CNC Cutting Speed, Surface Speed, and Spindle RPM
For our first chapter on feeds and speeds, I’m going to talk about spindle rpm or cutting speed and how to calculate it from surface speed.
The “Speeds” portion of the Feeds and Speeds combo refers to your spindle rpm. Determining the correct Speeds for a job is largely a question of determining how fast the tool can be spun without overheating it in the material you’re cutting.
Once a tool overheats, it softens (well short of melting), and this causes the sharp edge to dull. It doesn’t have to get very dull before the tool is done. If you keep going with a dull edge, you’re likely to break the tool, but you’ll see a very deteriorated surface finish before that happens.
There are some basic concepts and terms machinists use to discuss feeds and speeds that everyone should be familiar with.
In a series of experiments performed early on in machining, it was determined that your spindle speed is the biggest determiner of your tool’s life. Running too fast generates excess heat (there are others ways to generate heat too), which softens the tool and ultimately allows the edge to dull. We’ll talk more in our series about how to maximize tool life, but for now, consider your spindle speed to be largely about maximizing tool life.
“Feeds” refers to the feedrate, in some linear unit per minute (inches per minute or mm per minute depending on whether you’re using the Metric or Imperial system). Feedrate is all about the tradeoff between maximizing your material removal rate and being able to extract chips from the cut. Material removal rate is how fast in cubic units your mill is making chips–the faster the better for most machinists, right up until it creates problems. The most common problem is tool breakage or chipping when you feed too quickly. When that happens, the chips jam up in the flutes and pretty soon the cutter breaks.
I’m a Beginner, How About if I Just Run the Machine Super Slow?
It’s a common mis-conception that you can “baby” the cut in order to be ultra conservative. Just run the spindle speed way slow and the feedrate way slow and you won’t break anything, right? Well, not exactly. Metal is a very unforgiving material. Plastics, wood, and other softer materials can also have problems from improper feeds and speeds, but metal is the most sensitive.
Here’s some examples of what can happen if you run too slowly:
– If you reduce your spindle speed too much relative to the feedrate, you’re forcing the flutes of your cutter to take of too much material. The endmill is being pushed too fast into the cut and the chips get too big. You can easily break a cutter this way.
– If you reduce your feedrate too much relative to spindle speed, you will soon cause your cutter flutes to start “rubbing” or “burnishing” the workpiece instead of shearing or cutting chips. Many machinists will tell you the fastest way to dull a cutter is just to run it with the spindle reversed and make a pass, but having too slow a feedrate creates a similar effect. We’ll talk more about how this happens in the Feeds and Speeds article, but suffice it to say that running too slow is just as hard on your cutters as running them too fast, if not harder.
Okay, I Get It–There’s a Sweet Spot for Feeds and Speeds
Yes! That’s exactly right, there is a Sweet Spot for every cutting operation. It’s not a point that has to be hit exactly, but at the same time, it is not very large either, and there are penalties if you miss it completely. The more difficult the material you’re cutting, the smaller the sweet spot and the greater the penalties. Once you know where the Sweet Spot is, you can tweak your cutting parameters within that envelope to maximize Material Removal Rates, Surface Finish, or Tool Life. In fact, you can often maximize any two of the three, just not all three at once.
Let’s take a look at the sweet spots for different things, as well as the danger zones:
This chart is relative, meaning you can’t assume anything about the proportions or scale. Just look at the positions of the regions relative to one another, and relative to the idea of faster and slower spindle speeds and feedrates.
Let’s consider the different labeled zones, left to right, top to bottom:
Feeding too Much Chipload As we’ve discussed, when you feed too fast for a given spindle rpm, you’re likely to break the tool. The more you exceed the appropriate speed, the more likely. At some point, you’ll always break the tool. Consider the absurd case where spindle rpm is zero and you rapid the tool into the work. Pop! Just broke another tool.
MRR:Running the spindle as fast as we can without burning the tool, and feeding as fast as we can without breaking the tool is the sweet spot for maximum material removal rates. If you’re manufacturing, this is where you make money by getting further up and to the right than the competition.
Too Fast: Too much spindle speed will generate excess heat which softens the tool and dulls it faster. There are exceptions and mitigating circumstances we’ll talk about in more advanced installments.
Best Tool Life: Slowing down the spindle a bit and feeding at slightly less than appropriate for maximum MRR gives the best tool life. We’ll talk more below about Taylor’s equations for tool life, but suffice it to say that reducing the spindle rpm is more important than reducing the feedrate, but both will help.
Surface Finish : Reducing your feedrates while keeping the spindle speed up lightens the chip load and leads to a nicer surface finish. There are limits, the biggest of which is that you’ll eventually lighten the feedrate too much, your tools will start to rub, and tool life will go way down due to the excess heat generated by the rubbing.
Older Machines:So your spindle speed has come way down, and in addition, so has your feedrate. You’re probably on an older machine where you can’t run the kind of speeds you need to take advantage of carbide tooling. You may need to switch to HSS. It comes as a surprise to many that there are areas of the feeds and speeds envelope where HSS can outperform carbide, but it’s true, depending on your machine’s capabilities and the material you’re cutting. Check the article “Is Carbide Always Faster than HSS” for more information.
Feeding Too Slow: As discussed, feeding too slow leads to rubbing instead of cutting, which can radically shorten your tool life and is to be avoided.
Now that you know how the sweet spots break down, you’ll have a better idea how to steer your feeds and speeds to the desired results.
Let’s get back to figuring your proper spindle rpm or cutting speed.
Surface Speed: How Fast the Tool Slides Against the Workpiece While Cutting
When specifying the operation of a tool, surface speed goes hand in hand with chip load. Just as chip load is a better way to talk about feedrate because it is independent of so many factors, surface speed is a better way to talk about spindle rpm. Imagine that instead of a rotating cylinder with cutting edges, your tool was a flat piece of metal slid against the workpiece. The recommended speed to slide when cutting is the surface speed. Here’s the visual:
Visualizing Surface Speed…
Surface speed is measured in linear units per minute: feet per minute (SFM) for Imperial, and meters per minute in Metric.
You can’t really cheat on Surface Speed. It is what it is and exceeding the manufacturer’s recommendations is sure to reduce tool life fairly drastically except for some very special HSM cases you should only worry about when you’ve mastered the beginner and intermediate speeds and feeds concepts.
The Interaction of Surface Speed and Spindle RPM
Consider this table which shows tool diameter versus surface speed at 10,000 rpm:
Surface Speed vs Diameter at 10,000 rpm…
If we keep rpms constant, Surface Speed is directly proportional to diameter. The 1/16″ endmill at the bottom is travelling 1/8 as fast in terms of Surface Speed as the 1/2″ endmill at top. Hence, to achieve a given Surface Speed, small tools will have to spin faster and large diameter tools will have to spin slower.