Piling Up Chips
High-feed milling strategies produce high metal removal rates
Milling strategies for removing a lot of metal fast, especially for roughing, have changed dramatically from the good old days, a time as recent as the mid-1990s.
Machine technology was just on the cusp of developments that would enable cutting tool manufacturers to design high-feed tools that could more fully utilize machines with lighter-duty spindles and advanced lookahead controls, among other features.
Potential benefits of high-feed milling strategies for manufacturers include:
- Ability to achieve high metal removal rate in roughing with lighter-duty, more- affordable machines,
- More reliable processing with consistent and predictable results in tool life, and
- Components machined nearer to net-shape during roughing operations.
The bottom line in milling is metal removal rate, which is easy to calculate. Multiply the width of cut by the depth of cut and the feed rate to find the cubic inches/min of material removed. Changing any of the variables—width of cut, depth of cut, or rate of feed—affects the size of the pile of chips produced.
In those good old days, mold and die makers and anyone looking to cube a workpiece or hog out a cavity would rely on machines with high-horsepower, low-rpm spindles and geared heads to take big depths of cut (DOC) with large milling cutters. Corn-cob cutters and large end mills, among others, were the tools du jour.
"Technology was so low at that time, even though high metal removal rates were achieved, that side walls of cavities had big stair steps that had to be removed with finishing tools," explains Roger Goble, west area manager, OSG Tap & Die Inc. (Glendale Heights, IL).
Although high-feed milling began with developments in indexable cutters, the first step toward high-feed machining of small-to-medium core cavities was taken using solid-carbide ball mills with small depths of cut. Applying known chip-thinning principles for round cutting shapes results in an increase in feed per tooth, and correspondingly, the machine tool feed rate. "Making that possible was the development of machines with spindle speeds above 8000 rpm that could track accurately with look-ahead software, and move at feed rates as high as 200 ipm [8 m/min] and above," Goble explains.
Then, a couple of years ago, some companies, among them OSG, introduced solid-carbide high-feed cutters for small-to-medium core cavities. Goble explains: "Basically, we can use an end mill which has a wider width of cut than a ball mill and has shorter flute lengths for rigidity compared with a normal end mill. Instead of sacrificing all that rigidity like a normal end mill with the flutes that are one and a half times diam, thereby weakening the cutter, the cutter has the ability to run on average between 300 and 500 ipm [12–20 m/min] because it's almost like a solid-carbide blank."
"What that does for us is make it possible to take smaller depths of cut and get near-net shape after roughing so we can go straight to semifinishing, or even to finishing, because we are able to get a lot more metal removal in a lot less time," Goble says.
Development of hybrid high-feed milling cutters has gone in two directions: high-feed cutter designs that include a radius that can be thought of as a portion of a larger diam ball mill cutter and cutter designs that feature a straight cutting edge inclined at a low angle. Both produce a low angle of attack to the workpiece and result in the desired chip-thinning effect for high-feed machining, and that are available in indexable inserts and replaceable-tip-style cutters.
"High-feed milling is achievable using a method of extreme chip thinning, produced with shallow entry angles or geometries, which are built into the cutter and inserts to achieve high table feed," explains Bruce Carter, manager of rotating products, Sandvik Coromant Co (Fair Lawn, NJ). "For example, tipping the insert in the cutter body to produce a 10° entry angle allows you to achieve a 6:1 ratio of feed per tooth to chip thickness."
Sandvik's CoroMill 210 utilizes a straight cutting edge with a 10° entry angle to achieve feed rates from 0.040 to 0.060" (1–1.5 mm) per tooth. At these feed rates, chip thickness is 0.007 to 0.010" (0.18–0.25 mm). "Because the CoroMill 210 is optimized for the operation, if you don't exceed the maximum DOC, the chip thinning factor is constant on the straight cutting edge," Carter says.
Design of the cutter body, insert seat, and the inserts allows combining two different operations—high-feed milling and plunge milling into the same tool. The CoroMill's 10° entering angle allows extreme feed rates at small axial depths of cut when the tool is fed tangentially and also high radial DOCs when fed axially in plunge-milling operations, producing large chip volumes.
"The CoroMill 210 is both a plunge and high-feed mill that can be used for squaring a block of material, roughing material off a blade or a frame component in the aerospace industry, or used by automotive or general purpose manufacturers for machining everything from cast iron to titanium, stainless or alloy steel," Carter says.
"Basically, high-feed milling cutters involve a lead angle or large radius that allows you to have higher feed rates based on chip thinning, which is the whole key behind high-feed machining," explains Thomas Raun, die and mold specialist, Iscar Metals Inc. (Arlington, TX).
When milling with a ballnose or button-type cutter, for example, varying the depth of cut results in a chip-thinning effect. Large depths of cut involve bigger chip thicknesses, while shallower depths of cut mean smaller chip thicknesses. "What that gives you when machining with smaller DOCs is the ability to increase the feed rate to get what you should get according to a basic mathematical formula that can be applied to calculate the proper chip load," says Raun.
Iscar's high-feed cutters come in two types: its Multimaster FeedMill replaceable-tip type for smaller diam tools and cavities in 10, 12, 16, and 20-mm, and FeedMill indexable-insert type consisting of end-mill and shell-mill style tools from 1 to 6" (25.4–152.4-mm) diam. For indexable-type cutters, "We utilize our advanced pressing techniques to create a boss on the insert which fits into a pocket in the cutting tool. This unique design results in the cutting forces being absorbed by the carbide insert and cutting tool, relieving stress on the screw, typically the weakest point of indexable cutters," Raun says.
The principles of chip thinning differ from traditional chip formation, explains Stephen Jean, milling product manager, Emuge Corp. (West Boylston, MA). "In conventional milling, as the tool begins to cut into the material to make a chip, it takes the most material when it first engages the work. Those chips are like question marks. If you could look at the force that it took to do that on a chart, it would be a sharp peak and then tail off.
"Chip thinning attacks in a different way. It eases its way into the cut in a more gentle curving approach. It sort of attacks the chip a little bit, and increases the depth of that cut and width of the chip, then decreases chip thickness by following the geometry of the cutting edge or the angle of attack," Jean says.
Emuge's Time-S indexable insert end mills feature a blended doubleradius cutting edge to distribute cutting forces along the entire cutting edge. Time-S is intended for machining cast iron and steels hardened to RC 44. Metal removal rates of more than 150 in.3/min (2458 cm3/min) have been achieved, using an 80-mm tool. "The geometry promotes chip thinning. If you would try to achieve the same amount of metal removal with a conventional tool and run it in this manner, it would consume a lot of power on the machine. It would vibrate and cause a lot more wear," says Jean.
"High-feed milling involves a light DOC that requires high machine feed rates to achieve high feed per tooth to avoid rubbing the workpiece," explains Jim Minock, product manager, Seco Tools Inc. (Warren, MI). "There are different ways to achieve high-feed cutting. We use a radiused insert that generates a small lead angle. The main idea is to have a low setting angle and push the cutter hard to achieve correct chip thickness."
The technique is growing in popularity because high-feed milling can be easy to implement in existing machine programs, sometimes requiring only changes to feed rates. Minock says that high-feed milling is helping mold and die shops win business back from overseas, because they can quote shorter lead times for diework.
"With high-feed cutting, shops aren't limited just to face milling. They can also do circular interpolation or helical interpolation, cork screwing through the part," says Minock. "What I've seen in mold and die shops is that they use 3-D profiling to increase productivity. To machine die sets faster, they take a hardened part and use a high-feed cutter and Z-level profiling to a point where they can get to a semifinished state, and then finish the workpiece by EDM machining."
"Using a button cutter in light DOC has really spurred the development of the hybrid high-feed cutter," says Konrad Forman of Ingersoll Cutting Tools (Rockford, IL). "When you start into a cavity with the button cutter, you will encounter problems when you come against the wall, so hybrid high-feed cutters with uniquely shaped inserts were developed to take advantage of chip thinning produced with shallow entry angles.
"Because the high-feed method transfers forces axially up into the spindle rather than radially with side-cutting pressure, the user can take advantage of lighter machines," Forman points out. "A high-feed geometry is really very much like a giant button insert operating at lighter depths of cut. The high-feed inserts can also reach closer to smaller corner radii on floor and side walls with less cutting tool pressure [wall contact] than if it were a more cumbersome button insert," Forman says.
Ingersoll Cutting Tools continues to develop products that promote high-feed cutting strategies with very high density (more teeth) and a larger corner radius in addition to the traditional high-feed approach of using very shallow lead angles. Ingersoll high-feed cutters have 2, 3, 6 (double-sided three), and 10 edges and come in a size range from 0.375 to 6.00" (9.5–152.4-mm) diam.
Its latest line, the Hi FeedDEKA cutter, has 10 cutting edges on a single insert, five on one side and five on another for 0.060" (1.5-mm) DOC, and 0.02" (0.51 mm) wiper format for semi-finishing capability.
"In Europe this high-feed strategy has caught on a little quicker than here in the US because European machines are well- suited to this machining style," Forman says.
"The high-feed cutters overcome the limitations of button cutters employed with large DOCs where they put a lot of heat into the cutting edge, leading to premature carbide failure and inconsistent machining results," explains Ingersoll's Mike Dieken. "The advantages of a high-feed milling strategy with hybrid cutters include, in addition to high metal removal rates, providing process reliability for untended operation and freeing operators to tend multiple machines."
ATI Stellram (LaVergne, TN) has introduced its 7792VXD family of milling cutters that take shallow DOCs to maximum cutting depth of 0.098" (2.5 mm), and operate at high feed rates. Metal removal rates are improved by as much as 90% when compared with conventional cutting in face milling, pocketing, slotting, and plunging. The tools are available as shell mills or with Weldon shanks. Inserts are available in 9 and 12-mm sizes, and feature four cutting edges.
The series of tools is being expanded by ATI Stellram to include smaller-diam cutters with cylindrical shanks and modular heads using 6-mm inserts, also with four cutting edges. Cutting forces are directed axially into the spindle, lessening spindle wear and improving stability. The X400 insert grade is standard with this tooling range, and is preferred for machining hardened steel. ATI Stellram also provides software to recommend cutting conditions and to calculate power, torque, and force requirements for a wide range of materials.
Walter USA (Waukesha, WI) has designed a high-performance cutter for higher chip removal volumes. The F2330 cutter offers plunging capability best suited to high-performance operations in the die and mold industry, as well as an extension length to eight times the diam. The coolant-through milling cutter is available in diam from 0.750 to 3.0" (1.9–76.2 mm). Maximum cutting depth is 0.078" (2 mm), and the setting angle is between 0 and 15° depending on the cutting depth. The tool is fitted with polygonal-shaped three-edge cutting inserts with CVD or PVD coating for milling steel and cast iron. Corner radii are 0.032, 0.047, and 0.079" (0.8, 1.2, and 2 mm), respectively.
This article was first published in the January 2007 edition of Manufacturing Engineering magazine.