How To Machine Aircraft Titanium

Choose cutters, depths and tool paths with attention to particular steps in the process, and you can machine titanium more efficiently than you might suspect. Boeing offers practical tips.

New aircraft designs that make more extensive use of composite materials make more extensive use of titanium at the same time. Compared to aluminum, titanium is more compatible with composites in aircraft assemblies. As a result, the Boeing 787 Dreamliner, which is 50 percent composite materials by weight, is also 15 percent titanium by weight. That is significantly more titanium than the previous (heavier) Boeing 777.

Click images to enlarge This photo of titanium machining was taken at Boeing St. Louis. Here is a workpiece representative of the typical titanium aircraft part. A titanium structural component for an aircraft such as the 787 is a large workpiece consisting of many pockets like this one.

Obtaining enough titanium to meet the needs of this latest generation of aircraft has been a challenge. Titanium prices have risen in response to the demand, and new capacity for producing titanium alloys is coming online. Still unaddressed, however, is the question of machining all that titanium. While no one can say for sure, it seems unlikely that there is currently enough titanium machining capacity to meet all the needs of the various high-titanium-content planes being introduced to the market. One way or another, the aircraft-industry supply chain will have to realize more of this capacity. Shops will be asked to machine more titanium than ever before, and also to machine it faster.

One of the leading organizations in the study of just how to do this is the Boeing Research and Technology group (BR&T) based in St. Louis. Boeing researchers here develop techniques for more effective titanium machining—techniques that they convey to Boeing’s suppliers.

The archetypical titanium part is shown at right (the photo of the part held in a hand). The machining of aircraft structures made of titanium, like those made of aluminum, is fundamentally an exercise in machining pockets. Aircraft parts, with their webs and ribs, are made of many pockets. The pockets are particularly deep on the 787, because some deep-pocket aluminum parts have been replaced with titanium. Therefore, the pocket machining challenges are that much greater.

In aluminum, machining any particular pocket such as the one shown might not involve separate roughing and finishing operations. Titanium is different. Aircraft-industry manufacturers have learned to precisely cut aluminum at relatively consistent radial depths that allow even a heavy depth of cut to complete a wall or rib. But in titanium, the slow cutting speed means that roughing and finishing are still needed in order to remove the volume of material productively. As a result, machining a titanium part effectively involves a series of discrete operations, with different proven techniques at each step.

Those techniques are outlined in the collection of articles in the links under “Editor Picks” at right. The information comes from BR&T (or, in the case of one of the articles, from a major cutting tool supplier). As the articles describe, machining titanium aircraft parts productively does not necessarily demand a new machine tool or even any particular style of machine.

It also does not require great cost. The final article at right makes this clear. Any of the techniques in the articles below might be applied separately, but together, they produce a radically different titanium milling process that is likely to save not only time, but also considerable expense.

The 8-To-1 Rule For Finishing Walls And Ribs

Here is the most fundamental tool for milling titanium productively: an end mill with lots of flutes.

Click images to enlarge Compared to a 10- or 20-flute tool, the experimental 45-flute tool removes material even faster. The 10-flute carbide end mill is a fundamental tool for achieving high metal removal rates when finishing titanium ribs. These two ribs were used to test the effectiveness of the 8:1 rule. Any deflection during milling of the thick rib could be assumed to be deflection of the tool alone. When the thin rib was milled at the 8:1 depth, total deflection was even less than what was seen with the thick rib—confirming the stability of the cut. This chart compares the deflection for the two ribs seen in the previous photo. When pocket walls are milled in a single pass at full depth, cutting time is long and the thin wall is likely to vibrate. Machining in vertical steps using the 8:1 rule is a faster and more stable way to finish the pocket. The application of the 8:1 rule not only proceeds in vertical stages, but also alternates between roughing and finishing passes. The numbers here indicate the order in which the regions of material would be removed to finish this rib. Areas roughed at a large axial depth are followed by finishing passes taken at lighter axial depths. The rib remains supported by the uncut material and emerges from the stock as the areas are removed in this sequence.

Researchers with the Boeing Research and Technology group (BR&T) in St. Louis explain that one of the most fundamental guides for determining how to apply such a tool is something the group calls the "8-to-1 rule."

A tool with many flutes permits high metal removal rates during finishing. Titanium requires parts to be roughed and finished in separate steps. Aluminum aircraft parts are not like that. The speed and chip load at which aluminum can be milled permit high metal removal rates even when the tool is appropriate for finishing. But in titanium, the maximum practical cutting speed and chip load are much lower. Therefore, achieving a sufficient metal removal rate has to involve other strategies, such as taking a heavy depth of cut during roughing. During finishing, though—as a machined wall or rib becomes slender enough that cutting forces have to be reduced—a heavy depth of cut is no longer possible. What remains for productivity in finishing is to increase the feed rate. This can be done using a milling tool that has enough flutes to multiply the small chip load into a high value of inches per minute.

How many flutes? As many as you can use. Ten-flute end mills are available from various sources. A 1-inch-diameter, 10-flute tool running at 400 sfm and 0.003 inch per tooth produces a feed rate of 46 ipm. BR&T is routinely able to finish titanium at this speed and feed rate. The group also sometimes applies 20-flute end mills, and has experimented with a 45-flute tool (more on this below).

Again, these are tools for finishing. Their handicap is poor chip clearance resulting from the closely spaced flutes. To compensate, chip load generally has to be held to 0.003 inch per tooth, and the radial depth of cut for a 1-inch tool must not exceed 0.035 to 0.050 inch to leave ample room for chips to fall away.

As for the depth of cut in the axial direction, this is where the 8-to-1 rule comes in.

Because it defines the depth of cut according to how close the rib is to its final size, this rule essentially establishes the difference between roughing and finishing passes when milling pockets in titanium.

The Rule Defined

The 8-to-1 rule can be stated as follows: The maximum axial depth of cut should be no greater than 8 times the remaining thickness of a wall or rib adjacent to the cut.

For example, consider a pocket wall that must be machined to 0.050 inch thick. Roughing passes leave enough extra stock on the wall that it is still 1/8 inch thick after roughing. Because the wall is machined to this thickness, milling passes adjacent to it can be taken at a depth of up to 8 times this value, or 1 inch deep. (Boeing says 1 inch is also the maximum axial depth for the 400-sfm process cited above.)

Finishing passes along the wall then bring it to its final thickness of 0.050. These passes also can be no deeper than 8 times the machined thickness. In this case, this makes the maximum depth 0.40 inch.

Avoiding deflection is the reason for this ratio. Through experimentation, BR&T searched for a depth-of-cut guideline that could be applied uniformly across the range of wall and rib heights and thicknesses that Boeing components are likely to require. The photo of the two test specimens at right illustrates this experimentation. At 1/4 inch, the heavier of the two ribs is so thick that any deflection measured in the part could only have been the result of deflection of the tool. The sample thus provided a baseline for understanding the effect of tool deflection alone. In comparison, the 0.030-inch rib was machined using the 8-to-1 rule at an axial depth of 0.250 inch (call it 8.3-to-1). The deflection here could come from both the tool and part—but the graph shows the stability. For this rib, the overall deflection was actually less than the baseline deflection that could be expected from just the tool itself.

Titanium handles the 8:1 depth of cut because it is such a stiff material, say BR&T researchers. If the same rule were applied to aluminum, the ratio would be 4:1.

Finishing In Downward Steps

Limiting the depth of cut in this way means that deep pocket walls have to be finished with successive incremental passes. This is much different from the way pocket walls have typically been machined. Usually, the machining is done with a single finishing pass at the full depth of the pocket. This approach is sometimes seen to be not only more productive, but also conducive to a higher-quality pocket because it eliminates any feed lines between successive passes. Boeing believes both views are incorrect.

The single, full-depth pass generally requires a slow feed rate of 1 to 3 ipm. The corresponding metal removal rate is around 0.1 cubic inch per minute. By contrast, a 46-ipm pass in a series of 8-to-1 step-downs produces a metal removal rate of 2 cubic inches per minute. While this represents an increase of a factor of 20, it is only the beginning of the productivity improvement. An unsupported wall or rib typically vibrates during the full-depth pass, creating the need for repeated passes ("float" passes) to clean up the stock left uncut on the moving workpiece. For this reason, the vibration often results in poor thickness control, not to mention chatter marks that actually do have to be hand-blended away (unlike the generally harmless feed lines). The 8-to-1 process not only cuts the feature faster, but also avoids these additional steps.

But vibration is still a danger. To reduce vibration as the machined feature emerges from the stock, the successive passes should be taken from alternating sides of the wall or rib. Another illustration at right shows this. In fact, as the same illustration shows, the approach that maximizes support is to alternate between roughing and finishing all the way down. Completing the rib in this way means that the rib does not have to be touched again at each successive layer, as the tool descends to the next level of the pocket.

45 Flutes

To make the finishing passes even more productive, BR&T has been experimenting with how many flutes it is possible to cram into the cutter. The 45-flute tool shown is 2 inches in diameter. To allow the tool to be manufactured cost-effectively, it features a hollow core to reduce the amount of carbide required. At 400 sfm and 0.003 inch per tooth, this tool allows a feed rate greater than 100 ipm.

There are problems, though. The larger tool diameter increases runout error to the point of unacceptable variation in the chip load. The Boeing researchers are still experimenting with how to make this tool design practical enough to apply in production. For the time being, this tool represents the cutting edge—or 45 cutting edges—of how fast it is possible to finish-machine in titanium.

Getting The Metal Out

The [above section] about the 8-to-1 rule describes using end mills with many flutes to take fast finishing passes in titanium pockets. But what about roughing the titanium? If the component is machined from a solid block, then all of the rough stock has to be hogged from the pocket before the 8-to-1 technique can be applied.

Click images to enlarge Machining in circles, as illustrated by this drawing, keeps the load on the tool constant. Much of the cornering in this drawing is unnecessary. There is no need for tool paths to conform to the pocket’s shape until the tool actually reaches the walls. Material can be roughed out of the corner of a pocket by "slicing"—that is, by taking a series of successively shorter passes with a small-diameter tool. A relatively heavy amount of stock should be left on the floor of the pocket and machined away in a tool path that spirals out from the center. That way, the area of the floor being machined is always supported by uncut stock left alongside the cut.

Cutting tool supplier Sandvik Coromant has a research group devoted to aerospace machining. This group has worked to develop and evaluate techniques for efficiently machining titanium aerostructure components. Bruce Carter, aerospace projects manager with the company, says when it comes to roughing, there are essentially three options for hogging material out of a titanium pocket. They are: (1) drilling and profile milling, (2) ramping to incremental depths, and (3) drilling and plunge milling.

The first of these is generally the most productive choice, he says. The other two address the challenges of more difficult pockets.

Drill And Profile Mill

This approach begins with drilling a large-diameter starter hole in the pocket. For chip clearance, the drilled hole should be as large as possible, and at minimum, 1.3 or 1.4 times the diameter of the milling tool that will rough out the rest of the area. The rough milling cutter should then reach not quite as deep as the drilled hole—leaving about 0.20 inch of stock in place for finishing the floor later (more on this below). Starting in the drilled hole, the milling cutter proceeds outward to mill the pocket depth in one set of passes. Video animation under Editor Picks at [MMS Online] shows the best way for the milling cutter to enter the material from out of the hole.

This approach represents the most productive material-removal process for pockets in titanium, Mr. Carter says. However, it requires a relatively simple pocket shape that is free of any contour or features that would necessitate changing tools or machining successive layers in certain parts of the pocket. This approach also requires a stable process, meaning the pocket should be relatively shallow, and the tool overhang should be no greater than 4 times diameter. When the pocket is not shallow, or when the process lacks stiffness for other reasons, one of the other two options may be more effective.

Ramp And Interpolate

This approach does not require a drilled hole. It uses just one tool. This is a milling cutter that ramps into the material and interpolates to machine one layer of the pocket before ramping to the next layer. Depths of cut are light, which may make this technique best for less-rigid machines such as some 40-taper machine tools. The technique can be used with a high-feed mill, but a milling cutter with circular inserts can ramp more aggressively.

The approach can be much more effective than the previous technique for pockets that have varying depths resulting from a contoured shape.

Drill And Plunge

This technique is a problem solver, Mr. Carter says. Just like the first technique, this one begins with a drilled hole. However, from there, the machine essentially keeps on drilling—making overlapping plunges with a plunge-milling tool or a drill capable of machining this way. The Z axis is generally the stiffest axis of any machining center, so this technique can allow pockets to be machined in titanium even on machines with poor rigidity. It also offers an excellent way to machine deep pockets requiring tool overhangs of 4 times diameter or more.

Of course, one drawback of this machining technique is the cusps that are left between plunging passes all along the outline of the pocket. These have to be removed in a separate operation.

Corner Concerns

The first two techniques—drill and profile mill, and ramp and interpolate—share a common problem in the corners. Making a right-angle turn to machine an internal corner produces a dramatic increase in radial depth of cut. This can lead to excessive tool wear, tool breakage or unacceptable chatter marks in the corners—not to mention an unpredictable process that is difficult to leave unattended. Therefore, the solution Mr. Carter recommends is to have almost no corners at all. Specifically, instead of milling parallel to the walls of the pocket, he says to mill outward in circles until the walls of the pocket actually do have to be machined in straight lines.

A drawing at right illustrates this. The constant-arc tool paths allow the process to maximize both chip load and radial depth of cut because the load on the tool remains steady throughout this spiraling path. The feed rate may change to allow for more abrupt changes in the toolpath direction as the cutter reaches the wall—but even here, the tool should make large-diameter arcs that steer well clear of the internal corners.

How, then, should the remaining rough stock in the corners be removed? Mr. Carter suggests a technique that Sandvik Coromant calls "slicing"—which also could apply to the material left over in the corners after any of the three pocketing techniques described above.

Slicing

Slicing is a semi-finishing technique in which material is removed from corners via a series of increasingly shorter arcs to get down to a smaller corner radius. Another drawing at right illustrates this.

As the drawing shows, each arc permits a light radial depth of cut. The light pass can be taken at a relatively high feed rate. However, the radial depth increases as the tool gets closer to the corner, so the feed rate should decrease accordingly.

In the end, this leaves a corner radius that is slightly larger than the tool. This is not an approach to finishing corners; plunge and sweep is a technique for that (see the article [below]).

The slicing technique applies not only to right-angle corners, but also to corners that are much more acute. Acute corners simply require more slicing passes to sweep out the extra stock that the roughing left behind.

The Floor

The final important consideration for getting material out of the pocket is the floor, which (unlike the pocket’s walls) might be milled to its finish dimensions. However, finishing the floor involves more stock removal then many shops are used to considering as part of a finish pass.

Mr. Carter says leaving 0.20 to 0.25 inch on the floor of the pocket is good practice in milling a titanium aircraft component. This amount of stock helps support the thin floor against vibration as the material is machined away.

To ensure a stable cut, the floor of the pocket is machined to its finished depth in rings radiating out from the drilled hole. Thus, the cut always has unmachined stock next to it to provide support—all the way out to where the support comes from the adjacent walls, which themselves will later be finished, probably using the 8-to-1 rule described previously.

Plunge And Sweep For Finishing The Corners

Click images to enlarge This drawing illustrates the reason to remove material from corners prior to finishing pocket walls. If material is not removed from corners, radial depth of cut increases dramatically as the tool enters the corner. In addition to the effect on tool life, the surface finish of the part is likely to suffer. In the plunge-and-sweep technique, a land on the cutting edge is useful for plunging, but should not be used for sweeping. Thus, the technique could be done with land and no-land versions of this same tool (see next photo)....

A drawing at [left] shows why. A milling tool running at a light radial depth of cut takes on a much heavier engagement as soon as it enters the corner. The tool is likely to both chatter and deflect in this area—assuming it even survives the increase in load.

One way to finish the corners separately and safely would be to slowly side mill just this material. Another approach would be to plunge mill the corner material. Both techniques might involve large length-to-diameter multiples because the tool can be no bigger than the specified radius of the internal corner. After evaluating both techniques at length-to-diameter multiples ranging up to 5.5, the Boeing Research and Technology group (BR&T) in St. Louis ultimately arrived at a corner machining process that combines plunging and side milling together.

Plunging corners is inherently more stable. Experiments showed this. Compared to side milling, plunge milling reduces tool deflection and considerably improves surface finish, while cycle time results showed the best improvement of all. However, plunging alone is insufficient. To clear enough material from the corners to leave ample clearance for the wall-finishing tools, Boeing recommends a technique called plunge-and-sweep. After plunging the corner, side milling can sweep out more of the material adjacent to the plunged area.

The same tool can be used for plunging and sweeping if the length-to-diameter ratio is no greater than 4. Above 4, Boeing says, only similar tools can be used. The plunging tool tends to chatter as it descends deep into the pocket. To overcome this, BR&T engineers use a tool with a stabilizing land of about 0.004 inch on each cutting edge. The land rubs against the part material, essentially stabilizing the cut by acting like a bearing surface. Because the same effect is counter-productive in side milling, a separate tool is needed for the sweep.

These separate plunge and sweep tools could actually be the same except for the land. The only disadvantage would be the chance for confusing the two tools because the land is not easy to see. The shop performing plunge-and-sweep might therefore prefer different numbers of flutes for the different operations—just for the value of being able to easily tell the two tools apart.

A final advantage of plunge-and-sweep is that it opens up the possibility for the sweep to be quite large—making room for a tool much larger than the internal corner to perform the finishing of the walls. Perhaps best illustrated by the 45-flute tool in the article about the 8-to-1 rule at right, a larger tool permits more flutes, which allows finishing to be performed at a higher feed rate. In this way, getting the corner material out of the way before wall finishing ultimately makes the overall finishing operation much more productive.

Pricing The Process Instead Of The Tool

Click images to enlarge Expensive tools can actually reduce the overall cost of machining. The first formula computes the cost of removing each cubic inch of material based on the cost of machine, labor, and tooling—and the extent to which increased productivity can reduce the impact of the first two of these factors. The second formula makes a comparable calculation for the cost of finishing. The table is based on this second formula.

Apart from the toolpath considerations in machining titanium, one other important consideration is the danger of false economy when it comes to tool selection. The lowest-cost tool may or may not be least expensive option, say researchers with Boeing’s Research and Technology group in St. Louis. For example, high speed steel (HSS) tooling is used frequently in titanium because of the shock resistance of this material. An HSS tool might achieve a metal removal rate comparable to the best a typical carbide tool can deliver. When this is the case, the less expensive HSS tool can provide the better value.

But many shops have the potential to mill titanium much faster than they do today. The recommendations of the other articles in this series (see [above]) can allow shops to wring significant benefit from a higher-performance cutting tool such as a 10- or 20-flute carbide end mill. Because machining a part faster reduces the overhead cost absorbed by each piece, productivity improvements can easily make up for the added cost of the tool, even if the tool is quite expensive. This means buying the cutting tool solely for its purchase price can be costly. Even if the tool were free, the overall process might be more expensive because of the extent to which the cutter limits what the process can do.

The table [to the right] illustrates this point. The first two columns show HSS and carbide tools finishing ribs at the same metal removal rate. The "cheaper" HSS tool is also cheaper here in terms of cost per square inch. (Cost per square inch is the more appropriate measure of value for finishing. Cost per cubic inch works for roughing.)

However, the third column in this table is much different. The 10-flute carbide tool achieves a dramatically higher metal removal rate. As a result, even though this tool is more expensive, the overall cost of machining is lower.

The discrepancies between tool cost and tool value can be surprising. Instead of comparing tools, it is important to compare processes—or else the shop is likely to cheat itself with a process that is slow and expensive. The formulas the Boeing group uses to make this comparison are presented at right. Alternatively, enter the values into this calculator to immediately measure how changing the parameters affects the overall process cost—and to see in real time how to get to a more productive and more cost-effective process for machining titanium parts.