Drill And Bore With A Face Mill

Making holes in metal is probably the most common operation in any machine shop. Specialized drilling and boring tools do a fine job making accurate holes.

Increasingly though, shops are successfully using interpolated milling cutters to drill and bore blind and through-holes. Usually this operation is performed with end mills.

Because of the improvements in machine tool design, CNC and servo response, and especially in the design and manufacture of freer-cutting tool geometries, some face mills are now capable of pulling double-duty. They can handle linear milling of planar surfaces and helical milling of holes.

To find out when and why a shop might consider interpolation of a face milling cutter over traditional end mills, drills and boring tools to cut holes, we talked to Jeff Fox, training and applications manager for Widia North America, a cutting tool maker; and Jim Turner, senior application engineer at Widia's parent, Milacron. They are using circular and helical interpolation of face milling cutters to produce holes that are close to boring bar quality in roundness, size and finish.

What Is Interpolation?

Interpolation of machine tools, which is the movement of multiple axes at the same time, has been around for a while. On most CNC machine tools, interpolation is transparent to the machine operator and programmer.

An interpolator—actually a small computer within the CNC—does the complex mathematical calculations based on a few descriptive inputs. Once the interpolator knows how big and how deep to make a circle, the operator doesn't have to think about it.

Circular interpolation involves simultaneous motion of two of the three axes on a standard three-axis machining center. The cutting tool is fed to a programmed depth of cut, often by plunging. Interpolation is then performed by combination moves in the X and Y axes.

Helical interpolation employs all three axes simultaneously. As the X and Y axes interpolate a circle, the Z axis is fed down in a spiral motion until it reaches the programmed depth.

Why Not Drill, Bore And Ream?

In general, there are two methods of generating a hole: milling and drilling. To clarify our terms, let's agree that milling a circle involves a cutter rotating on its own axis in conjunction with an orbiting workpiece motion.

Drilling uses a fixed diameter tool, rotating on its own axis, and plunging uni-directionally (Z-axis feed) into a stationary workpiece. Making a very accurate hole—meaning good size, roundness, depth and finish—has traditionally been at least a two-step process and sometimes has required several more steps.

First, the hole is drilled. Sometimes, when drilling from a solid, a pilot drill is used to make a place for the drill to start. As a drill advances through a workpiece, it encounters vagaries in the material. These can be material inconsistencies such as inclusions or hard spots. The drill will tend to deflect or wander off course slightly when encountering one of these "bumps in the road." In some applications, "a drill can wander as much as 0.008 to 0.015 inch," says Mr. Fox.

To straighten the wandering drill path, a boring bar is used. It can be set to the exact diameter initially or gradually brought to size with incremental passes. After employing a boring bar, hole size should be at spec. To meet very tight surface finish specs, a reaming tool is used to smooth the bore and bring size to finish diameter.

Proponents of interpolation use the process to eliminate some of the steps in hole drilling. For shops faced with increasingly demanding production and shipping schedules, knocking off a few steps in the production process, especially in a pervasive operation such as drilling, can have significant impact on throughput and profitability.

"Trying to simplify the manufacturing process is a key driver behind using interpolation of a face milling cutter," says Mr. Fox. "If you can eliminate a pilot drilling sequence, or a boring sequence, or drill several different size holes with one cutter, you've saved cutting time. That's good. Moreover though, you've eliminated the attendant non-cutting time [such as tool change, tool setting and balance, loading and transport] for those other tools."

What Does It Take?

"The key to using interpolation is smooth transition around the workpiece without having to do position updates every half-degree and leave marks on the work," says Mr. Fox. "Today, much of that is done in software. Most newer CNC machine tools are capable of running an interpolation macro. Differences between controls generally play out in how fast the X and Y axes can create an orbit."

One software technique used to perform circular interpolation is called looping. Basically a software macro does the math that results in a tool orbit of a programmed diameter.

Feed in the Z axis is set incrementally. In each orbit, the tool notches down in the Z axis by a prescribed amount. The interpolation, or combination X-axis and Y-axis moves, is "looped."

"We run the same circle over and over and move down in Z axis one increment for each orbit, until the milling cutter reaches programmed depth," says Mr. Fox. "This gives us the smooth orbit, without pause, needed to drill and bore using a face milling cutter."

Using this incremental Z-axis feed significantly reduces the amount of data blocks needed to execute a programmed interpolation. According to Mr. Turner, "if I have a counterbore that is to be two inches deep, I start at one point and tell the control to make a circle and return to my start point. I then tell the control to move two inches in the Z axis from where I'm starting. However, if my insert is capable of a quarter-inch depth of cut, I need to tell the control for each circular revolution or orbit to change my depth of cut by a quarter inch. Eight revolutions are needed to make the hole, but those eight revolutions are made from a single block of code."

The calculations needed to divide the two-inch depth of cut command to accommodate the quarter-inch feed requirement are in the interpolation macro. The macro "does the math" needed to get the cutter to the programmed depth—using a single go-to command.

"It used to be that if you had a machine capable of helical interpolation, you had to program eight orbits of the cutter with a quarter-inch depth of cut change for each pass," says Mr. Turner. "That was eight blocks of code in order to make one circle. It's much easier to program milled holes today with the interpolation macros built into the CNC. The same hole that used to need eight blocks of code now needs only one."

In addition to software, good hardware is needed for interpolating holes. A machine tool with a very true spindle and a good set of ballscrews is also important for interpolation because of axis reversals that occur in the X and Z axes when a circle is generated.

Face Mill And Drill

Metalcutting shops are continuously searching for ways to consolidate operations. Five-sided fixturing, gang tooling, turn-mill and mill-turn, are examples of ways to reduce multiple handling of workpieces.

Shops are also demanding that cutting tool makers try to find ways that allow more operations to be performed by a given cutter. Widia and several other cutting tool manufacturers have developed single cutting tools, with insert geometry and chip breakers, that can perform with one tool what once took multiple tools.

"Until recently," says Mr. Turner, "there simply wasn't a single tool available with the chipbreaker geometry that could effectively pull double-duty performing both face mill and end mill work. These new cutters enable us to use one tool for plunging and the same tool for sidecutting." Depending on the insert shape, chamfering can also be done with the same insert.

The advantage of one tool doing the work of three is obvious for shops strapped for tool pockets in their machining centers. It's also advantageous to use one tool for a range of hole sizes. Milacron has successfully processed work-pieces requiring face milling, chamfering, the rough and finish boring of six- and eight-inch holes, all with just one cutter.

What's Happening In The Cut?

Once the rpm is established in the conventional drilling operation, the Z-axis feed rate is the primary variable that needs to be considered. Interpolation on the other hand is a more complex set of variables.

There are, for example, two feed rates that need to be understood. "Feed rate one," says Mr. Fox, "is how deep, in Z-axis, the tool is fed per revolution or orbit of the hole. Feed rate two is how fast the cutter is moving through the material in the X/Y plane."

What's making it possible to use a face mill for plunge and side cutting is insert geometry that is designed as positive axially and positive radially. What's not obvious to the observer of an interpolated milling cut hole is that most of the cutting is done on the face. Chip loads on the side are relatively low.

Mr. Turner says he could use an end mill, drop down to a Z value, run around the circle and repeat that until he gets to depth, which is the conventional hole milling technique. Using the face mill, the depth of feed cannot exceed the height of the insert, and therefore, most of the cutting is done on the face of the cutter. Moreover, metal removal is higher because of the size of the cutter and the number of teeth.

The size of a face mill is also an advantage. Using a cutter close to the size of the hole diameter reduces the size of orbit needed to get around the hole circumference, which also reduces side loading.

"Instead of using a two-inch end mill to go in and cut a six-and-a-half-inch diameter hole such as in a pocketing routine," says Mr. Turner, "we can plunge in with a six-inch cutter. We made a six-and-a-half-inch hole but side cut only a half-inch circle.

"You wouldn't do that cut with a six-inch end mill," Mr. Turner continues. "We're trying to use tools that would be in the chain for other operations and extend their usefulness to drilling, which is why the face mill works."

Cored Holes And Solids

Ideally, milling interpolation for drilling and boring holes is best applied in holes above six inches. "It's still more economical to cut with a drill and boring bar below that," says Mr. Fox.

When interpolating a face milling cutter for large holes cut from solid, it may be advantageous to use a drill as a pilot hole. "Chip evacuation is the main reason for drilling a pilot," says Mr. Turner. "These milling cutters don't have flutes to help auger the chips out of the cut. A drilled hole, using the biggest standard drill in the shop will provide sufficient room for chip relief."

It's in cored holes that interpolation with a milling cutter is very efficient. With blind or through-holes, the milling cutter needs only to be a minimum of half the hole diameter to effectively interpolate a hole. At less than half the hole diameter, the orbiting cutter would leave material in the center of the hole.

On the other end of the scale, orbiting a six-inch cutter to make a six-and-a-half-inch hole can be done. That same six-inch mill can then cut an eight-, ten- or twelve-inch hole if needed.

On blind holes, Mr. Turner cautions that chip evacuation can be a concern with a milling cutter that is very close to the hole diameter. High pressure coolant is helpful in evacuating chips as is a horizontal spindle orientation on the machining center. Vertical machining centers benefit from interpolating a face mill for hole making if the hole depth is not too excessive for chip clearance.

How Good Is It?

Drilling and boring with a face mill really extends the usefulness of a single tool. In many operations, milling a surface and then cutting out a large cored bore is ideally suited to interpolation with a face mill.

"In applying this technique," says Mr. Turner, "we were hoping to eliminate rough boring bars. It's still a milling operation, so there will be some milling pattern marks in the bore. If feeds are slowed, a reasonable semi-finish cut quality can be produced with this technique. However, we've found that for tolerances tighter than 0.002 inches and surface finish specs better than about 125 Ra, you'll probably still need to use a finish boring bar for good results."

A bored finish is created by cutting a continuous spiral chip. Many shops require production of this kind of surface to satisfy a boring tolerance spec. Milling makes very small chips and the surface is serrated or cross-hatched. "To get the boring bar look, you need to use a boring bar," says Mr. Turner.

Consider Milling Holes

Few metalworking processes can be eliminated completely. There is always a need to drill and bore holes. What Widia and Milacron are trying to accomplish by using interpolation to drill with a face milling cutter is to reduce some of a shop's tool inventory and its associated costs for purchase and setup.

"In cellular manufacturing, a shop will often try to use redundant tooling to keep running," says Mr. Turner. "Tool pockets can be a premium especially if every workpiece hole needs multiple tools to rough out the bore. One cutter that can do the rough boring work of several tools and face mill is very helpful here."

For high mix, low volume operations, interpolation can save a shop significant direct and indirect machining time. Throughput calls the tune for these businesses. Reducing the need for setting rough boring bars can enable a shop to really shave precious time off increasingly shorter lead times.

"Using milling cutters for drilling and boring means a shop doesn't need to stock a large selection of boring bars," says Mr. Turner. "A job shop can carry a four-, six- and eight-inch face milling cutter that can be used on any job. For a workpiece that has a four-and-a-half-inch bore and another part with a five-inch bore, one boring bar might not have the range for both jobs, while a four-inch face mill could do them both."

Manufacturing today is about choices. Shops have many tools at their disposal to get the job done. Applying a face mill to drilling and boring operations is another opportunity to incrementally increase the efficiency and profitability of machining appropriate workpieces.