and then working with customers.”
Another example of a tool-dependent advance is CNC Software’s partnership with Sandvik Coromant to create toolpaths for the Prime turning insert. Mund explained that the tool was intended to do two-way cutting, forward and backwards, which required a special software strategy. “It can look a little odd if you’re not prepared for it,” said Mund. “It’s also fantastic.”
In the earlier discussion of dynamic machining with CAM software, we noted that it created a toolpath with a “theoretically optimal engagement” of the cutter. The folks at CGTech, Irvine, Calif., argue that most CAM software doesn’t account for everything involved in the physical interaction between the variety of materials being machined and the variety of tools being used to cut them. The result, said VERICUT Product Specialist Pete Haas, is the widespread use of sub-optimal feed rates, which Haas considers one of the top three sources of waste in any machine shop. (The other two are poor programming and scrap, gouges, and rework.) To address this failing, CGTech introduced a product called VERICUT Force.
Force takes the output from any CAM package and breaks the moves into smaller blocks so it can make fine adjustments to the feed rate throughout the machining process to maintain truly constant chip thickness. (It does not change the trajectory.) And it makes those adjustments, said Haas, based on three factors: First, details about the tool, including helix angle, rake angle, number of flutes, and desired chip thickness. Second, a material database resulting from tests on 115 different materials. (The list is growing and CGTech will add your own exotic or proprietary material for a fee.) And third, “contact mapping of the cutting tool and the material that’s being cut in the program,” said Haas. “We know things the CAM systems don’t know by doing this contact mapping of every move in the program, block by block, with a tool. We’re taking slices through that cutting tool and then analyzing the forces across the entire surface through every move.”
The goal is a feed rate that produces the maximum safe chip thickness throughout the entire process, because that ensures the tool is doing as much work as it can within any given cut. Too thick a chip and you risk overloading the cutting edge and breaking the tool. But, as Haas also explained, too thin a feed-per-tooth also hurts tool life due to poor chip formation, in addition to lowering productivity.
Besides making the program faster, Force also makes it safer, explained Haas. “Because if your program produces a spike where you’ve plowed into some material—and I’ve seen programs that produce large spikes—that’ll be mitigated by Force. It will not happen, and you will not get that spike in the new NC program sent out to the machine.” As Haas sees it, “We’ve been upside down in NC programming. We’ve been setting one feed rate to do all the work when we should be setting chip thickness constant and adjusting the feed rate. VERICUT Force makes it easy to do it correctly.”
How effective is Force? The better your CAM package the less room there is to optimize. But as the CAM vendors themselves acknowledged, the product sells so it must be adding value. Haas said CGTech has had customers realize a payback within three months. And besides higher throughput, he’s seen up to tenfold improvements in tool life. Doubling is common. He also pointed out that unlike other means of improving the performance of a given toolpath, like add-on adaptive control systems, optimization from Force can be applied to multiple machines with one software license. “I can take your G-code right now, run it through Force, and put it down on the floor and in half an hour we’re cutting. I don’t need any hardware. I don’t need any extra software on the machine,” he said.
Finally, Force also produces charts that give the programmer a visual representation of areas in their program that can be improved, either by going back to the CAM system to fix things before optimization, or by letting Force tackle the opportunities. Haas described the charts as bringing “something to the programming world they’ve never had before. It’s a great tool I wish I had in my programming days.”
Connect With Us
