5 months by cncdivi
Why use a single flute end mill? Because they work better in some cases, that’s why!
BTW, sometimes these beasts are called o flute end mills or 1 flute end mills.
There are a lot of strange beasts out there in the cutting tool world, and a lot of physics that are not obvious. For example, many machinists will know that more flutes means more productivity, but that certain materials, like aluminum, require fewer flutes–usually a two or three flute end mill. If that’s the case, when would it ever make sense to use single flute end mills? Is there a time when the least number of flutes possible is a good idea?
In a word, “Yes!” Let’s talk about why.
The reason we use fewer flutes in some materials has to do with the behavior of chips in those materials. Simply put, aluminum creates bigger chips, all other things being equal. This has to do with the way the material curls as well as other factors.
The space created by the flutes of the endmill is where the chips have to go as they’re being cut. If there is not enough space relative to the volume of the chips, you’re going to have problems and may wind up with a broken cutter. Chip welding is one type of problem where the chips weld on to the cutting edge making it stop cutting.
Chip welding in aluminum…
To minimize these chip evacuation problems, we typically dial back the number of flutes for aluminum because it creates a larger volume of flute space to carry away the oversized chips. Single flute end mills have the best chip evacuation possible. The chip large flute valley on single flute end mills is what makes it so.
This productivity issue, where more flutes can be more productive, has to do with two factors: Material Removal Rates (MRR) and Surface Finish. One matters more to roughing (MRR) and one obviously matters more to your finish passes. This all has to do with what I’ll call the Tyranny of Surface Speed.
Let’s put aside this issue of flutes and talk about single point cutting on a lathe. It’s so simple, it helps shed light on what’s going on. For every material, there is a best surface speed that the manufacturer recommends. This recommendation largely has to do with spinning to the (or workpiece on the lathe) as fast as possible without harming tool life. The limiting factor is heat.
Tungsten Carbide will tolerate a lot more heat than High Speed Steel before it begins to soften. If the material your tool is made of softens, the tool’s sharp edge quickly dulls and your tool life is shot. So, you want the tool to handle as much heat as possible, and that’s why Carbide can often beat HSS. Since we can’t beat the speed limit, we have to fiddle with other factors when we’re up against it.
So, let’s assume you’re running the tool flat out in terms of Surface Speed. Any faster and it gets too hot, dulls, and it is finished. How else do we get higher material removal rates? The answer is we space out more cutting edges (flutes) around the circumference of the cutter so that as the cutter is spinning, we get a lot more bites (chips) of the material.
It’s now pretty obvious. At a given surface speed, a 4 flute end mill can take 4 cuts at a given chip load (chip thickness) while a 2 flute end mill only takes half as many. So the 4 flute end mill might have 2x the Material Removal Rate. This is why we see cutters with many flutes become popular in challenging materials that only allow fairly slow surface speeds. Using more flutes is how we get productivity back.
Now what about Surface Finish? I’ve been known to say using more flutes is like using a spindle speeder or having a faster spindle, except it’s even better because you don’t up the surface speed and compromise tool life with high temperatures the way a speeder would.
Other than the tendency to run hotter due to surface speed issues, the material doesn’t know the difference between being cut twice a revolution by a two flute end mill at 6000 rpm or 4 times by a four flute end mill at 3000 rpm. Hence, switching from a two flute to a four flute is like doubling your spindle speed.
When we increase speed relative to chip load, we improve surface finish (at least until it starts rubbing, see below). If you think back to why we had to use a two flute–to create chip clearance, you can start to see that on cuts where the cutter isn’t shrouded in material, you could even use a four flute in aluminum. For example, if you are peripheral milling the outside of a part and there are no concave indentations, let ‘er rip.
Are you becoming even more convinced there can never be a good case for single flute end mills?
Well, then it’s time to delve into times when they make the best sense. To do that, we have to consider the phenomenon of rubbing when chip loads get too low. You can read more about it in our feeds and speeds tutorial, but suffice it to say that if you move the tool too slowly, eventually the chips are so thin relative to the cutting edge, that it is unable to cleanly slice them off. It plows at them and can even skate along for a couple revolutions before it manages to pull out a rough dirt clod of a chip.
Now let’s take a CNC Router example. Say it’s got a spindle capable of 24,000 rpm, but it will go no slower than 12,000 rpm. When cutting aluminum, the first thing we discover is we need carbide to run at those surface speeds–preferably a good coating is needed to up the limit even more. As we begin working through the feeds and speeds (hopefully using G-Wizard Calculator!), we discover we’re going to need some pretty high feedrates at those rpms too. For a 1/4″ endmill, it wants to run at 24000 rpm and a feedrate of about 255 IPM. Now depending on the machine, we may have discovered a problem. What do we do if our machine can’t feed that fast?
The answer is to use a single flute endmill because it halves the necessary feedrates without rubbing. So there is one case where it helps, when the machine just can’t feed fast enough to keep up with what the spindle is putting out and maintain adequate chip loads.
Here is the other case: Whenever the extra chip clearance is of benefit.
There are lots of chip clearance challenging scenarios out there:
– You’re cutting really gummy cast aluminum plate. Definitely go to 2 flutes instead of 3, but you may find you have to go all the way down to a single flute.
– Micro-cutters have terrible geometry compared to larger cutters, it’s just life in the world they live in. You can only make the cutting edge so sharp, and at micro-scale it isn’t sharp enough. So the flutes are beating their way through the material like a cold chisel and 5 pound sledge instead of cleanly slicing. The tendency to chip welding is much higher and chip clearance is problematic when micromachining. Switch to single flute. Datron has been recommending this for roughing for a long time and even makes special singles flutes with a geometry allowing them to be balanced for high rpms.
– You’ve got to cut a brutally deep slot or small deep pocket and it is extremely hard to pull the chips up out of the hole. They are just hanging out down there clogging up the works. Ideally, you’d try through spindle coolant, but failing that, give single flute endmills a chance.
– You’re doing deep relief 3D profiling where the cutter is dropping into a lot of narrow spaces without much clearance.
Okay, that’s two good cases for single flute end mills, and we’ll end on a third: Some materials just come out better with single flutes. Typically, these are softer materials that are easily scratched. Making it easier for chips to get out of the way so they don’t go back in and scratch things up is a good idea.
Many plastics fall into this category, although a two flute will polish some plastics. A lot of wood products will also benefit from a single flute cutter. Soft woods and MDF comes to mind.
Any cutting of stacked sheets can sometimes benefit from a single flute cutter as well. These differences are typically not very profound, and usually will only come to light at higher rpms.
There you have it. A bunch of information to help you decide when it makes sense to use a single flute cutter.
On my visit with Datron, I learned they recommend single flute endmills for many applications. Fewer flutes means less chip recutting and the finishes just come out better. I walked away from the demo with a mirror finish mold part straight off the machine that sure made me a believer!
Since then, Datron has started recommending our G-Wizard Feeds and Speeds Calculator to their customers. If you haven’t tried it yourself, check out our Free 30-Day Trial.
Frequently Asked Questions (FAQ)
For applications requiring fast, high-volume material removal, the single flute can provide the best chip evacuation. These tools are perfect for aluminum, brass, plastics, composites, and any soft metals.
You want as many flutes as will be successful with the material at hand and which your machine can keep up with feedrates for. The widely accepted rule of thumb was to use 2 or 3 flutes for machining aluminum and non-ferrous materials and 4 flutes for machining steel and harder alloys.
To provide maximum chip evacuation in difficult situations--for example, when cutting grooves or slots in aluminum or other non-ferrous metals. Or to prevent chip recutting in plastics so they're not scratched.
They can be, depending on the material. In general, multi flute end mills provide much better surface finish and allow you to increase your feedrate. The more flutes you add the better your finish, and the stronger the core strength, but the harder it is to eject a chip.
The difficulty of ejecting the chip is where more flutes may not be better. In aluminum and non-ferrous metals, you can't use more than 3 flutes. In plastics, recutting chips can scratch up the plastic, so the fewer the flutes, the less likely you'll be recutting.
Like what you read on CNCCookbook?
Join 100,000+ CNC'ers! Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:
- Our Big List of over 200 CNC Tips and Techniques
- Our Free GCode Programming Basics Course
- And more!
Just enter your name and email address below:
100% Privacy: We will never Spam you!
Bob is responsible for the development and implementation of the popular G-Wizard CNC Software. Bob is also the founder of CNCCookbook, the largest CNC-related blog on the Internet.