High-feed milling (HFM) has been used for years to achieve high metal-removal rates, increase productivity and decrease workpiece cycle time. The roughing process—applicable for both solid-carbide and indexable insert tools—combines a shallow depth of cut (DOC) with a large cutting radius and small lead angle to ensure that the cutting forces are directed axially towards the machine spindle. It allows feed rates up to 10 times higher than normal rough milling.
Why should part manufacturers consider implementing HFM or, if they are already using the technique, consider more advanced HFM technologies?
According to Tom Raun, milling product manager, Iscar Metals Inc. (Arlington, TX), there are three key reasons. “High-feed milling is easy to implement, and because it takes a light axial DOC it can work with a broad range of gage lengths—including tool assemblies with long overhangs,” he said. “It also works well with modern CAM toolpaths, such as VoluMill and Mastercam’s Dynamic Motion, that allow users to cut more aggressively. Finally, HFM allows you to get to near-net shape quickly and set up subsequent semifinishing and finish operations. Because it uses a lighter step down, HFM does not lead to large scallops and large steps like a 90° cutter would, making finishing easier and more efficient.”
HFM began many years ago with button cutters and has grown from there, according to Shane Schultz, applications engineer, Sumitomo Electric Carbide Inc. (Mount Prospect, IL). “It’s highly versatile; with the proper insert geometry and setup for HFM, you can also mill holes via helical interpolation, open up holes, perform shoulder milling, create profiles, or do plain old slabbing, often in the same setup,” he said. “That’s helpful if you don’t have room for redundant tooling in your toolchanger.” The process also works well in low-horsepower machines, adding to their versatility.
Schultz agreed that HFM is particularly effective for long, 15–20″ [381–508-mm] reaches, deep cavities, tall fixtures, or large weldments. “I preach this in my seminars all the time,” he said. “In these situations, HFM is our first recommendation for removing material because of its high axial forces in Z. Other milling approaches are likely to produce tangential forces that cause chatter and vibration.”
Tyler Martin, STEP technician for Seco Tools LLC (Troy, MI), added that manufacturers should consider HFM for one key reason: productivity. “Advancements in grades and edge preparations have enhanced a highly productive machining method, helping to increase tool life and reduce power consumption,” he said. “More difficult-to-machine work materials are being used than 10 years ago, and HFM is an excellent choice for these materials.” For example, when machining gray cast iron or softer steels, HFM may not be a good choice, but for hard steels, superalloys, or difficult-to-machine stainless steel, HFM will almost always be the most productive choice, according to Martin.
HFM’s ability to reduce cycle time in hard materials or 3D shapes with tapered walls and/or curved surfaces is a key factor, according to Alyssa Walther, applications engineer, OSG USA Inc. (Glendale Heights, IL). “High-feed milling is also excellent at minimizing radial deflection, which will positively impact parts that require long reach from the tools,” she said.
Another important factor in HFM is that the orientation of the inserts in the tool direct most of the cutting forces back towards the spindle (parallel to the tool axis), with only a small portion acting perpendicular to the spindle (tool axis), according to Luke Pollock product manager, Walter USA LLC (West Waukesha, WI). This makes for a stable operation since the cutting forces push directly against the machine in the direction that provides the greatest stability. “That’s why this technique is very useful when trying to machine deep pockets where long extensions—which are inherently unstable—must be used.”
HFM uses light DOCs, but because of the insert orientation, it also employs high advances per tooth (APT). “If the workpiece is large enough, and the machine has the capability to move at high advancement rates, the metal-removal rate [MRR] can actually be higher compared to traditional face or pocket milling,” said Pollock.
Cutting tools required for high-feed milling differ from standard milling tools in several ways. Typically, a high-feed tool has a lead angle of 10–20° from the surface being machined, according to Martin. This lead angle helps thin-out the chip and allows for much higher feed rates than conventional-style cutters.
Walther added that HFM tools have either a very large corner radius or a specific “cutting angle” ground into the end face of the tool or insert. “At small DOCs, either configuration allows for smaller true chip loads, which in turn allows higher feed rates,” she said.
High-feed mills are differentiated by the design of the insert and the way the insert is oriented in the cutting tool, added Pollock. “The large lead angles generate a high chip thinning factor, where chip thickness is something less than the APT. In these cases, a feed rate multiplier—calculated by dividing the recommended APT by the cosine of the lead angle—should be used to achieve the desired chip thickness. This adjusted value should be used to program the feed rate.”
Toolholding and workholding requirements for HFM are also somewhat different than standard milling operations. In high-feed operations, the tool should be held tightly and true due to the forces put on the part, according to Sumitomo’s Schultz. “Traditional collets and end mill holders, with two set screws to clamp the tool, will typically push the tool off center, producing runout and hindering tool life and tool performance. With 1″ [25.4-mm] indexables, it’s better to use a milling chuck, hydraulic chuck, or Rego-Fix type holder—not ER 32 collets or expandable collets. The latter are generally weak, and there is a lot of Z axial force being pushed down onto the part, and because of the high lead angle, forces are pushed back up into the spindle. You need a tool that is stable, rigid, and doesn’t move or push up into the toolholding system.”
Martin pointed out that a fixturing system is only as good as its weakest link. “In high-feed milling, since much of the cutting force is directed into the spindle, tools can perform at longer gage lengths than can a conventional cutter. This can also be easier on the spindle because less lateral force is being put on the connection interface. HFM can prove difficult on parts with poor fixturing or unsupported areas because of the force direction as well.”
HFM cutters can actually provide assistance to some clamping systems, according to Walther. “Since cutting forces are mainly directed along the centerline axis of the tool, and towards the direction of the spindle, this creates a very stable and vibration-resistant machining environment,” she said. “It is an excellent option for weak clamping situations.”
However, as with any milling application, the stronger the hold on the tool and the truer the holder keeps the tool on center, the better the tool will run. “Typically, mill chucks and hydraulic holders are ‘beefier’ holders and offer the best rigidity, excellent holding strength, and as such, natural vibration dampening,” said Walther. “While shrink-fit holders aren’t typically as robust as a mill chuck or hydraulic holder, they have excellent holding force on the tool shank and offer high runout precision.”
Taking advantage of the benefits of HFM requires a machine with the capability of feeding at elevated rates. Sometimes, machining can even be done in rapid mode on some lower capability machines because the APT is so high, according to Pollock. “Primarily, though, the machine has to have good look-ahead capability, the ability to process machine code quickly, and the fluidity to make the required movements,” he said.
Another key factor is to size HSM tools to fit the machine, according to Iscar Metal’s Raun. “For example, a 2″ diam [50.8-mm] indexable cutting tool is a very common size, and many people apply it on CAT 40, CAT 50, HSK 63 and HSK 100 machines alike. However, based on machine power alone, most CAT 40 machines—particularly older ones—don’t have the horsepower and torque to effectively use 2″ indexable cutters. In those cases, they must be run at lower feed rates and DOCs, which reduces cutting efficiency. In these situations, you will likely find you can do just as much or more with a 1.5″ tool as a 2″ one because you can use deeper DOCs and higher feed rates.”
Martin agreed. “A typical 3″ [76.2-mm] high-feed mill running in steel can easily achieve MRRs that will nearly stall out a 30-hp [22.4-kW] machine. In addition to horsepower, traverse [feed] rate is often a constraint as well. Many older machines may max out at 200–300 ipm [5080–7620 mm/min] and can constrain the ability of the tool to achieve maximum productivity. If we take the same 3″ cutter and run it in steel, the recommended starting feedrate is at least 250 ipm [6350 mm/min].”
The machine’s CNC must be able to process lines of code fast enough to be able to feed the tool to its capability, added Schultz. “Some 1980’s-vintage machines may not able to feed faster than 40 ipm [1016 mm/min], and high-feed milling feeds will be 10 times that, so you should evaluate your CNC to see if it is capable of running HFM. It is possible to apply new high-feed mills on older machines, but they work best with large cutters because feeds and speeds are not as accelerated.”
Walther added that, without good look-ahead software, circular shapes will be misinterpolated into polygons. “Machines with stronger and faster acceleration capabilities are also more beneficial for smaller workpieces.”
The type of HFM tools selected depends on the type of work materials being machined. “For heat-resistant alloys like Inconel and Hastelloy and other nickel-based alloys, I lean toward a positive insert, meaning one-sided, that has relief and is freer cutting,” said Schultz. “A double-negative, double-sided insert is a good option for carbon steels and easier-to-cut materials.
According to Martin, positive axial rake tools will be better for superalloys, titanium, stainless steel, and negative geometries can be better for difficult steels, hardened steels, and cast iron. “A heavier edge preparation and a neutral or negative rake angle that works well in hardened steel can create difficult work-hardened areas in a stainless steel,” he said.
According to Raun, both the type of work material and the frequency with which a shop changes out jobs and work materials are critical factors. “The mantra I try to impart to field reps and customers is that you have to look at tools in terms of versatility vs. being application specific,” he said. “If you are looking for versatility, use a tool like our H600 that you can switch back and forth between jobs with different materials. We also have different grades and geometries that allow you to machine the whole ISO materials group. But we also have application-specific tools for processes where you are trying to squeeze out every bit of efficiency. For example, our FFQ4 is more efficient for shearing ISO M and ISO S materials due to radial and axial positioning. It’s not that the H600 can’t do it, but the FFQ4 does it better.”
Pollock agreed that different materials require different approaches. “At Walter, we have three types of high-feed mills. A positive insert geometry with three cutting edges cuts smoothly and cleanly without generating much additional heat, so it’s perfect for soft materials or stainless steels. We also have a high-feed mill with negative geometry with six cutting edges on the insert. Because it’s negative, the insert has a much stronger cutting edge, but it generates more heat and cutting force and is better suited for abrasive materials such as low-carbon alloy steels and cast irons. Our third style uses a four-index positive insert that can be used in different milling bodies.”
As in other areas of machining, recent advances in tooling technology are making HFM more productive and more efficient. Seco Tools’ most recent HFM advancement is the High Feed 6, a free-cutting double-sided insert. “It cuts like a tool with a positive axial rake but gives the economy of a double-sided insert,” said Martin. “This tool can help customers cut costs in machines where feed rate or horsepower is a constraint.”
While the basic features of high-feed cutters remain the same, tool substrates, coating technologies and grinding technologies continue to improve, according to Walther. Features that improve chip shape, chip control and surface finish are also important advances. “For example, the new OSG HFC-Ti solid-carbide high-feed end mill is designed not only for extremely high feed rates, but for simultaneously floor finishing in titanium alloys,” she said. (Floor finishing is a process for finishing the floors of pockets in precision parts.) “The OSG PHC high-feed indexable cutter has insert grades XP2040 for stainless steels and XC5040 for heat-resistant superalloys. These inserts are optimized at their cutting edge geometry, substrate and coating for just such materials.”
Sumitomo recently introduced two new inserts that are effective for HFM. “Our WFXH utilizes high-positive, square inserts that allow us to reach DOCs up to 1 mm, with a lighter feed rate than a standard high-feed mill but with lower cutting forces. It’s designed for less rigid, high-speed machines,” said Schultz. “Sumitomo has also developed a double-negative style cutter with a square insert that provides eight cutting edges. It is in field testing and due to be released soon.”
However, Sumitomo’s established Trigon-style inserts, with three cutting edges, are HFM workhorses. “The Trigon is considered a 90°-type tool, but it has relief and clearance for chip evacuation, and has the best lead angle compared to round or square inserts” said Schultz. “The first edge has a flat facet that works as a wiper on the bottom that can maintain surface finish, the second edge has a high lead angle for chip thinning, and the third, and most important for versatility, edge has a radius around the outside corner to do angles, walls, profiling and 3D profiling. It allows us to get close to our finish dimensions, unlike some other geometries.”
The MSX, which holds Sumitomo’s Trigon style insert, is probably the best high-feed technology the company offers, according to Schultz. “We offer four different inserts ICs [inscribed circles]: 6, 8, 12 and 14 mm.” He added that Sumitomo offers Top Clamp, an extra clamp with a screw in the center that adds extra rigidity, and dependability to cutter performance, when needed, to a tool setup.
Walter’s latest HFM development is the M4002 product family, part of the M4000 “system insert” program: one insert can be used in a variety of different milling tools commonly found in machine shops, including 90° face mills, high-feed mills, center cutting end mills, 45° face mills, chamfer tools, and T-slot cutters. “Only one insert needs to be purchased, inventoried and consumed, allowing the end user to maximize economy of scale and make buying and storing inserts easy,” said Pollock. He added that M4000 inserts are available with Walter’s latest coating technology, Tiger Tec Gold (WKP35S), an ultra-low pressure CVD process for coating milling inserts used to machine steels and cast irons.
Iscar is going back to the future with its new HFM tools. “Within the past year, we introduced the FFQ4, which goes back to the old single-sided cutting tool design, for difficult-to-machine materials,” said Raun. “It provides flank relief and more positive axial and radial relief angles, which help reduce heat better than double-sided technologies, like our H 600 feed mill. Also, we reduced the lead angle on the FFQ4. Typically a feed mill will have a 12–17° lead angle, but with the FFQ4 we reduced it to 9°. That plays nicer with lighter duty machines and long overhang environments.”
For ISO S and ISO M materials, Iscar is seeing large increases in tool life and improved wear characteristics with its IC882 insert, which has a hard PCD nanolayer coating, and the IC5820, with a CVD coating. As with its other tool coatings, Iscar uses a post-coating smoothing process on its two new inserts to improve chip flow over the rake, which produces a cleaner, more accurate cutting edge.
Also, in four to five months Iscar will be releasing a new family of tools that it says will be very effective for HFM. “We came out with our H600 family in 2007, and it’s been a great HFM tool for a decade, but now we are going to have the new best thing,” said Raun. “Stay tuned!”
Connect With Us