Probing machining options beyond drilling
By Jim Lorincz
Drilling, most everyone agrees, is still the most widely employed method of making holes, in large numbers, in materials of all types. Of course, for each given hole size, a drill with a diam within a few thousandths of an inch of the hole diam is required, meaning that a significant number of drills must be available out in the shop to produce different-size holes.
As hole diam gets larger, something greater than 1½" (38.1-mm), the power and stability of the machine required to produce the hole become much more important. An additional consideration arises if the holes are being made in high-production lot sizes, or if just a few holes are required. Again, machine capability and availability of the right tooling in the shop are the key considerations.
"Indexable drills are pretty economical and efficient in drilling even to 1¾" [44.45-mm] diam," says Patrick Nehls, product manager, Walter-USA Inc. (Waukesha, WI). "Above that size, we see fewer indexable drills used, and there are fewer holes being drilled."
In determining which holemaking strategy to adopt, Sandvik Coromant (Fair Lawn, NJ) suggests five considerations:
- Hole diam, depth, tolerance, surface finish, and configuration,
- Configuration of the component including stability, overhang, rotation for fixturing,
- Machine power, rpm, coolant-through availability, stability,
- Batch size, 10 holes or 1 million,
- Machining cost.
Once hole diam and depth are determined, answers to the remaining questions about machine capability and tools available to do the job are to be found on the shop floor and in tool cribs and machine ATCs, and in the product offerings of tooling manufacturers.
Trepanning larger holes from 3 to 6" (76.2–152.4-mm) diam, for example, gundrilling deep holes, and boring are not included within the scope of this article. Hole depths to 5xD are generally assumed, unless otherwise stated.
Upper size-of-hole limits for drilling depend on machine power and stability to push drills through the material. "There are general limits for drilling, which are dependent on machine capability, based on size of machine, power, setup, feed force, and torque," explains Bruce Carter, manager rotating products, Sandvik Coromant. "In considering the machine's power, for example, it's important to consider where in the range the full horsepower and torque are delivered."
For larger diam holes and cavities, developments in tooling, machine technology, and readily available canned programming routines are making helical interpolation milling (a.k.a. corkscrew milling), circular interpolation milling, and plunge milling (a.k.a. Z-axis milling) effective choices for manufacturers where drilling may not be the better option.
- Helical interpolation milling involves using a milling cutter to open the hole by ramping into a solid or an existing hole, and then spiraling down in the Z-axis simultaneously with an X/Y circular motion.
- Circular interpolation milling involves walking around an OD or ID at the full depth of the cutter to open an existing hole.
- Plunge milling, or Z-axis milling, can create a new hole (drilling) as well as rough out a cavity by successive plunge cuts along a shoulder.
"Helical and circular interpolation milling enable the manufacturer to generate large holes with a machine of limited horsepower, say 10 hp [7.5 kW] or even 15 hp [11.2 kW] that is not able to push either a spade or indexable drill through to make the hole," explains Konrad Forman, product manager, Ingersoll Cutting Tools (Rockford, IL).
"To drill a larger hole, traditionally users would start with a smaller diam drill and go up successively with larger size drills to enlarge the hole," Forman says. "That involves purchasing the required tooling, and the extra time required to change drills. Using one tool and a helical ramping move, the user can start with solid material, and corkscrew mill simultaneously in three axes to generate the required hole size," Forman explains.
Forman says that when properly applied, high-performance milling tools can produce roundness within 0.0005" (0.013 mm) with an excellent finish.
Helical interpolation can be accomplished with many different types of standard milling cutters, including shoulder milling cutters, round button cutters, high-feed milling cutters, and helical milling cutters, among others.
Most modern machine tools have a canned cycle for helical interpolation. In three-axis machines, the canned cycle makes for quick programming of the three X,Y,Z axes. In addition, CAM software programs include even more sophisticated algorithms necessary for interpolating.
"Unless they are running an older CAM package or an antiquated system, users can readily find the functionality to create a helical toolpath or a circular toolpath," says William Fiorenza, product manager, Ingersoll Cutting Tools. "In the tool and die area, about 60% are doing programming offline with a dedicated programmer who creates the most efficient toolpath possible. The other 40% of the programming is done by very skilled machinists," Fiorenza says.
In helical and circular interpolation, the cutting length of the insert and the tolerance that the end user is attempting to maintain are key considerations, says Michael Gadzinski, national training manager, Iscar Metals Inc. (Arlington, TX).
"Solid carbide end mills can be used, but normally only for very short depths because clamping can limit the potential depth of interpolation. Normally this is done with some indexable carbide end mill or face mill to get a better surface finish and a cleaner and straighter sidewall," Gadzinski says.
Plunge milling has been around a long time and is becoming more popular. "One reason for its popularity is that machine tools and conversational programming allow the end user to do the stepovers for plunging more easily without having to manually program the entire G-code," Gadzinski explains. Tool manufacturers have begun concentrating more recently on designing tools with the capability to optimize plunging.
In the mold and die industry, plunge milling is being accepted as an effective way to rough out cavities. "They find they can reduce cycle time plunging and roughing parts out rather than doing more normal linear machining," Gadzinski says. Scallops that remain after plunging can be removed with helical milling or conventional semifinishing and finish-machining techniques.
Helical interpolation is a highly effective method of machining out a hole and is becoming more and more widely applied. It requires that the tool has some ramping capability. The downward helical cutting action as it is ramping down in the Z axis results in reduced side pressure on the tool when compared with circular interpolation, where the full radial engagement of the tool is subjected to all of the cutting forces.
"Circular interpolation is effective when there is an existing hole and you want to enlarge it to a certain depth, whether it's a through hole or blind hole," explains Jim Minock, product manager, Seco Carboloy (Warren, MI). "The tool is inserted into the hole to the depth of the tool and then you mill around the hole in a complete circle. If you need to go deeper, you drop down lower and repeat the process until you are all the way through the part."
Possible machining strategies are limited only by the imagination and skill of programmers and machinists. For an application that required a 12" (304.8-mm) diam through-hole in a block of 4140 material 28" (711.2-mm) thick, Seco-Carboloy was able to reduce machining time for a customer by more than 2 hr by changing from a spade-drilling/plunge-milling process to helical interpolation ramping.
Originally the customer first used an 8" (203.2-mm) indexable spade drill to drill 14" (355.6-mm) deep, and then used a 6" (152.4-mm) diam plunge mill to increase the bore size to 12" (304.8 mm). The part was rotated and the process was repeated on the opposite side to create a through hole. Seco-Carboloy's better idea was to apply a 6.6" (167.6-mm) diam high-feed cassette cutter to the application using helical interpolation ramping. The customer was able to rough-machine the bore in 20 min or 40 min for the complete bore using the high-feed cassette cutter, compared with 85.2 min per side, as compared to a total of 170.4 min for the previous technique.
There is nothing preventing a helical interpolation move from being combined with a ramping or facing move for profiling. Walter-USA's Nehls explains: "When you look at ramping or helical interpolation, or ramping and face-milling a profile part, it's pretty much the same thing. With helical interpolation, it's pretty clear that you are just making a round hole and progressing down through the part in a helical fashion. There's nothing stopping you from taking that helical movement and turning it into a straight ramping operation, going across the part for profiling instead of into the part."
In some applications, creative machining techniques can point to the application of newer styles of multifunctional drilling-type tools. Ingersoll's Forman describes how taking a traditional approach to opening a 7" deep pocket that is 4" (101.6-mm) wide and 11" (279.4-mm) long in 6Al 4V titanium with a 50-taper, 50-hp (37.3-kW) machine can be done faster by plunging with a Quad drill.
"The traditional way of opening the cavity is to ramp in with a 3½" (88.9-mm) diam drill for the access hole, walk around with a 2½"(63.5-mm) face mill, one in a stubby holder and one in a more extended holder when you run out of room. At the bottom there's a 1" (25.4-mm) radius, so a long-reach ballnose tool is used.
"Because our Quad drill can plunge, another method is to take a 3¼" (82.55-mm) Quad drill, plunge down as far as you can without violating the bottom radius, and take the drill with 50–75% stepovers and walk across and make a channel, throwing the titanium chips out more efficiently and without creating any webbing. Scallops are easily handled with the same endmill by walking around the side wall and finishing up with a ballnose end mill," he concludes.
Turbo indexable square shoulder end mills from Seco-Carboloy (Warren, MI) can be used for both helical interpolation and circular milling. High Feed cutters use an unusual insert shape and process to effectively thin the chip at low DOC, but move at very fast feed rates for high metal removal rates. The round cutters are primarily used for copy-milling applications, but they too are configured to ramp down and interpolate in corkscrew milling. Plunge milling can be accomplished with the same tools as those used in helical interpolation.
CoroDrill 880 from Sandvik Coromant (Fair Lawn, NJ) features four cutting edges and wiper geometry for applications including helical interpolation, plunge drilling, and boring. Versions are being introduced covering diam from 0.473 to 2.5" (12.7–63.5 mm) with lengths ranging from 2 to 5 times diam. CoroMill 210 is available with diam to 4.0" (99.06 mm) for plunge milling and high-feed face milling. Plunge milling with the CoroMill 210 removes large volumes of metal in the axial direction, such as when milling deep cavities or externally along deep shoulders.
Xtra-tec F4042 shoulder-milling cutters from Walter-USA Inc. (Waukesha, WI) provide a good surface finish with a 90° shoulder with each orbit of the tool. The F2330 High Feed Mill has a three-sided trochoid insert. The F2334 Round Button insert cutter features a back that is actually square or hexagonal so top clamps aren't needed for anti-rotation and four, six, and eight cutting edges are possible. The F2280 Octagon cutter yields four cutting edges when helical interpolating, using two adjacent corners of the insert.
Heliplus milling cutters from Iscar Metals Inc. (Arlington, TX) with extended 22-mm cutting edge are used for very steep helical interpolation and penetration into deep cavities, as well as circular interpolation. For plunging, the Plungemill and the Feedmill are used in applications such as mold and die and applications, where there are large overhangs and a lot of stock to be removed.
Quad Drills from Ingersoll Cutting Tools (Rockford, IL) in 0.625–3.25" (15.9–82.6-mm) diam range feature heavy-duty square inserts for plunging. S-MAX Plunging Cutters are available from 2 to 4" (50.8– 101.6-mm) diam and feature aggressive 0.600" (15.24-mm) stepovers. ChipSurfer solid carbide drill-mill plunging tips in 0.375–0.625" (9.53–15.88-mm) diam for wide range of materials including stainless and high-temp alloys. The Punch-In-Quad high-positive plunging cutter features quad inserts in 0.75–4.00" (19.05–101.6-mm) diam range.
The Mill1 Max line of tooling from Kennametal Inc. (Latrobe, PA) is engineered for high-speed, high-feed machining of aerospace aluminum alloys. Mill1 Max is available with a complete line of corner radius choices from 0.8 through 6.4 mm, together with end mills, shell mills, and integral shank (monoblock) toolholders. The KSOM Mini face-milling tool features a range of cutters and inserts with a 25° clearance angle and eight cutting edges on the inserts for face milling, ramping, helical ramping from solid, slotting, and plunging.
This article was first published in the September 2006 edition of Manufacturing Engineering magazine.