CNC programming (AEROSPACE)

CNC Programming

Toolpaths and programming techniques Hardened steels Titanium High-temp alloys

V0.1 9/11/2019

“Difficult to machine materials”

Machining has specific rules.

So what causes poor tool life?

▪ Speed?

▪ Feed?

▪ Chatter?

▪ Vibration?

▪ Tooling?

▪ Fixturing / component location?

▪ Harmonics?

▪ Chip section?

▪ axial / radial depth of cut ?

▪ Toolpath?

▪ Conventional / climb ▪ Instability ▪ ‘snatching’

“Difficult to machine materials”

Using specific machining techniques, it is possible to improve the cutting tool performance or time life: •Address heat generation! – (arc of engagement) •Control cutting forces (stability) •Entry and exit paths (arc on /off)

•Trochoidal toolpaths (slotting & profiling) •Helical interpolation…(hole making and pocket entry) •Plunging…(directing cutting forces) •High Feed Technology…

Cutting Fundamental impacting the programming.

• Utilizing a small radial depth of cut (ae) results in a small arc contact width • This allows for limited heat generation along the cutting edge, coupled with a much longer time to cool out of the cut

Out of Cut ae (Radial DOC)

“Arc of Contact” or “Degree of Engagement”

The theory Uncut chip thickness radial measurement plane fZ = Feed per tooth per revolution

fZ

rC = Cutter radius ae t = Full uncut chip thickness t

ae = Radial DOC

rC

The theory

• The uncut chip thickness can be found by: 2

2 t = rC −  rC − (rC − ae) − fz  + (rC − ae)   2

2

• This equation can be used to solve a value of fz that will give the correct chip thickness at the given ae • Example: 10mm endmill, recommended fz 0.040mm, 0.8mm ae 2

2 tc = 5 −  52 − (5 − 0.8) − 0.04  + (5 − 0.8)   2

– t = 0.022mm – To get tc = 0.040mm, adjust fz to 0.074mm

in practice, the surface finish controls what can be achieved – and even then it depends on tool concentricity… Feed marks on the surface are generally caused by eccentricity rather than feed / tooth. (if you measure then they relate to feed/rev rather than feed/tooth) In addition to chip thickness correction you also have to consider deflection – very often it is not possible to achieve the theoretical chip thickness required – particularly on long reach applications.

Now, we are not mathematicians…

for us ‘engineer’ a good formulae is to use Hm or average chip thickness – with a simple calculation for reference… here are the calculations

Take Away

• Solve correct fz to correspond with ae – will increase programmed feed rate • Start at high end of Vc (cutting speed) – Tool will stay cooler allowing higher speed – Can obtain as much as 2X normal recommended Vc

• Axial depth of cut ap can be maxed out – Limitations will be spindle power and workholding / part rigidity

These three steps will maximize overall MRR

On long reach finishing tools you need to calculate ap to give two points of contact – this stabilises the tool, having one flute ‘in cut’ as the second flute impacts the material. The best results without increasing deflection is to use 2 points – up to – but not including three points. This gives maximum ap values for the RSM range….

The first principle of machining

When the cutting edge penetrates the material and shears the excess away from the parent body. It is true for every machining process (turning, milling, drilling, grooving etc…) The chips shown are the ‘bits we throw away’ yet show many indications of the chip creation / correct cutting… the steel chips (high feed) show the oxidisation or tempering colours indicating correct speed (brown to dark blue) the laminations are very clear, the exit point of the chip well-formed indicating the correct feed rate…. More difficult to see in stainless steels / titanium – but never the less the chip formation is the same.

Chip Creation and Problematic Areas

Thin entry (CONVENTIONAL MILLING) creates friction and shear heat before the chip is created, the chip section is very thin and cannot absorb the heat, therefore the heat remains with the cutting edge and accelerates tool wear.

Thick exit creates an additional problem of chip adhesion which when exported from the cutting edge can break down the cutting edge definition.

“Thick to thin” entry (CLIMB MILLING) creates a large chip section immediately the shear process begins, this allows heat created to be absorbed by the chip, flowing away from the cutting area as the chip is created..

The largest chip section – created early and away from the cutting edge - assists centrifuge forces in removing the chip. The “thin exit” helps prevent chip adhesion and edge definition failure.

Choice of Diameter – 70% rule ?

Entry – Keep Calm and Arc On.

Exit –

SOLUTIONS

Progressive ‘thick to thin’ machining section

SOLUTIONS

On breakout the cutting action is conventional on the left hand side, pushing material away from the cut and tends to roll material away… the cutting action on the right hand side is climb milling and snatches as it breaks through – more importantly – from the moment the cutting edge breaks out until the centreline of the cutter exits the material, the cutting edge hits an extremely weak section of material. This either pushes away OR more likely – snatches and pulls the weak section into the cutting path creating shock to the cutting edge (instability).

If you machine part of the left hand side of the exit away, it does several things…

1.

2.

3.

The subsequent slotting tool does not break out on centreline The breakout section on the left hand side becomes a wedge section and is stronger than the section produced by normal breakout, preventing the push and roll off created by the conventional cutting action.

The material to the right hand side is much stronger – and has the same effect as machining a 45 degree on exit. The majority of the cutting action from the breakout position is thick to thin (climb milling) and gives a progressive reduction in cutting force… compared to the section produced by normal breakout which is a thin ‘point’ on a weak section for the majority of the remaining toolpath.

SOLUTIONS

FACING

▪ Unidirectional ?

▪ Bi-Directional ?

▪ Thin to thick chip creation… or thick to thin ?

SOLUTIONS

1.

3.

4.

2.

Facing, an alternative method : 1. Prepare the corner 2. 2nd pass 3. Subsequent passes 4. Last pass

CORNER TECHNIQUE

CORNER TECHNIQUE

Loop and arc onto previous tangent point Continue on profile – ‘kissing’ corner Tool remains stable and arc of contact is progressive and controlled

DEPTH OF CUT NOTCHING

The explanation shown is profiling, similarly a slotting operation with two passes or more to achieve depth could be produced by a different Z start and a plus z finish (creating a taper) which is corrected in the next pass – in both cases the depth of cut changes incrementally – spreading the depth of cut notch over a constantly changing area of the flute.

TROCHOIDAL MILLING

• Trochoid: the curve generated by a point on the radius of a circle or the radius extended as the circle rolls on a fixed straight line – Also includes variants which follow along a curve

• Trochoidal milling is an enhanced method of peel milling which allows a slot to be produced while controlling the radial engagement • Essentially the endmill is moving in a motion similar to circular interpolation while shifting the center of the circle along a defined path

Trochoidal milling is not necessarily used for slotting, it is mainly used for metal removal where the ae value (set in the CAM control) exceeds the maximum allowed. This makes the machine take several ‘swarfing’ or profiling cuts to achieve the profile required – typically corners or deep features within a component design Then following this logic – it’s possible to create not just a parallel slot – but any profile or feature within the aperture… The program shape does not have to be circular – it can be arcs and flats – D shapes – in fact any toolpath where the arc of contact is controlled to a percentage of the tool diameter.

The objective is to run at maximum speed for a given arc of contact – without variation of arc of contact, where the temperature will rise beyond the operating temperature should the arc increase…

The same process can be applied at lower cutting speeds – and used in conjunction with indexable tooling – where the step over can be increased accordingly… this is often referred to as High Performance Machining rather than High Speed Machining…

TROCHOIDAL MILLING RECOMMENDATIONS

• Endmill diameter should be at least 15% smaller than desired slot – Prefer 35% smaller – Consider corners in part

• Use a stepover that is between 5 – 12% of the endmill diameter… with usually 9% the optimum for titanium.

• Use the calculated maximum radial depth of cut as the ae to calculate chip thickness using procedure for basic peel milling

Stepover

TROCHOIDAL MILLING RECOMMENDATIONS

2 2   2 w  w      rC −  − rC + stp  −      w 2   2   ae = stp +    1 −    2    (2  r − 2  stp − w)   w        C  2    

stp

Maximum Radial Depth of Cut (ae)

rC w

▪ Trochoidal machining maximizes material removal rates and frequently enables the part to be machined to final dimensions in a single process (vs. typical defined rough and finish operations).

▪ This is possible because Trochoidal machining minimizes stress induced into the part during machining. We should note the Trochoidal process requires tools designed specifically for that operation and the Harvi III frequently establishes the performance benchmark

3D PROFILING / 3D CONTOUR MILLING

Create a smooth accurate surface As close as possible to desired surface geometry Reduced cusp height and time spent hand-finishing

Material removal rate Maximize MRR while achieving goals above

Tool life Long edge life, reduced breakage while achieving goals above

Achieve the above in difficult materials Hardened steels Titanium High-temp alloys

End Radius Effect - Uncut Thickness

Maximum approximated uncut chip thickness

tcfrp = Full uncut chip thickness in radial plane tcfrp ap = Axial depth of cut ap R Hmax R = Radius of cutting edge revolved profile Hmax = Uncut chip thickness

End Radius Effect - Uncut Thickness

• 1

rEC = R 2 − ( R 2 − ap) 2

• 2

2 tcfrp = rEC −  rEC − (rEC − ae) − fz  + (rEC − ae)  

• 3

2

2

2

2

2 tc = R −  R 2 − (R − ap ) − tcfrp  + (R − ap )   2

Radius R is extremely important to uncut chip thickness!

End Radius Effect - Uncut Thickness … for us in Aerospace : The tool with an approach angle (or both) gives a better explanation on the working diameter (De) : the benefit of machining “off centreline” encourages surface speed, better cutting action and chip ejection.

In explanation:

The chip created in the upward toolpath has surface speed across the complete cutting area (min at finished surface max at De) an open flute profile to eject the chip effectively. Whereas the downward path cuts across the cutter centreline – has ‘zero’ surface speed on centreline, and has a small flute cross section with 360 degree cutting (hence ‘drill’) chips are restricted and are difficult to remove.

The surface produced by upward cutting is generally clean – compared to the downward toolpath which has a tendency to cause galling – or cold welding of chips onto the finished surface. Tool wear characteristics are flank wear on the upward cutting toolpath and chipping or micro rupturing on the downward toolpath.

MRR as a geometrical effect

• MRR comparison at adjusted feedrate to achieve equal uncut chip thickness tc – 150 sfm, 1/2” diameter, .0068” fz, .050 stepover, .060 ap • Ballnose Endmill - .0468 in3/min

– 150 sfm, 1/2” diameter, .0098” fz, .050 stepover, .060 ap • Contour Endmill - .0674 in3/min

• MRR comparison at adjusted feedrate to achieve equal uncut chip thickness tc and equal cusp height H – 150 sfm, 1/2” diameter, .0068” fz, .050 stepover, .060 ap • Ballnose Endmill - .0468 in3/min

– 150 sfm, 1/2” diameter, .0087” fz, .065 stepover, .060 ap • Contour Endmill - .0780 in3/min

67% Increase in MRR at these conditions!

Experiment with AdvantEdge in Contour Milling

Experiment with AdvantEdge in Contour Milling

Summary on how to Approach Contour Milling

• Analyze the part and pick the best tool – Switch to contour mill / KenFeed design if possible – For ball milling need to consider Harvi Ball

• Pick key scenarios in the machining path of the part and calculate the adjusted feedrates based on cusp height and chip thickness • Remember to also adjust Vc (cutting speed) to effective cutter radius rEC

• Contour milling is essentially basic peel milling but done axially rather than radially

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.

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

The 8-to-1 rule can be stated as follows: an unsupported section of Ti6-4V needs to have a cross section strength of 8:1 for the material to be rigid enough for it to be machined. The impact force must be less than the material cross section strength, otherwise the material deflects and begins to vibrate. The cross section strength of other titanium alloys are slightly different but nevertheless follow a similar strategy. This rule is then applied to the cutting tool and the material section BEFORE machining; for example, the stated 1/8” finished wall can be machined with an axial depth of cut of 1.16” given the machining allowance of 0.020” (0.125” + 0.020” = 1.160”) this is also true for roughing and semi-finishing where the wall section before machining needs to follow the 8:1 rule.

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.

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

In applying tools to the cross section the choice of diameter is controlled by two factors – 1. The reach or depth of feature to be machined 2. Any feature or corner radius contained within the feature – (this could be pocket corners or upstands which restrict the maximum diameter possible).

Applying flute count and axial depth of cut depends on the depth of the feature. Axial depth of cut should not exceed the 8:1 rule – BUT – the first pass should be calculated without a full radius – it’s only the last pass where the radius comes into full contact when producing a shoulder or floor of the pocket.

The flute count ideally needs to give two points of contact as a minimum and up to, but not contacting three points, to minimise deflection (especially on long reach applications where tool to shank diameter ratio is greater than 5:1) combined with the radial depth of cut (ae) the distance between the points of contact indicate the correct flute count…. A single point of contact will cause vibration! a)

The higher the flute count - the shorter the axial contact points (especially true for 2” diameter x 45 flutes – excellent for large substantial sections – but not for the majority of Aerospace components & thin walls!)

b)

An increased flute helix – also reduces the contact points (a reduced helix will increase the distance between contact points)

c)

ae can also effect the distance between points – an increased ae will produce a shorter distance than a reduced ae value.

Axial depths of cut can be modified to prevent depth of cut notching (working between the two to three point contact) but consideration should also be given to the last pass which will include the full radius.

NB: It’s interesting to note that “one shot machining” follows a similar strategy – the tools tend to have less helix and therefore can use large ap values – but still apply the 8:1 material section wherever possible.. also concentricity becomes a major issue with large diameters and high flute counts, as surface finish is dictated by feed / revolution and the feed marks become more obvious compared to a smaller diameter.

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

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 stepdowns 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.

Plunge and Sweep for Finishing The Corners

Though the “slicing” technique described in the article “Getting The Metal Out” (see Editor Picks at right) can be effective for roughing material from a corner in titanium, the considerations that go into finishing an internal corner go well beyond efficiency. Surface finish and part accuracy during the finishing pass also have to be considered—and both of these concerns are likely to be unmet if the same tool that finishes the walls of the pocket proceeds directly into the corners. When finish milling titanium, the corners have to be treated as an entirely separate operation, often performed before the finishing of the walls.

A drawing at enclosed 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.

Plunge and Sweep for Finishing The Corners

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.

Getting The Metal Out

The article at right 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.

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.

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.

This approach represents the most productive material-removal process for pockets in titanium. 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.

Getting The Metal Out Note of the expert :

Chip removal from a drilled hole can be an issue – especially on vertical machines – the chips tend to be retained within the hole and re-cutting chips becomes a problem, especially when taking several passes in Z where chips collect within the lower part of the hole.

With high feed machining the best combination is helical entry into the material – then open out the feature… ramping, particularly a slotting entry, can sometimes cause more damage due to the full ‘wrap around’. In addition, depending on the length of the feature, the axial depth cannot be reached in one direction, if the tool dwells – instability occurs and resultant early damage to the cutting edge follows…

This is particularly true when using long extensions – it pays dividends to create a large radius in the corner – then profile or loop - using a smaller radial engagement to minimise this effect.

Getting The Metal Out

Drill And Plunge This technique is a problem solver. 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 plungemilling 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.

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 40taper 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.

Getting The Metal Out Note of the expert :

whilst we would agree with the statement that a circular insert can ramp more aggressively – it does not mean that it is either quicker or achieves a deeper depth of cut. Yes, high feed requires a shallow angle of entry – but it does so much quicker than the round insert… and for an insert of the same IC? –

A round insert uses up to 25% of the IC so a 12mm insert uses up to 3mm - against the hIgh feed 12mm insert 2.5mm – but the metal removal rate is 2 to 3 times quicker….

Getting The Metal Out

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? “slicing”—which also could apply to the material left over in the corners after any of the three pocketing techniques described above.

Getting The Metal Out

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 at right).

High feed: due to the size and shape of the chip created in large radial engagement (80% step-over) insert damage can occur when the chip traps between the upper part of the insert (non-cutting) and the wall.

To minimise this possibility consider changing the last pass to 25% step over – the chip created will be smaller and therefore has more room in the flute to prevent collision with the side wall.

Getting The Metal Out

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. 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.

A Two Speed Approach To Plunge Roughing

The tool paths for a plunge roughing routine ought to be straightforward. Indeed, a plunge roughing move is literally straightforward, in that milling in this way involves driving the tool directly into the workpiece along the Z axis. The tool cuts on its face, feeds back out of the work, steps over to make an overlapping plunge and so on.

The step over is where the strategy lies. Adjacent plunging moves need to overlap to some extent (in part to provide an opening for chips to escape), but how much overlap is enough? What pattern of plunges is the most efficient?

Efficiency, after all, is the point of plunge roughing. Taking advantage of a machine’s stiffness along Z, the technique permits more aggressive cutting of harder materials in cases where that hardness might constrain cutting with conventional X- and Y-axis milling paths. In aircraft part machining, the technique is sometimes used to quickly hog pockets out of titanium. With pockets in these parts getting deeper, personnel with Boeing’s Advanced Manufacturing R&D group in Saint Louis, Missouri, have been experimenting with plunge roughing in search of strategies for optimizing the technique’s effectiveness.

Boeing engineer/scientist Keith Young offers an example of such a strategy. It involves a 2-inch diameter plunge roughing tool. When milling titanium with this tool, Boeing personnel achieved the highest productivity through a strategy that uses two different speeds.

The first pattern of plunges is made at 200 rpm, he says. The stepover increment is 1.8 inch—a stepover close enough to the size of the tool that there is little overlap between plunges. The design of the tool, with its clearance for chips, is part of what makes this large spacing possible.

Four-point “stars” are left standing between the widely spaced plunges (as the illustrations show), but these stars can be removed quickly. A follow-up pass takes out these posts at 400 rpm.

Using this two-speed approach, Dr. Young says a pocket can be roughed out of titanium in relatively little time. Boeing typically applies the strategy to deep pockets by plunging away the material in levels of 0.5 inch.

Appendix

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.

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.

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.

Pricing The Process Instead Of The Tool

Apart from the tool path 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 “Editor Picks” at right) 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 (middle photo) in the sidebar on 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.)

Pricing The Process Instead Of The Tool

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 a 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 costeffective process for machining titanium parts.

Sources

ATI Tungsten Material Group The Boeing Research and Technology group Modern Machine Shop Kennametal Team

Shivanand Durge Program Manager Aerospace & Defense