End mills, traditionally made with two to four flutes, are used in one of the oldest mechanized machining processes—milling. Cutting-edge software, machine tools, novel strategies, ever-improving techniques and design updates in the tools themselves keeps milling useful in the 21st century. The machinist who masters the art of these metal eaters can save their shop time and money while producing superior parts.
“In a typical, traditional approach, when machinists use end mills for more material [removal], more roughing, and if the tool is buried more, the fewer flutes they would use,” said Drew Strauchen, executive vice president at GWS Tool Group, Tavares, Fla. “With conventional wisdom, roughing uses two- or three-flute end mills and semi-finishing and finishing operations uses more flutes—four, five and beyond.”
Tradition and convention are subject to change, though.
“There are many modern machining techniques and strategies that really turn [that wisdom] on its head,” said Strauchen. Now, faster machines with more horsepower and faster, more precise spindles have made possible aggressive machining strategies like high-efficiency milling (HEM), also known as dynamic milling, and trochoidal milling.
“Dynamic milling is defined as a method that is done with a large axial depth of cut (DOC) and small radial DOC to reduce the engagement time of the cutting edge of an end mill, which reduces the force load on the tool and spindle and the generation of cutting heat, while increasing the amount of material removed,” said Tyler Hashizume, product engineer II, OSG USA Inc., St. Charles, Illinois.
Dynamic milling relies on the ability of CAD/CAM software to create a trochoidal milling program; a milling machine to read complicated trochoidal programs at high speed; and a machine that can rapidly move the spindle and table.
“Once these conditions are met, it is possible that not only high efficiency is achieved, but also that tool life and the life of the machine spindle are greatly extended,” said Hashizume. “In such an environment, it is less important to consider chip evacuation by enlarging the chip pocket of the end mill, but rather how to increase the number of flutes to increase the tool rigidity and feed rate to achieve high efficiency.”
In contrast to the linear radial toolpath in conventional machining, trochoidal milling uses a spiral (or D-shaped) toolpath with a low radial DOC to reduce load and wear on the tool. Since trochoidal milling uses a tool to machine a slot wider than its cutting diameter, the same tool can be used to create slots of varying sizes. This can free up space in the tool carousel and save time on tool changeouts, depending on the requirements of the part.
These strategies change the way a machinist tackles a job, and it’s becoming popular for machinists to use multi-flute end mills—those with five or more flutes—to do both roughing and finishing, eliminating the need to fill up the tool carousel with an array of different end mills. These modern strategies mitigate the need to bury the tool into a part and any worries about getting chips clogged up in the flute gullets, which can lead to a broken end mill and the failure of the part in progress.
By eliminating the need to change out one mill for another and employing more cutting-edge techniques, today’s machinists can go faster, which leads to increased productivity.
The question is how can a machinist seemingly defy the laws of physics and use the speed of a higher-flute tool without clogging it with chips and causing it to break? The answer is in new programming strategies. Today, CAD/CAM software, with sophisticated toolpath generation built in, allows programmers to generate more efficient toolpaths that are speedy but prevent the tool from getting into danger zones. The software’s approach is very specific, so the mill is never over-engaged with the part. Users can tell CAM software, “I don’t want to exceed this amount of tool engagement,” and the application will create the toolpath necessary to ensure the tool never gets engaged beyond the point he defined.
Edwin Tonne, training and technical specialist, Horn USA Inc., Franklin, Tenn., said the perceived application for multi-flute end mills is for semi-finishing and finishing workpieces. “But, actually, if the shop is willing to re-program the job multi-flutes can be used to rough and to pocket as well,” he said.
Tonne agreed with Strauchen that modern CAM software is what helps make possible processes like trochoidal milling and high dynamic milling. “CAM software has gotten really good at high dynamic milling, where it’s managing the chip thickness,” he said. “So, you can use that in a roughing operation.”
Tonne also agreed the software enables processes that lead to higher productivity. With trochoidal milling “you have some unproductive time in the cut but [the process] more than makes up for it because you can take a really big axial DOC, even with a small end mill,” he said.
The newer processes enabled by modern CAM software are a boon for machining hard materials that need to be machined with low radial engagement, which otherwise would risk breaking the end mill. For example, when machining steel greater than 50-60 HRC, a two-flute end mill probably will snap.
“But using a multi-flute end mill with high-speed techniques and low radial engagement you can mill a slot or any kind of feature in it,” Tonne said.
Newer software and machining techniques can even help make an older machine perform like a shiny new model. “If they have machines even with moderate speed, a lot of times an older machine that has moderate capabilities—if it’s partnered with a new machining strategy—can still take advantage of modern high-efficiency machining and toolpath strategies,” said Strauchen. “The best way to figure it out is to bring specialists in that are savvy with modern programming techniques … and help customers maximize what they have.”
There’s even more encouraging news for smaller shops when it comes to multi-flute end mills and CAM software. “They’re great tools for low power and smaller taper machines like 40-taper because with multi-flutes we’re taking deep axial cuts and balancing the radial forces by using the length of the tool for stability,” said Matt Clynch, national product specialist-milling, Iscar USA, Arlington, Texas. “With those smaller taper machines, if we take deep radial cuts with the large widths of cut it would start to bend and the assembly topples.”
Using these tools in an HEM/VoluMill environment (toolpath software from Celeritive Technologies, Moorpark, Calif.) will mitigate assembly disasters, he said. This approach can make the smaller tapered machines competitive with larger taper machines. “The metal removal rates we can achieve are very close if they aren’t in fact beating the standard way to rough material out on bigger taper machines like 50-taper and HSK A100,” Clynch said. As a result, a wider segment of the industry can be competitive because smaller taper machines are less expensive and easier to learn.
“All the CAM systems have different names for this type of programming,” he said. “HEM, VoluMill—there’s all sorts of them. If you really want to give it a blanket name it’d be ‘optimized roughing.’ These CAM systems have made it so easy, you just say this is my percentage of diameter width of cut and it does a lot of the back figuring for elevated surface footages and correcting of feed rates. It figures the tool path for you. It’s just made it so much easier for the small guy to be competitive.”
However, Clynch offers several cautions. When using this strategy, a machine tool’s acceleration/deceleration rates have to be higher because with the smaller moves the tool makes, the machine has to ramp up and down more to adjust the speed. The machine tool needs more memory for longer programs and it also needs enough “look-ahead,” or buffer space, to run smoothly. If the machine can’t read the code fast enough, it jerks, stalls or dwells trying to keep up, he said.
How can the use of multi-flute end mills lead to higher productivity if they take such small bites of metal? “Because the normal operation of the multi-flute is decreased radial engagement, let’s say less than 25 percent of the diameter, the arc of contact is smaller,” said Horn’s Tonne. This allows the use of two to three times the normal cutting speed range.
The DOC can also be increased. For example, the machinist could run a process using a 5/8" (1.6-cm) diameter, two-flute end mill on titanium 6AL-4V at 130 sfm using full slotting and 1× the diameter DOC for productivity of 1.49 in³/min. (24.4 cm3/min.). Doing the same process with an eight-flute end mill with 230 sfm and 0.019" (0.048-cm) radial engagement or width of cut and 2× the diameter depth of cut increases productivity to 1.57 in³/min. (25.7 cm3/min.). “So, the net gain on productivity is significant,” said Tonne.
By adding flutes, the machinist can decrease the feed per flute and still maintain the same feed compared to an end mill with a lower flute count. For example, for a four-flute end mill running 0.002" (0.005-cm) per flute, substitute a five-flute end mill and maintain the same feed with decreased pressure per flute. “So, you get a little more flexibility in your tool wear without decreasing your productivity,” Tonne said. “The linear feed rate can stay the same and the cycle time will stay the same but you’re decreasing the section each flute has to take.”
Don’t equate cycle time with tool life, though, said Clynch. Just because a machine ran six hours, that doesn’t mean it used six hours of tool life. The end mill may have only been engaged with the workpiece a fraction of that time due to the short arc of contact. “Pay close attention to this to make sure you are getting the maximum [life] out of your tools,” he said. “If not, you may be leaving money on the table!”
With a higher number of flutes, though, chip formation and evacuation become concerns. Mitigate these concerns by adjusting radial engagement and table feeds to the application and target material; choosing the correct tool for a specific application; and selecting tools tailored for a high number of flutes—for example, those with a specific core design enabling bigger flute space toward the front end, or a design that optimizes chip formation.
“Very important is the amount of coolant that can be provided and ensuring that the coolant stream direction maximizes the chip evacuation out of the cutting zone,” said Bernd Fiedler, senior product manager-solid end milling, at Kennametal, Fuerth, Germany. “Sometimes high-pressured air can be a good option to remove chips out of the working area and prevent chip clogging, especially in pockets. ”
The higher the number of flutes per given diameter, the smaller the flute space on the end mill, Fiedler said. Depending on the material and its specific chip formation behavior, sufficient chip evacuation is critical and needs to be closely observed. In general, cut-off material moves down to the core and then breaks or rolls into chips, but it’s helpful to know how to read different materials and their tendencies. Steels up to 45 HRC, depending on the type of alloy, tend to roll and then break. Hardened steels are brittle and create thin chips. In general, stainless steels have less tendency to roll, but this is also heavily dependent on the alloy. Cast iron breaks into dust particles. Titanium tends to curl and fills up the available flute space quickly.
“There are several general indicators that chip formation is insufficient,” Fiedler said. “Chips are very curled or rippled, have no uniform edge, or they are deeply colored. For instance, when the side that rolls over the cutting edge is no longer shiny but shows color changes.”
What to do if chip formation doesn’t look right? “Unfortunately, there is not a simple answer to this. It depends on the application and material,” said Fiedler. In the case of chips changing their color, the coolant supply into the work zone needs to be improved. Vibration might be the cause of all this, so the tool and workpiece clamping need to be checked. Modifying the feed rates and axial DOC can also help. Curling and ruffling of chips often indicates feed rates are too high, so adjusting the feed rates can help, but it is important to maintain sufficient average chip thickness
Is there a limit on the number of flutes for one end mill? The primary method of manufacturing end mills is grinding using automatic NC grinding machines, said OSG’s Hashizume. As long as they are manufactured using such machines, the capabilities of CAD/CAM applications and the grinding machines themselves (especially the size of the grinding wheel) impose limitations on the number of flutes it is possible to create. “The larger the OD of the end mill manufactured, the bigger the space that can be used for one cutting edge, and the more cutting edges that can be manufactured,” said Hashizume. The maximum number of flutes depends on the diameter of the tool, Tonne agreed.
From what he’s seen in the industry, 20 flutes on a 1.25" (3.18-cm) tool is the maximum. “With that many flutes, the radial engagement due to the limited usable flute volume is much less than 10 percent,” he said. “So, you start to diminish the practicality in most applications or limit your work to pure finishing and not much else.”
Don’t forget about the material you’re removing, said Clynch. “In theory there is not a limit, but you’ve got to have some place for the chip to form correctly,” he said. For normal, everyday materials like ISO P, ISO M, and high-temperature alloys there has to be a limit on the number of flutes. The rule of thumb is for every millimeter in diameter of a tool you get one flute, he said. For example, for tools with a ½" (12.7-mm) diameter, the maximum flute number to be effective is 12 and for tools with a 1" (25.4-mm) diameter the maximum flute number to be effective is 25. “For practicality that’s a good way to do it,” Clynch said.
Connect With Us