How to Machine Titanium Like a Pro

Titanium used to be a mystery material that only a few specialized shops could handle well. Now it’s nearly become a staple, and quite a few machinists will come across it at least at some point in their career.

Machining titanium brings some unique challenges compared to other more common materials like aluminum and steel. But since there’s good money to be made in this kind of work, more and more shops are eyeing up these jobs.

If this article, I’ll go over what strategies have worked really well for me, how to select great cutters, and what other considerations need to be made.

The Challenge

By far the main challenge with machining titanium is dealing with heat. Titanium is tough stuff, so the potential for heat from friction is huge. It also doesn’t conduct heat well, so the heat is focused in the cut zone and it doesn’t dissipate quickly.

A large percentage of the decisions you make will relate to the balance between programmed cycle times and heat.

The reason that heat is so deadly in titanium machining is because titanium work hardens. This means that if the material gets too hot while you’re working on it, it will get harder and harder. Harder material = more heat when cutting = harder material.

I like to think of it like surfing. If you stay ahead of that wave (hot zone), you’ll be fine. Let the wave catch up to you, you’re done. Fast, cool cuts are usually the way to go.

Machining Strategies for Titanium

The strategies for machining titanium are very different from soft materials like aluminum or mild steel. If you’re familiar with machining high-temp superalloys like Inconel, you’ll see a lot of similarities in approach.

Avoiding Jarring Engages and Disengages

Since the cutting pressures are so high, the shock that the cutter experiences when engaging and disengaging from the material really does a number on it. Aside from extra wear on the cutting edges, this is where the tool is most likely to chip.

Using larger arc-ins and arc-outs are a great way of reducing the shock. Even if you’re doing a straight cut along the outside of a part, a generous arc will help your tool last longer.

This is especially important when using high feed moves, like with peel or high-feed milling.

Plunge Milling

This is by far my first choice for roughing. You’ll be hard pressed to find a technique that will get a higher material removal rate.

The reason for this is that you’re cutting in the direction where the tool is strongest. Side milling pushes on the tool in a cantilevered way, whereas plunge milling directs the cutting forces straight up into a rigid spindle.

With a stable tool, the process can handle tremendous cutting force.

This process works particularly well on deep part geometry, like pocketing, or anything that a large diameter cutter can fit into.

The downside to this approach is that there will usually be a fair amount of semifinishing; plunge milling leaves a very scalloped , rough surface that needs to be cleaned up later.

Even still, plunge milling for roughing paired with peel milling for semifinishing and finishing is an extremely effective way of handling titanium.

Low Radial Engagement with Peel Milling

The classic approach of a 0.5xD radial and axial stepover really doesn’t work for titanium. This just generates way too much heat, and it’s really likely to snap your endmill in half.

What works way better is to maximize your axial depth of cut as much as the part geometry and flute length will allow, and use a small radial stepover. I find that 5-10% of the cutter diameter works really well. At more than 25% engagement, you really start to lose the advantages of this technique.

This works great for deep pockets and slots. With shallow geometry, you really start to lose the advantage of this technique.

A real perk of this technique is that it makes use of chip thinning – small stepovers produce thinner chips. This means that you can increase the feed to maintain chip thickness.

Use the calculator below to see how much harder you can feed the endmill to produce the desired chip thickness. Note: this is to calculate max chip thickness, not average chip thickness.

Another real advantage of peel milling is that the teeth are in the cut for much less time per revolution. This means that overall, much less heat is produced. It’s also distributed over more of the cutter, since there’s a higher axial depth of cut.

Since there’s less heat generated, you can often crank up the RPM. As a rule of thumb, you can often double the RPM with 10% radial engagement compared to a full slotting speed, and increase it by 50% for a 25% radial engagement. This is a significant increase in material removal rates.

If you’d like to know more about how you can get the most out of peel milling, I’d really recommend that you read this article about peel and trochoidal milling .

High-Feed Milling

This is a viable option when there’s a lot of material to remove and the geometry is highly accessible. It can also be a really effective way of tackling shallow geometry and facing operations.

High feed milling uses a really low axial depth of cut, usually about 0.030″-0.050″, but a full-diameter radial depth of cut. Using specialized inserts with large radii, we’re able to achieve significant chip thinning. This means that we can crank up the feed rate and remove material efficiently.

The downside to this is that these cutters are usually large in diameter – often around 1.25″ or more. This means that they can’t get in to tight corners for geometry like small pockets.

At the end of the day, though, this can be a really effective solution when the part geometry is a good fit.

Varying Depth

Titanium is a really tough material. It’s abrasive when you cut it, and it puts a lot of pressure on the cutting edges. There’s also a very thin but hard oxide layer that forms on the part surface.

What this means is that wear can really concentrate on the tool where it contacts the part at the top of the cut. This is a common area to see chipping on the cutter, which can leave lines on the part and cause a hot area that results in work hardening.

A really good trick to prevent this is to use a varying depth of cut. For example, if you’re using a cutter that has a 1″ cutting depth, don’t do all of your cutting 1″ deep.

If possible, do some cuts at 1″, some at 0.875″, some at 0.750″. This will spread that wear concentration along a greater area of the tool and increase tool life.

Thin Feature 8x Rule

A common application for titanium is aerospace parts, which typically have tall, thin walls to provide strength. With heavy cutting forces, these walls can deflect. This will result in walls that are thicker than permitted.

Here’s a good rule of thumb to use:

When the wall height exceeds 8x its thickness, special considerations need to be made.

In other words, if a pocket has a wall thickness of 0.090″, you’ll have a hard time using standard toolpaths if the height is over 0.720″.

A useful way to treat geometry that exceeds this is to leave a lot of stock for finishing. Leave enough stock to match this 8 to 1 rule, and then use a low axial depth of cut but a high radial depth of cut for finishing.

Turning

For turning titanium effectively, use the same principles as milling: Thin your chips!

Round inserts work well when the depth of cut doesn’t exceed 25% of the insert diameter. Beyond that ratio, the benefits of chip thinning are lost. You can use the same calculation for peel milling to determine how the feed rate can be increased.

For heavier cuts, try using tool configurations with a lead angle on the insert. For example, a 45-degree lead angle will produce a chip that is 30% thinner. That means that a traditional feed rate of 0.020″ per rev can be increase to 0.026″ if the tool has a 45-degree lead angle.

Selecting Appropriate Cutters

Cutters for titanium are very different from what you’d typically use for other materials, like steel. While regular endmills for steel will work for titanium in a pinch, they really won’t perform very well at all.

To illustrate this, I tested two different endmills under the exact same conditions. Same material, same holder, same speeds and feeds, same coolant, same program. The difference in performance were absolutely massive.

Here’s the video of this test:

Let’s go over some of the features typical of milling cutters for titanium. I’ll explain what they are and what they do.

Helix Angle

Titanium really sends a shock into the cutter every time the edge enters the material. To improve surface finish and make your cutters last significantly longer, these specialized endmills for titanium have a high helix angle on the cutting edges.

What this means is that the teeth spiral noticeably, instead of being closer to straight. Usually for steel the teeth will be as a slight helix, but for titanium the angle of the teeth is often between 30-60 degrees from the tool axis.

This results in a smoother cutting action that more so shears the material away instead of whalloping it off. You can really hear the difference between a low helix and a high helix cutter.

As always, this is just a matter of balancing parameters to find the “sweet spot”. A low helix leaves a poor surface finish and leaves the cutter more prone to chipping; a high helix endures more wear and therefore can dull faster.

Variable Pitch

Since titanium is such a hard material that sends shocks into the cutter, there’s a major risk of vibration when cutting. When these impacts matches the resonant frequency of the part and workholding, this can compound the vibration into something unmanageable.

Unless you have a variable pitch cutter. A variable pitch cutter has an unequal spacing between the teeth. What this does is break up the harmonics that you can otherwise get from the even, rhythmic slamming of the teeth into the workpiece.

So instead of having a 6-flute endmill evenly spaced with teeth 60 degrees apart, you’ll have one spacing at 63 degrees, another at 57, one at 59, one at 61, etc.

In essence, this reduces vibration. You’ll see this perform best in applications with low radial engagement, like with peel milling.

Variable Helix

A variable helix accomplishes basically the same thing as what the variable pitch cutter is aiming for. The uneven helices prevent that rhythmic hitting into the workpiece.

Sharp Cutting Edge

For metals like steel, prepping an edge by slightly rounding it can make the cutting edge stronger. This is especially common to see with indexable inserts. Since steel is free-cutting, the tool doesn’t need to be razor sharp.

This isn’t the case with titanium. A slightly rounded edge will put a lot of heat into the cut, resulting in work hardening and an overall bad day. The cutting edge needs to be as sharp as possible to keep the cut cool.

This is why titanium cutters will have something called secondary relief. Instead of a duller edge, there will be a very small flat along the cutting edge that’s not at such an aggressive angle. This makes that cutting edge considerably stronger, but doesn’t negatively affect the chip flow.

Basically, it makes your tools stronger and last longer.

There are a few different styles and sizes of secondary relief, so usually finding the sweet spot for your application is just a matter of a bit of testing.

Tool Accuracy

This is probably one of the most overlooked aspects of cutters. Specifically, the accuracy of the cutter shank.

If the cutter shank isn’t particularly precise, it affects how well the holder can grip the tool. For example, if the tool is undersized or has concentricity issues, you could have either a weaker hold or an imbalanced chip load.

Now I’m not saying that the tool will fall out of the holder (although that can happen too) but this can do two things to your process:

First, the weak connection won’t dampen vibration. Second, the uneven chip load will cause some of your teeth to wear out prematurely.

So when you’re looking at a lineup of possible cutter options and comparing prices, just take a look at the tolerance of the tools too. It can make a big difference on your process.

Number of Flutes

Some materials just have an automatic go-to for number of teeth on an endmill. Three for aluminum, four for steel… Not so with titanium.

In general, you’ll commonly see titanium endmills with 6-10 teeth. The number of teeth that works best is really dependent on part geometry and chip evacuation.

If you have a part with deep pockets that are at all kinds of tight angles, it’s really easy to bury a cutter in the corners. In this application, a 6 flute endmill might work best.

If your part is more so full of squarish pockets that are fairly open, then a 10-flute endmill might work great. It all boils down to what’s the largest amount of teeth you can pack onto an endmill without it getting clogged with chips.

With 10 flutes, you’ll get phenomenal feed rates. But if you’re shoving it into tight corners where there’s a huge amount of radial engagement and nowhere the chips can go, it’ll snap in half instantly. It doesn’t matter how fast your CAM says it can go, a snapped endmill won’t get the parts out the door any faster.

This usually is just a matter of testing. Eventually you’ll get enough of a feel for it where you’ll be able to guesstimate reasonably enough, but until then it’s just a matter of adding teeth until something breaks, and then going back one step.

Coatings

These are really important. For titanium, you want tool coatings that perform well with heat.

The most common coating you’ll find for titanium tools is titanium aluminum nitride, or TiAlN. This coating will create an aluminum oxide that protects the tool. This is my general go-to.

If you’re having problems with chipping, though, there’s another coating you can try. Titanium carbo-nitride is stronger and more resistant to fracturing. This is more common to see on indexable inserts, and it can really increase the life of your tool.

Workholding

Titanium really resists cutting, so your workholding needs to be dead solid. This is especially true for plunge milling. Here are a few pointers:

Whenever possible, direct your cutting forces against a dead stop, like a shoulder on a fixture.
For thin walled parts, like what’s common for aerospace, make sure the part is well supported underneath. Otherwise, it’s very likely that you’ll have a terrible surface finish on things like pocket floors, and they’ll tend to end up too thick.
Hardened steel grippers work really well for clamping rough stock.
Any fixturing elements that are under pressure with the titanium will be subjected to a lot of wear and tear. Try heat treating any fixtures that you want to last.

Machine Requirements

The good news for this is that modern machines are becoming more and more solid, even at an entry level. This is because modern tolerances are much tighter than they were even 15 years ago. This results in stronger, more accurate equipment.

Rigidity

Since titanium cutting is so prone to vibration, rigid machines really shine. If you need to remove a lot of material efficiently, don’t expect to do it on a cheap machine.

That said, even smaller, more entry level machines can do a good job of small components. They usually can’t take very heavy cuts, but if the job only requires small tools, then you don’t need anything bigger.

For something that will handle really hard milling, look for something that advertises rigidity against low-frequency vibration. This is because the cutting is done at a relatively low RPM, which translates into lower frequencies.

Power

For machining titanium, you want something with high torque, and generally lower RPM. Working out a practical max RPM is fairly straightforward. Just calculate the speed of the smallest diameter tool that you want to use to the full.

For example, let’s assume a max SFM of 600; it’s pretty rare to go above that when milling titanium.

If you want to maximize a 1/4″ endmill:

RPM = 600 SFM x 12 / π x 0.250″ dia.

RPM = 9,166

For a 1/8″ endmill, the max speed at 600 SFM would double to about 18,000 RPM. To be honest, though, it’s pretty rare that you’d ever run such a little endmill that fast. In real life, a 10k RPM machine will work great. Realistically, many of the high-torque titanium machines max at 6k RPM and they work just dandy.

In terms of torque, we can once again use some calculations to see what kind of machine stats would work well.

An average number used is 1 HP required per cubic inch per minute of titanium stock removal. Obviously, sharp tools will take less and dull tools would be more. But this is a nice, easy rule of thumb that will get you in the ballpark.

We can use this formula:

HP = Axial Depth of Cut x Radial Depth of Cut x Feed Rate (IPM) x Power Coefficient (1HP/cu in/min)

So let’s say that we’ll use a 1.0″ endmill to shear off a cut 1.5″ deep and 0.100″ wide, with a RPM of 800 and a feedrate of 24 IPM.

HP = 1.0 x 0.10 x 1 x 24

HP = 2.4 HP – really not a lot.

For torque, here’s the formula we’ll use:

Torque (ft-lbs) = 5252 x HP / RPM

Torque = 5252 x 2.4 / 800

Torque = 15.75 ft lbs – again not a lot, most machines should be able to handle this without any problem.

But let’s say that we want to drill a 2″ hole, pushing it pretty hard. Here are the parameters:

90 SFM = 172 RPM

Feed Rate = 0.007 CPT = 1.2 IPM

The area of a 2″ circle is 3.14 sq in. The cut will take only 3.14 HP, but it will require 96 ft-lbs of torque!

In other words, low-end torque is really important if you want to take big cuts.

Depending on the operations you want to do, your existing machines might not be up for it. You may not be able to push the tools as hard as what they’re able to take. Take this into account when quoting titanium jobs – you need to know what your machines can handle.

Coolant

For machining titanium and other high-temp superalloys, proper coolant is absolutely critical. Some say that it’s one of the most important things to get right.

Aside from making sure that you’re using a high-end concentrate and you follow the manufacturer’s mixing instructions to a T, coolant delivery is a major aspect of being successful.

Titanium puts a lot of heat into the tool. Way more than other materials, like hard tool steels or steel alloys. The coolant needs to be directed straight into the cut area with high volume and high pressure to get rid of this heat.

High pressure coolant, in the range of 300-1000 psi is considered a must by most machinists. The tricky part is that the coolant can push chips back into the cutter. This chip recutting not only drastically reduces tool life; it can cause process instability when it builds up and snaps the tool.

Through-tool coolant is a really good idea. High-end cutters will have a well thought-out delivery system that puts the coolant right where it needs to be, with enough pressure and volume to blast chips even out of deep pockets.

I’ve noticed a major difference in tool life when the right coolant is being used properly. Aside from making your process more productive, it also makes it safer. Titanium chips are very flammable, and if the coolant isn’t taken care of properly, you could have a very hard to put out fire in the machine. I’ve seen it happen in my shop several times.

Tips

Don’t hit feed hold or slow down your feed while cutting.

This is pretty well guaranteed to make your cutter rub and it’ll make a hot zone, while will cause work hardening. Once you’re in the cut, let it run.

Change your cutter as soon as you have signs of wear.

Tool wear with titanium isn’t linear. When it fails, it fails fast. It’s better to be swapping your tools out quickly so you can send them out for regrinding instead of crying over carbide pieces and scrapped work.