Get a Fine Finish for All Your Holes
"Modern drill geometries can yield 20- to 60-microinch root mean square (rms) or 40- to 120-micron Ra finishes in one pass," said Tony Yakamavich, senior product specialist of drilling at Sandvik Coromant Co. (Fair Lawn, NJ), a manufacturer of cutting tools.
The drill bit geometry has a number of features that help the drill create smooth surfaces. For example, drill bits with a smaller chisel and thinner web can be more accurate than old 118-degree drill points. "An old tool tended to move from side to side as it was drilling because the chisel pushed the material rather than cutting it," said Yakamavich. "The modern geometry, however, cuts that center portion, shearing the chip. It's a freer-cutting tool, which creates a better sur-face finish."
The thinner web at the point allows the drill to bite in right away and cut along the centerline from the start of the drilling process. "When a conventional tool touches the part, it walks a little before it starts drilling," said Ryan Schwane, product engineer at Guhring Inc. (Brookfield, WI), another company that makes cutting tools. "Because the point doesn't get off to a good start, the tool tries to return to the center while it's drilling. This movement often causes a poor surface finish and creates extra heat, which encourages the work material to weld to the cutting edge and scrape the walls."
Straight flutes and double margins are other design features that can enhance surface finish. Straight flutes minimize the spring effect common in drills with helical flutes, and the double margin aids centering. Because both features work together in Guhring's RT 150 GG drill to keep the point from "wiggling" in the hole, the drill produces reamer-class surfaces and burnished-quality finishes in short-chipping materials, even in holes that are 10 Arial the diameter.
Although these tools are more expensive than conventional drills, using them isn't always more expensive. They can boost productivity in the average shop by 30%, and in many applications can replace the reamer and the center or starting drill, said Yakamavich. "Tool cost is an extremely low contributor to overall cost, but machine time is a high dollar item," he said. Reducing machine time by combining three operations -- center drilling, drilling and reaming -- can more than pay for the extra cost of the drill.
For this reason, manufacturers can reduce the cost of making quality holes and, indeed, make them free by suggesting these advanced drills to manufacturing departments that are challenged to achieve good surface finish. If manufacturing is already using them, yet finish problems develop, quality control can shorten the troubleshooting process by offering more feedback than simply informing the machinist that the surface finish is not within specification. Inspectors can look for various telltale signs to help manufacturing solve the problem.
Based on the signs an out-of-control drilling process leaves behind, quality control can create a rudimentary design of experiments to expedite the search for a solution. Although the drill's geometry affects surface finish dramatically, Yakamavich said it can be ignored if manufacturing is using the advanced drills recommended by cutting tool manufacturers for the work material and hole size at hand. "You know that the geometry is correct because we have learned what finishes to expect for each work material over the years," he said.
Wear, a diagnostics tool
Assuming that the tool is the correct one for the job, the first item to check when a finish goes bad is tool wear. In general, wear along the cutting edges of the tool degrades surface finish because it alters the geometry. Advanced drills have as positive a rake and as great a clearance as possible for the given work material to enhance the shearing action that creates smooth finishes. As the edge wears, however, the geometry becomes less positive, leaves a rougher surface, and eventually smears the surface. Positive rake is always a welcome geometry in drilling, said Yakamavich.
A study of the wear pattern on the tool can give the troubleshooter a new set of clues for identifying the problem. Worn peripheral corners can explain a slightly undersized hole with rifling or scarring along the walls. "As the peripheral corners of the drill wear, they not only affect the surface finish [on the way in] but also make the hole's diameter slightly smaller," said Yakamavich. "Therefore, as the drill retracts from the work, the margins can scrape the wall surface."
When rubbing marks along the cylindrical land of the tool occur simultaneously with rifling, helical patterns or uneven wear in a hole that might be slightly oversized, the culprit is usually a lack of concentricity. "You'd probably see alternating scarred and compressed areas because the drill would be digging and pushing against the wall, creating many stresses as it wiggles around," said Schwane. "So some of the cylindrical land would then press on the material while the point would be digging into the work."
The tool moves off center for a variety of reasons. One is the tool's walking around the center slightly when it encounters a high cutting force from too fast of a feed rate or not enough relief on the tool. The advice for manufacturing here is to try slowing the feed or modifying the tool geometry. For example, drills made for hard materials have shallow point angles, as great as 150 degrees, and can create a rifling effect, or spiral mark, along the wall. Thinning the web is the best place to start correcting the problem, because thinner webs encourage the tool to bite into the work.
"Another way to combat walking in this case, would be to add a chamfer along the outside corners to lead the tool into the cut, much like the lead-in angle does on a reamer," said Schwane. "To take it a step further, put a radius on the corner of the tool for a slow transition to the diameter. Material isn't being removed in as big of bites on the outside, and the cutting edge is actually lengthened quite a bit and spreads out the cutting forces on the corner."
Other reasons for the tool to deviate from centerline is misalignment or lack of rigidity in the workpiece, machine tool or both. The result is uneven wear or vibration. "If the workpiece is loose or the spindle is weak, vibration will occur and create a pattern on the wall," said Yakamavich. "Machinists often can hear a little singing and feel the vibration. They'll usually see catastrophic failure before surface finish deviations develop, though. If the material moves or the spindle is not rigid, the drill is going to break."
Because of the new drills, higher speeds and feeds, and the rising trend to complete a job in one setup, rigidity is more of a factor now than it used to be, especially for carbide tooling. "Before, we used to be concerned with axial thrust," said Harold Bartsch, manufacturing engineer at SPX Power Team (Owatonna, MN), a company specializing in workholders. "Now we have to hold and support the part in three dimensions to counteract radial forces. Drilling is no longer just a simple operation that you put it in a drill press and poke a hole."
For this reason, the company both uses and sells wedge clamps actuated by cartridge-style hydraulic cylinders. Rather than pinching the work, this clamping scheme wedges the work to offer greater support. In the Power Team's shop, so-called tombstone fixtures hold as many as 20 of these cylinders at a time. "It lets us clamp on the edge of a part and expose as many sides as possible so that we can machine the top face off, mill it, drill it and index around to the sides," said Bartsch.
Vibration also can come from the tool itself, perhaps a loose insert in a pocket or a large radius causing excessive high side forces. Another source of tool vibration in deep holes is changing harmonics. Each diameter-to-length ratio vibrates differently, and the difference can be significant when the holes are deep. "Therefore, it is extremely difficult to make one tool to eliminate the vibration at each ratio," said Yakamavich. "In those cases, adjust the feed rate in the cut to compensate for the length of the tool and depth. In some cases, reducing the feed rate by 10% eliminates the vibration."
Curing the blues
If poor surface finish is not discernible through tool wear and surface patterns, the second item to check is excessive heat. Discoloration of the chips, hole and tool can help pinpoint the cause of poor surface finish. When a drilling process is under control, the chips should be silver. The exception is a process using straight oil as the cutting fluid. In this case, the chips can appear to be brown.
When overheating becomes a problem, the chips and inner surfaces of the hole turn blue. On high-speed steel (HSS) drills, the bluish tint can appear along the cutting edges. Because tungsten carbide behaves differently than steel at high temperatures, the cutting edges made from carbide turn a whitish-gray color, burnt brown or black when they get too hot. Overheating also will cause welding of chips to the cutting edge, often called "built-up edge," on both carbide and HSS tools and chipping at the outside corners of the cutting edges on carbide tools.
Overheating is one cause of wear. Another common one is an inadequate application of cutting fluid. Unlike milling and turning, drilling is a process that always demands a generous amount of cutting fluid. Not only is the tool engaged in the cut continuously, as it is in turning, but it also is buried deep in the work and remains in contact with the hot chips longer. Cutting fluids, therefore, are necessary to cool the cutting zone, lubricate the cutting action to prevent welding and flush the chips from the hole.
Because cooling is the most important function of the cutting fluid in drilling, most fluids specified for this operation are water based. Water's high heat capacity makes it a superior coolant, and most water-based formulations contain the necessary lubricating agents. Even so, lubricity is more important to create fine surface finishes in drilling than in general-purpose milling and turning. Consequently, Schwane recommends a mixture richer than the 5% to 6% concentrate typical for general-purpose machining. "If you are concerned about surface finish, concentration should be at 8% to 12%," he said.
Because cutting fluid is important for good finishes, drilling specialists at cutting tool manufacturers recommend drills that deliver coolant through the tool to the cutting zone. "Unlike the past, there are different ways to provide coolant through the tip of the tool to keep the tool and cutting zone cool, even under extreme conditions for the high penetration and fast cutting drills," said Schwane. These tools deliver fluid at the high volume and pressure necessary to absorb the heat and flush the hot chips from the hole.
Yakamavich agrees that holding tight finish tolerances requires machines with coolant-through spindles that can exploit these tools. "Machines without coolant-through spindles must rely on flood cooling," he said. "It is extremely difficult to get good finishes otherwise because the coolant very seldom gets to the cutting edge. It's always diverted by the chips trying to exit the hole. Delivering coolant through the spindle is very important for cooling the cutting zone, lubricating the cutting edge and removing the chips."
Mind the speed limits
Other causes of overheating are feeding parts too fast and dull tools. Feeding too aggressively is easy to do as manufacturing tries to duplicate the fantastic feed rates demonstrated by machine tool builders at a trade show. Not all materials will permit feeding at 40 to 70 ipm. "In steel and stainless steel, it's a much different story," said Yakamavich. "Some drills, with parabolic flutes and special edges, can exceed conventional feed rates but only in certain materials."
The reason for poor surface finish at excessive feed rates, or with dull tools, is that the tool is pushing the material not shearing it. "Finishes will be as rough as 120 to 125 microinches rms," said Yakamavich. "In the case of excessive feed rates, the feed increments are so fast that the edges don't have a chance to cut all that material and the margins push or burnish the hole."
Extreme feed rates, as well as incorrect tool geometry, can cause chips to pack in the flute. Because debris accumulates at the cutting edge, heat builds there and causes the peripheral corners of the tool to fail. The combination of the dull tool, excess heat and packed chips gouges the wall and welds bits of chips to it. Eventually, catastrophic tool failure occurs.
The correct tool geometry and cutting speeds and feeds should control chip formation and prevent chips from binding in the flutes. The optimum chip is silver and has the shape of a "6" or a "9." If they are that shape, yet packing and binding are a problem, check the volume and pressure of the cutting fluid. They must be high enough to flush the chips from the hole.
Although textbook chips are 6s and 9s, soft, gummy materials are known to produce long, stringy chips that are impractical to break. "Fortunately, the flutes [in drills with the correct geometry] are designed to pass those chips, getting them away from the cutting edge and out of the hole," said Yakamavich. "So we're not too concerned about long, stringy chips, unless they are irregular and rough." Roughness indicates inadequate lubricity in the cutting fluid, and any binding requires adjusting the cutting parameters or trying a different drill with a more positive geometry or with parabolic flutes.
Choosing the right drill, running it at the correct speeds and feeds, and supporting it correctly with fluids, solid workholding and a good machine will produce optimum chips -- an excellent sign that the operation is giving the best finish possible.