I’ve been working with companies that are industry leaders in areas like HSM for the past 14 years.
I’m going to share everything I’ve learned about what HSM is and how you can pull this off successfully in your shop.
What Is High Speed Machining?
For many people, this term can be a little vague. For all the companies that boast HSM that I’ve worked with, all of them had slightly different definitions of what it meant.
For example, one company defined it as anything with a spindle speed over 20,000 RPM. According to this definition, micromachining with a 0.005″ endmill is HSM by default. That doesn’t really capture the intent.
Another company defined it as any kind of machining that removes material quickly. Again, not the clearest definition. A 150-HP mill with a 8″ diameter shell mill facing a steel plate will remove material quickly, but this is a really old-school approach. This doesn’t really define HSM well.
So what is High Speed Machining, then?
Here’s the best, simplest definition that I can give:
High Speed Machining is a machining methodology that focuses on extremely fast but light, low pressure cuts. The result is an overall increase in the material removal rate.
This explanation is a good way of separating things that could be considered HSM by default from the stuff that really makes the cut (see what I did there?).
Ultimately, HSM works on a gradient. It can be done to varying degrees, but the principles can be applied across the spectrum.
It’s not just a matter of RPM. The intention with HSM is using high speeds to achieve a high material removal rate. To accomplish this successfully, there are eight pillar concepts that need to be understood. Here they are:
- Rigidity of Tool and Workpiece
- Tool Balancing
- Tool Harmonics Testing
- Controlled Tool Load
- Chip Thinning
- Cutter Selection
- Material Understanding
- Machine Requirements
While many of these concepts are highly applicable to standard machining, they’re taken to a whole new level with HSM. In fact, it can take a bit of a “development phase” to get this all right when you’re setting this up for the first time in a shop.
So why is this such a challenge, and how can you actually do this successfully?
Why High Speed Machining is Challenging
Ok, so if you simply crank the speeds and feeds on the controller, very bad things will likely happen.
High Speed Machining is all about being able to compensate in other ways. Simply pushing tools harder will make them break. You need to approach this in a well thought out way.
Beyond that, there are a few common challenges to High Speed Machining. Here they are:
- Lots of metals work-harden. Running at high RPM can mean more heat generated during cutting. Some metals get extremely hard when heated and will cause catastrophic tool failure if measures aren’t taken to reduce heat.
- High speeds increase the risk of vibration, or chatter, while cutting. This drastically reduces tool life and can easily damage and scrap the parts.
- The cutting forces can actually be quite high. A common problem is for tools to pull out of their holders and cause major issues.
- This is high performance machining! Not all machines, especially older ones, are up for the task.
- The toolpaths that enable these speeds are more advanced. They require a measure of extra training, as well as a solid CAM package to do successfully.
- It can be extremely expensive to set up for truly high performance HSM.
This isn’t an exhaustive list, but it gives you an idea of why a lot of shops are hesitant to jump on board. If not done properly, you can do a lot of damage.
If all you’re doing is bumping up the RPM on your machine, you’re not getting the most out of HSM. Let’s go over the pillar concepts of High Speed Machining and how you can put them into practice.
1 – Rigidity of Tool and Workpiece
Vibration is enemy #1 in High Speed Machining. This is often the single greatest challenge when applying this methodology. If you can’t keep your cutter from screaming, your tool life will be horrible and the part will look like garbage, if not scrap.
When the cutter engages the workpiece and starts removing material, there’s a chain of connections. Each one allows for a certain amount of vibration to transfer. This is generally what it’s made up of:
- Rigidity of the machine spindle
- Connection between toolholder and spindle
- Connection between any extensions on the tool
- Connection between the tool holder and the cutter or inserts
- Connection between the workpiece and the workholding
- Connection between the workholding and the machine table
- Rigidity of the machine table
All of these need to be solid to prevent vibration between the cutting edges of the tool and the part. Just like a chain, the weakest point will bring down the whole system.
Now all of this applies to traditional machining. But with HSM, you’re demanding high performance from your equipment. That means that this setup needs to be significantly more reliable. Special attention needs to be given to getting the most out of each element.
There have been several developments over the years that have made this more attainable. Let’s do an overview of some of these and see how they make HSM doable.
The connection between the tool holder and the machine spindle is critical. There are a number of different styles of connection that offer advantages in this arena.
For example, the HSK style of toolholder for many years has been considered the gold standard for HSM. HSK is the German abbreviation for “Hollow Taper Shank”. It works on an interesting principle.
When you slightly deform metal under clamping, the connection tends to have vibration-damping properties. This could be an entire article in itself, explaining why this is, but for now let’s just leave it at that.
HSK tooling is clamped from the inside, and the clamping pressure actually slightly bends the metal. The result is an incredibly rigid, vibration-dampening connection.
Basically, it keeps your tool really solid. According to some studies, the HSK connection is as much as 5x stiffer than common steep-taper connections like CAT, BT or SK.
Other Tool Tapers
There are some other types of tool connections that work under a similar principle. For example, Kennametal has the rights to producing the KM toolholding system.
There are also improvements that have been done to the standard steep taper connections that have improved the rigidity. For example, tighter tolerances specified by new DIN standards make more precise fits, meaning a more solid connection. There are also toolholders that are dual contact on both the flange and taper, like the popular Big Plus™ systems, which increase rigidity.
There are also some really great ways of gripping endmills that are more conducive to HSM.
The standard weldon shank endmill holders are not suitable for HSM. Neither are standard ER collets – they both just allow for too much vibration.
Heat shrink and hydraulic tooling, however, work great. Hydraulic clamping has inherent vibration damping properties, and heat shrink grips the tool extremely well.
There are also other really effective systems, like Duo-Lock™, which prevents pullout. Pullout happens when the tool vibrates and pulls out of the holder. This means that the tool is now longer than the machine realizes, and it’s pretty well guaranteed to be catastrophic.
Since fixturing is such a huge topic, I’ll keep this high level.
Your clamping needs to be really solid to hold up to these cutting forces. Holding on to the bottom 1/8″ of a part in a vise is pretty unlikely to give you the results you’re looking for.
Some shops use dovetail vises to lock the parts in place. Some use really strong edge clamps, like cam-lock systems. Many use grippers to bite in to raw stock.
For aerospace parts, this can be really tricky. They’re often very thin-walled, so the parts themselves will ring like a bell while you’re cutting them if you don’t take special measures.
2 – Tool Balancing
For the shops that are committed to HSM, this is a must. Many toolholders are balanced to a rating of 10,000 RPM off the shelf. Thing is, HSM is often done way above this, usually at 20k RPM and up for aluminum.
If the tool isn’t properly balance, the vibration can really damage the machine spindle bearings. It will also significantly reduce tool life and give you a nasty surface finish.
This is something that can be really fussy. A tool that’s not balance will cause vibration. To illustrate how important this is, Sandvik did an interesting test.
They put a little sticker on a balanced tool and ran it at 15,000 RPM. That sticker put the tool out of balance by over 3 pounds at that speed.
As tools become longer and are run at a higher RPM, this becomes really critical.
Cost of Tool Balancing
The reason that not every shop is balancing their tools is because 1) the equipment can be expensive and 2) it requires more time to set up the tooling.
The balancing equipment itself has a large price range. Basic models that are slower to process tools can start at around $10k for something that’s still name brand. From there, you can pay upwards of $60k for something more automatic.
Besides that initial expense, it takes time to balance tools. Every time you put a new endmill into the holder, you need to re-balance. This means tying up personnel. In other words, the benefits of tool balancing should outweigh the expenses.
3 – Tool Harmonics Testing
This has been around for a long time, and it’s just as practical now as when it came out. Some people refer to this as “ring-testing”.
Essentially, every tool assembly will have a frequency at which it resonates. When the cutting edge hits the metal, this sends a shock throughout the tool. If this frequency matches poorly with the tool assembly’s frequency, vibration will be amplified instead of dampened and things can explode.
A harmonic tester has a striker that will tap the tool assembly near the tip. A sensor will read the vibration. A computer will plot a chart that will indicate “safe” and “unsafe” ranges of RPM that the tool can be run at.
Probably the most well-known company that makes these testers is Blue Swarf. From experience, I can tell you that this system makes a huge difference when you’re cutting aluminum at 22,000 RPM with a 3/4″ endmill with a 14″ gage length.
Essentially, it’ll help you find that “sweet spot” for that high RPM before you load the tool up into the machine and hit the green button.
4 – Controlled Tool Load
Even with a balanced tool that’s been ring-tested, you can get extreme vibration. If your tool load is constantly varying while it’s working, you can get huge problems with chatter.
This is especially true in tight corners. With a standard linear toolpath, there will be a really high radial engagement as the tool pushes itself into a corner. Typically the cutter contact doubles. This excessive engagement usually leads to chatter, which shortens tool life and gouges the part as the tool vibrates.
Beyond corners, you need to be careful with lead-ins and lead-outs. If you engage the material in a straight line, it puts quite a shock on the tool.
This isn’t a big deal for traditional machining. But entering the material at 30 inches per minute versus slamming into it at 800 inches per minute are two very different things.
Straight disengages from the cut can put shock on the tool too.
One solution is to arc in or arc out of the cut. This does a lot to soften the blows and load the cutting pressure evenly.
You’ll also want to make good use of peel and trochoidal milling for tight areas. Trochoidal milling is useful for machining slots and other tight areas, like corners in pockets. If you want to know more about how you can properly apply these techniques, you’ll probably want to read through this article.
5 – Chip Thinning
This is more than just an issue of climb versus conventional (up vs down) milling.
By using the low radial depth of cut that peel milling is famous for (if you’re not familiar with this then you really should read that article linked to above) you’ll end up with much smaller, thinner chips.
This allows for really
While you can definitely use these principles to an extent for soft materials like aluminum, you’ll really see this shine in exotic metals like titanium, Inconel and other high-temp superalloys. Aluminum is usually buttery enough that you can push a cutter through it fairly hard. Not so with the superalloys. They’re just too super.
Another major advantage to this is that thin chips allow for really fast heat dispersion. The chips take the heat away from the part, and when the tool has less contact with the chips, less heat is taken.
As you can probably imagine, High Speed Machining has the potential for a lot of heat, so anything you can do to prevent this from building up is only going to help.
This is an advantage for cutting aluminum but this is absolutely mandatory for work-hardening materials like titanium, stainless, and Inconel. If you can’t get the heat out in the chips, the metal will harden, break your cutter, and create a hard spot that will be very difficult to get rid of.
6 – Cutter Selection
The cutters used for HSM are different from the ones that you’ll use for more traditional machining. Basic requirements are to match cutter geometry to material needs, stabilize the tool, and maximize rigidity.
Again, this is a huge topic, but here are the highlights:
Since HSM is so demanding, we need to do everything we can to make sure that there are no weak points.
Typically, sharp corners are an area where stress really concentrates. In a high-performance application like HSM, a larger corner radius will make a huge difference in terms of dispersing that stress and improving tool life.
To put this really simply and make it as practical as possible, here’s what I’ve experienced. If I’m going to do some machining with a 1/2″ endmill, these are my typical options for a corner radius:
- 0.030″ – Better than nothing
- 0.060″ – Noticeable improvement
- 0.090″ – Works great
- 0.120″ – In the range where it doesn’t really matter, and probably part geometry will make this more annoying than it’s worth.
I’ve found that these work well across the board in everything from soft aluminum to 4340 steel to titanium and Inconel. Protect your endmill corners whenever possible.
While this an element that’s the same across the board, other things are very material-specific.
HSM Tooling and Aluminum
Chip clearance is very important, but this isn’t anything specific to HSM. Something that does make a real difference, though, is how easily the chips can slide across the flutes of the tool.
This is why a lot of shops really like to use polished carbide endmills. Instead of having grinding marks that create friction, a polished carbide endmill allows the chips to easily slide off the tool, making for a smooth, low-heat cut. It actually ends up noticeably increasing tool life.
There’s another thing that’s really interesting when it comes to using carbide cutters: edge prep.
Now we all know how important it is to have a slightly rounded cutting edge when cutting steel with inserts. For aluminum, though, you traditionally want the cutter to be razor sharp.
With HSM, though, it’s different. A razor sharp endmill at these speeds will actually bite into the material too much. This means that there will be uneven forces when cutting, something that will likely cause vibration.
I’ve found that endmills with a slightly rounded cutting edge are far more stable. The cutting pressure loads up the tool, and the result is stability. At one shop that I worked at, we would actually just run a hone stone down the flutes before running it, to break that edge down slightly. It ended up working way better than a sharp too.
HSM Tooling for Titanium and Inconel
This is completely different from aluminum. Instead of large gaps between the teeth for chip clearance, we go the opposite direction. We pack as many flutes as we can on a single cutter.
It’s common to see half inch endmills with anything from 6 to 10 flutes. There are two major advantages to this.
More flutes mean higher feedrates.
The best HSM technique for these alloys is peel milling. Since the radial engagement of the tool is low, the chips are small and thin. This means that you don’t need a lot of chip clearance. Ultimately, you can pack more teeth on to the cutter and use a higher feed rate to keep all these teeth busy.
Smaller flutes mean a larger core diameter, which gives a stronger tool.
Because these flutes are small and shallow, there’s simply less carbide ground away. The core diameter of the tool is significantly large, and the tool is much stronger. This means that it can take more abuse before it snaps. You can really push these things.
7 – Material Understanding
At the end of the day, you need to understand the material that you’re working with. HSM is different for aluminum compared to titanium.
For example, cutter RPM for titanium is usually pretty low for roughing. Often you’ll be running at 200 SFM or so. For the finishing, though, the speed can be cranked up considerably. Commonly you’ll be finishing at 300 SFM or higher.
In all honesty, titanium roughing is often done in a more traditional way. I’ve never been able to beat the material removal rates of plunge milling in titanium. Where plunge milling isn’t practical, though, high speed peel milling is a great option.
Aluminum could not be more different. Since the material is so soft, you can bury the cutter quite deep as long as you can keep the load consistent. What’s really important here is tool balancing and checking harmonics.
The bottom line here is that you need to get familiar with different materials. Just because you’ve done HSM in aluminum, that doesn’t mean you’ll do a good job competing with titanium.
Ultimately, by specializing in a few different types of materials, shops car really develop high-performing techniques to get the most efficiency possible.
8 – Machine Requirements
Really, you don’t need to have a million dollar machine to do high speed machining. Modern machines are getting better and better at handling it even at an entry level.
Don’t get me wrong. The big expensive machines are amazing. The Makino Mag 3 is an aluminum profiler that costs a pile of cash (or good credit) and it’s an absolute beast. I’ve worked on a massive Cincinatti gantry mill that would spew aluminum chips 100 feet from the spindle. The operator’s job was to try to shovel the chips faster than the machine would make them. The machine had 3x 100 HP spindles, so the operator never won.
But you can also do solid work on the $200k machines. With lower overhead, this option might make a lot of sense.
The only time that you’re very unlikely to succeed is if you try to push a tired old mill from the 90’s at these speeds. It will likely die. These machines have their place, and it’s not in the HSM arena.
So what are some key features that will let you really take advantage of high speed machining?
Block Look Ahead and Processing
High speed machining means that the controller needs to process a lot of motions fast. Block look ahead means that the controller will read ahead in the code and basically plan out the movements. Essentially, the machine “learns” the toolpath instead of simply reading it.
If the controller can’t keep up with the code, the machine will end up hesitating and you won’t be going anywhere near as fast as you programmed.
I’m not saying that HSM is impossible without a solid controller speed and a good amount of look ahead, but it sure won’t be easy.
RPM and Torque that Match the Material
A high performance aluminum profiler is very different from a high performance titanium machining center. You need to leverage the right machine against the right workpiece to get the best cycle times.
Here’s a reference of the what you’re doing vs what you need:
|Ti64 – Roughing||Low||Very High|
|Ti64 – Finishing||High||Low|
|7075 – Roughing||Very High||High|
|7075 – Finishing||Very High||Low|
|4340 – Roughing||High||High|
|4340 – Finishing||High||Low|
Basically, a 12,000 RPM machine with high torque won’t be a high performer with aluminum. If you need to really beat the competition, get the machine to match the material.
A Fast Machine
Ok, this might seem kinda obvious (high speed machining needs a machine that can move at high speeds) but let’s just go over what specifically the machine needs to do.
Obviously, the feed rate needs to be high. If your program is set to a higher feed rate than your machine is capable of, you’re not going to magically make the machine go faster.
But one common thing here is that the machine needs to change direction quickly. Since stopping or changing direction instantly isn’t physically possible, the machine needs to have a really responsive acceleration and deceleration.
So before deciding on a machine purchase, here’s something that I’d recommend doing to “test out” a potential machine to see if it’s suitable.
Design a a part that requires a lot of fast moves. Maybe something like a slot that changes direction in a tight zigzag or something. Ask the machine sellers to do a finish cut on this shape as quickly as possible while maintaining accuracy of 0.0005″.
If the move is complicated enough, you’ll probably see a fairly noticeable difference between a machine with a fast accel/decel and a machine that just not quick enough.
The reason that you should see it cut an actual part is that many machines have a “high speed mode” in which accuracy is sacrificed for speed. The machines move lightning fast, but I’ve seen them over/under shoot by 0.020″. This obviously will not help you for finishing passes.
Ultimately, HSM is becoming more of a norm than a specialty. Machines and tools are getting faster and better. In order to compete for production contracts, shops need to step up their game and push their equipment to deliver.
So does your shop do high speed machining?
It’s not something that needs to cost millions. A lot can be accomplished with a few new pieces of equipment, or even a simple change in approach. The main thing required is a shop culture that’s open to trying out a different way of doing things.
These are some of the basics of high speed machining, but this is by no means an exhaustive list. Other elements like high feed cutters, variable helix endmills, high performance tool coatings, coolant/lubrication delivery systems, insert geometry, and a dozen other things can all contribute to achieving high speed success.
Do you think that there’s anything worth adding? Does your shop do anything differently? Post it in the comments below.
What is High Efficiency Milling (HEM)?
High Efficiency Milling is a methodology that focuses on making the cutting tool work as efficiently as possible. Apparently HSM focuses too much on RPM and fast feeds, so HEM is all about maximizing Material Removal Rates (MRR). Essentially, it’s a term that people came up with to add to the preexisting pile of buzzwords in the precision machining industry.
It’s honestly not really all that different from HSM, and a lot of people use the term interchangeably. That’s what happens when people make up new acronyms to try and look smart. You get scholarly articles on the differences between HSM and HEM as they relate to MRR written by a B.S.PhD.
If you do a good job of HSM, there’s no need to distinguish it from HEM. Just get those cycle times down and good parts out the door.
What are some specific techniques of High Speed Machining?
Key techniques for high speed machining are chip thinning, high RPM achieved by harmonics testing, even tool load, peel milling (high axial depth of cut and low radial depth of cut that allow for high feed rates) and trochoidal milling (even tool load for complex toolpaths).