Machining In Circles

By converting conventional point-to-point contouring programs to arcs, shops are slashing program lengths, boosting average feed rates, and getting better surface finishes.


Facebook Share Icon LinkedIn Share Icon Twitter Share Icon Share by EMail icon Print Icon

Almost since the beginning of NC, the way in which milling machines generate a curved tool path has changed very little. Any form that can't readily be described with a standard circular or higher level interpolation routine is instead defined as a series of points tracking over the intended tool path, and interpolated directly from point to point. And so what is intended to be a smooth flowing surface is in fact a lengthy series of linear cuts.

Geometrically speaking, lines aren't a terribly good way to represent curves, of course, but that paradigm has been enforced by the very nature of conventional motion control technology. So shops hoping to cut surfaces that are both accurate and relatively smooth have little choice but to have their programming systems spit out points by the millions to make those linear moves as small as possible. CNC technology has improved enormously, however, and today's state-of-the-art controls can process those programs at much higher speeds and accuracy than were possible only a few years ago.

That's great technology if you have it. For now, though, most shops are left to cope with the substantial drawbacks imposed by having to run programs with all those points. Huge NC files. Compromised feed rates in order to maintain accuracy in tight contours. Stuttering cuts as controls struggle to process dense point (block) clusters. And that's not to mention the rough surface finishes that must be ground out by hand.

There is a relatively simple alternative, however, that goes a long way to alleviating many of the constraints imposed by point-to-point contouring, even on rather modestly appointed CNC machine tools. The basic idea is to use a succession of arcs rather than line segments to construct curving tool paths, and then to execute those arcs using the circular interpolation capabilities of the CNC. Practically speaking, this technique will limit the machining process to 2D cuts in the three primary machine planes (X-Y, X-Z or Y-Z) on most machine tools. But those cuts typically will be much smoother and oftentimes defined with less than a tenth of the program data in comparison to point-to-point contouring. Moreover, the fine finishing of a cavity can generally be accomplished at a much higher average feed rate, not just because the CNC block processing speed barrier is lifted, but also because of the ability to manage programmed feed rate more intelligently and dynamically across the entire part program. For die and mold makers, these capabilities add up to less time on the machine and on the bench.

Here's how it's done.

Filtering Points

A handful of NC programming systems have the ability to output part programs in the form of arcs. Essentially, they generate the base tool path geometry in a conventional manner--that is, in the form of points--and then systematically fit arcs of various radii to that data end to end, based on a prescribed accuracy tolerance (much like the cordal deviation used in point-to-point tool path generation) and a minimum standard for continuity where each arc intersects with another. Then the program is output in the form of circular interpolation commands that are sequentially executed by the CNC.

For shops without arc fitting capabilities in their programming system, arc-fitting programs are available that can read the output of a range of CAM systems, and then produce a new post processed file in the form of arcs. One such product is NWD SuperCut developed by Northwood Designs, Incorporated (Antwerp, New York). Earlier versions of the software were known as The NWD Filter, and worked only in conjunction with Mastercam. But the newer version handles just about any combination of CAM systems and controls.

Speaking more specifically as to how the arc-fitting process works, Northwood's president, Bill Elliott, says that they do not actually interpolate the points of the original part program--that is, to draw arcs that intersect each point. Rather, the process is more aptly described as a complex mathematical averaging of the original program data that factors both the position of each point as well as the line segments in between.

In the vast majority of cases, says Mr. Elliott, the arcs will more accurately reflect the true geometry than the points from which they were generated. It all has to do with the natural ability of arcs to fit to a curve. Where curves blend into flats or near flats, however, it does make sense to switch back to linear moves, and the system has the intelligence to use whichever entity fits best.

Because an arc can represent a far larger portion of the base curve than a line segment within a comparable accuracy range, this is how the substantial part program data reductions are achieved. The actual reduction depends on the surface topology, of course, but tool path files that have been converted to arcs are typically 60 to 90 percent smaller than the point-to-point programs they replaced.

Interestingly, the more points that are used to define a tool path, the fewer arcs will be required to accurately define the same path. It all has to do with the logic by which arcs are fit to the data. In very simple terms, if the point data is relatively sparse, the system is going to make more conservative assumptions about where the true geometry is supposed to be, and consequently has to use more entities to define the path. If the point data is plentiful, however, fewer such assumptions are necessary, and the system can make each arc as long as possible without compromising accuracy. The result is both a smaller and a more accurate tool path file. A good approach, then, is to set the cordal deviation smaller than normal when initially generating the points. While that will take some more processing time in CAM, the payoff is well worth the cost.

Smaller NC files mean less need to drip feed program data through DNC or some other auxiliary memory, but that's only the beginning of the benefits of this methodology. Particularly on older controls, slow block processing capability usually proves to be the limiting factor on actual contouring feed rates in point-to-point programs. And many shops, wanting to avoid conditions of data starvation, program for the worst case scenario--that is, for the tightest curves with the densest point spacing--which means that the rest of the program is executed at excessively slow feeds. With arcs, the achievable feed rate ceiling is substantially raised, if not eliminated altogether. Cavities can be cut faster and with a better surface finish.

As feed rates increase, however, another issue comes to the fore: cutting accuracy. New high-performance CNCs have excellent look-ahead capabilities with the ability to automatically decelerate and accelerate the feed where necessary in order to keep the tool from straying too far off its programmed path. Not so with more modestly appointed controls, which leave programmers again with the dilemma of having to anticipate the worst case, and set the feed accordingly. That rate may be higher with arcs, but much of the program will still have to be run slower than necessary in order to maintain accuracy in the tight curves. Some programmers might attempt to deal with this issue by manually resetting the feed in various portions of the program, but for the huge files common in die and mold machining, that approach is not terribly practical. More likely, operators hoping to "optimize" a routine are forced to play "dial-a-feed," standing at the machine and manually adjusting the feed rate override with each pass of the tool.

But with each arc comes a simple bit of information--the radius--that provides a better means to dynamically manage feed rate. The NWD software, for example, allows the user to establish a maximum feed rate for arcs of any radius. And when the program sees that the maximum feed for an arc is less than the programmed feed rate, it automatically adjusts the feed to the lower rate. Then when the path begins to flatten out again, it resets the feed to the maximum allowable rate. In order to establish a maximum feed discipline that covers all cases, the programmer enters maximum feed values for a representative sampling of radii across the entire arc range. The NWD software then essentially runs a curve through those data points, creating a case-sensitive upper limit across the range.

As for how to establish an appropriate maximum feed curve, Mr. Elliott suggests this simple test: On the machine tool, slowly cut a one-inch radius circle in a test piece. While keeping the tool repeating over this same circular path, slowly increase the feed and listen closely. When you hear the tool hit metal again, meaning a deviation from the intended path, that is the maximum feed for a one-inch radius arc. Repeat this same test for a sampling of five or six circles of various radii, and that should provide a very good basis for nailing down a safe operating range for the machine.

We should point out here that the automatic feed rate adjustment is not itself a look-ahead function. In the part program, each new feed rate comes in the same block that identifies the arc coordinates and radius. So over-travel is still possible if, say, a full-feed move blends abruptly into a small radius arc. But, says Mr. Elliott, even controls with limited look-ahead functionality should be able to "anticipate" and manage such events. And because each arc describes so much more travel than a line segment, the look-ahead range of the control in effect is extended by a similar amount. Moreover, the software is able to detect when a sudden directional change occurs in the tool path and then automatically switch to exact stop mode. Such a capability comes into play, for instance, when a tool path across the bottom of a cavity comes to a steep side wall.

Making Electrodes

Global Precision (Davie, Florida) has been using the arc-fitting method to prepare part programs for about a year. The largest share of Global's work is in making multiple cavity plastic injection molds for the packaging industry, and snap-top closures are a particular specialty. They also make a wide range of precision molds for electrical connectors, medical device components and other demanding applications as well.

Virtually all of Global's cavities are finished with ram EDM, so the majority of their precision machining is done on copper and graphite electrodes. The company possesses a deep understanding of the EDM process, and that drives the standards to which electrodes are made. According to CNC supervisor Rick Zicarelli, virtually all 3D surfaces are held to a tolerance of ±0.0002 inch, a dimensional standard that essentially rules out any aggressive post-machining finishing operations that run the risk of taking out too much material. They must machine the electrodes virtually to the final finish.

While stringent accuracy standards certainly ensure close adherence to the base geometry, the larger issue to Global is to maintain a high degree of consistency from electrode to electrode. According to EDM manager Rich Eggleston, a 0.0005-inch variation in electrode size is too much to maintain their desired level of process control. While Global does have the equipment and skill to compensate for such variation by manipulating the orbiting path, they'd rather not. Many jobs require multiple electrodes, loaded with electrode changers, and run unattended--and they certainly would not want to "comp" all those tools individually for reasons of both quality and efficiency. Far better to get the electrodes right from the start, and not have to deal with exceptions.

When Global was cutting these surfaces point to point, it simply wasn't practical to consistently machine to this level of accuracy. Too much data in the programs. Too much time in the cut. And still too much hand finishing. Now the surfaces are programmed in Mastercam (CNC Software, Tolland, Connecticut), and the tool path is converted to arcs with the NWD software.

This way, Mr. Zicarelli has much more control. He may set an arc tolerance as small as 0.000001 inch to get a fine finish on an electrode, use tools as small as 0.010 inch in diameter, and stepovers as small as five "tenths" (0.0005 inch). In comparison to trying to do the same work point to point, Mr. Zicarelli figures they've seen reductions in program length from 50 to 90 percent. Consequently, they have been able to machine as much as three or four times faster, and without the feed stutter they often encountered when cutting point to point. While Global hasn't been able to eliminate post-machining handwork entirely, nowadays it's just a very light touch-up. And most important, the electrodes consistently meet their high quality standards.

Cutting Steel

Bourhis Mold (Hawthorne, California) makes plastic injection molds and die cast dies for a blue chip list of West Coast customers. They also, through arc cutting, have come to the point where their machined surfaces require relatively little benching, but that wasn't quite the aim starting out.

Bourhis put in their first CNC machine in 1991, a Fadal 6030 vertical machining center, and since have emphasized a CNC approach to all their work, and with considerable success. Long part programs were a problem, however, as they ran into technical difficulties trying to drip feed data to the control. So they initially were just looking for a way to reduce program length. "We tried using a larger cordal deviation (in CAM)," says operations manager John Carroll, "but that produced too coarse of a surface, and the finishing would take forever."

When Mr. Carroll began filtering the programs into arcs, the program data problem was solved. Then they came to realize the equally powerful capability of dynamically managing feed rates. A mold for the back of an airliner seat proved the point. The cavity was a long, nearly flat surface--the sort of geometry that can be cut very fast--but with a small radius at the ends blending into the diagonal wall. While that little radius was easy enough to cut, it ruined the opportunity to cut both fast and accurate across the entire cavity. When this form was cut point-to-point, says Mr. Carroll, he'd program the whole job at 200 ipm knowing that the feed would be overridden at the machine. They'd end up running the whole job at 20 to 30 ipm. With the ability to dynamically alter feed rate, however, the flats could be run flat out, and just the radii at the lower feed. And a job that would have taken 10 days to cut was done in less than three.

Bourhis also employs NWD's "uni-directional filtering" technique that helps to further smooth the cut surface. What's that mean? When tool paths are generated conventionally for zigzag cuts, the line segments or arcs for each successive pass are calculated from opposite directions. This means that the endpoints of side-by-side entities rarely match, which has a detrimental effect on surface finish. With uni-directional filtering, each pass is calculated from the same direction, which creates a much smoother cutting pattern throughout.

The net result is that Bourhis also has cut bench time way down, to a tenth of what it once was. "Now we just stone it and it's done," says Mr. Carroll. Moreover, he believes that the combination of faster cutting and less benching has increased the shop's output capacity by as much as 15 percent.

Will everyone get those kinds of results? That's hard to say, because so many things still depend on the application, and how shops deal with all the other process components of machining sculptured surfaces. But the arc fitting method does have an ardent following among a growing number of die and mold shops that are finding it allows them to get more firepower out of their existing arsenal of tools.

What About Curves In The Control?

The ideal situation for machining sculptured surfaces is not to have to approximate the original surface geometry at all, but to import it into the CNC and cut directly from that data. While direct surface machining may seem a remote possibility, some control builders are quickly moving down that path. Siemens already has a CNC that internally represents all geometry in the form of NURBS (non-uniform rational B-spline) surfaces and curves, and Fanuc recently has announced similar capabilities as well. Of course, having such capability in a CNC does not necessarily mean that it will be easy to import surfaces from a wide range of commercially available CAD/CAM systems, at least as the technology is configured today. Northwood Design is working on that issue, however, and also has software with the capability to convert point-to-point tool paths to NURBS curves, much in the same way they now work with arcs.


  • DNC: Faster And Better -- Part One

    Direct numerical control (DNC) should solve problems, not create them. If you under-stand how DNC works and follow the tips presented in this article, you can maximize its benefits and avoid headaches with your system. Part One of a two-part series.

  • How to Slash 5-Axis Finishing Time

    Finally there is an alternative to ballnose endmills for finishing 3D parts. The combination of finishing tools shaped to provide more cutting surface and a CAM system with the ability to apply them on a five-axis machining center can dramatically reduce finishing cycle times while delivering better surface finishes.

  • Understanding NURBS Interpolation

    The right way to program curves? A solution to yesterday's problems? The truth is probably somewhere in between.