7 Biggest Feeds and Speeds Mistakes CNC’ers Make
These 7 mistakes are things I hear over and over again talking to CNC’ers. There are some better ways and some better answers that can really improve your Feeds and Speeds practices if you’re open to them. Fixing your Feeds and Speeds is one of the easiest productivity hacks you’ll ever make. Not to mention it’s nice not to be dodging broken cutters all the time, LOL.
Assuming Feeds and Speeds Can Solve All Problems
Don’t get sucker punched assuming Feeds and Speeds cure all problems!
When I hear from folks who are breaking tools, they almost always assume it’s the result of bad feeds and speeds. In fact, if they use our G-Wizard software (ok, or some other calculator), they’re often irate about it–“Why is your darned software breaking so many of my cutters?”
It turns out the problem for these folks is seldom Feeds and Speeds. They’ve assumed that since their end mills are snapping right and left, it must be a Feeds and Speeds problem, but the truth is, Feeds and Speeds are just one part of the puzzle, albeit an important part.
When I work with folks having this sort of trouble, I check the feeds and speeds first. Sometimes they have a wrong setting in G-Wizard or they’re ignoring something it’s trying to tell them (like red tool deflection warnings), but usually it is something else happening.
Here are the most common problems I’ve come across that are not Feeds and Speeds issues:
- Failure to use some form of lubricant when cutting aluminum. This is probably the #1 error, and with the advent of inexpensive router-style CNC machines, it has become extremely common. Folks, aluminum has an affinity for the cutting edge of your endmills. It literally wants to chemically bond or weld itself to that edge. Once it does, tool breakage is inevitable. The best way to prevent this is to use some form of lubricant–flood coolant or mist being the best choices. Even spritzing the cutter every now and then with a can of WD-40 will work. If you can’t lubricate, you need to find a way to clear chips immediately from the cut and avoid much depth of cut at all. Even then, chip welding is a ticking time bomb.
- The second most common error I run into with beginners is excessive runout. Heck, it’s even happened to me–I broke 5 1/8″ endmills in quick succession as I trial and errored my way to finding that I had a bad ER32 collet. DOH! Runout is additive to chip load, and too much chip load is what breaks endmills suddenly. Runout is always present, it’s just a question of degree. It is in your spindle, tool holder, and collets. You can get a handle on it by measuring it very easily. Dealing with it ranges from easy (replace that bad collet) to difficult (get a spindle or machine with less runout). The smaller the cutter, the less tolerance for runout it will have. And unfortunately, the less expensive the CNC machine and tooling the more runout is likely to be hiding there. Tiny cutters and cheap CNC are a perfect storm.
- Using too many flutes in a material like aluminum. Aluminum requires fewer flutes because it produces bigger chips that curl in a way that takes up a lot of space. It needs more space between the flutes of your endmill and endmills with fewer flutes have more space. Stick to 2 and 3 flute endmills unless you really know the sneaky ways to cheat on that rule.
- Splintering and Tearout in materials like Plywood. Splintering and Tearout are reduced by proper speeds and feeds, but that’s not nearly the whole ballgame. There are also special cnc router bits for minimizing splintering and many tips and techniques. See our article on minimizing splintering and tearout for what is practically a bible on cnc machining plywood.
If you’re consistently having trouble, move past your first assumption and check on these other things.
Thinking Slower is Safer
When we want to be safe, we instinctively slow down the machine. It’s just human nature. Gotta make that loud noise less loud and everything will be okay, right?
Not so fast!
It turns out that going slower can actually be the least safe thing you can do in terms of tool life. There’s some sneaky geometry going on that will mess you up if you don’t know about it.
A slower feedrate for a given rpm results in a lower chip load. That’s fine, to a point. But you can get to a point where the chip load is so low that the cutter can’t efficiently make a chip. Instead it starts to rub or burnish the material instead of slicing off chips cleanly. We can see geometrically how this happens with the following diagram:
Cutter at top can slice off chips, cutter at bottom is “rubbing” them off…
Imagine the cutting edge is actually rounded rather than ending in a sharp point–they are if you look at them under magnification. If the top of the material lines up above the centerline of the cutting edge, all is well, the edge can get under the material to slice off a chip. But if it is below that centerline, then the cutter is spending more time pressing down than slicing up. It plows along the surface trying to rub a chip off. This produces tremendous heat which will in turn dull the cutter and make the problem worse.
How can you tell what the minimum speed is you should allow? It’s not easy, but we’ve done the research here and our G-Wizard Calculator will give you a rubbing warning. If you don’t have G-Wizard, start worrying about rubbing if your cut depth is less than the cutter’s chipload.
Let’s take the alternative. We’re charging along in the cut and all of a sudden there’s a noise. Suppose we reduce the spindle rpm without reducing the feedrate? Very bad idea–reducing rpm at the same feedrate kicks up the chip load and will likely break your cutter. Always reduce feedrate first!
Here’s one more example. We enter the cut, perhaps it’s a nasty parting off cut on a lathe, and suddenly there’s loud chatter. Again, our instinct is to slow down. But chatter is a resonant vibration. It’s just as likely to stop if you speed up as slow down because you’re changing the frequency in either case–so be sure to give both a try. Chatter is actually very manageable if you understand a little bit about how it operates. The chapter on Chatter from our Free Feeds and Speeds Tutorial will give you the tools you need to tame Chatter very quickly.
Ignoring Cut Depth and Cut Width in Favor of Feeds and Speeds
HSM Toolpaths like this Trochoidal Milling Tool Path are particularly sensitive to optimizing Cut Depth and Cut Width…
Did you know that an awful lot of what’s going to happen to your cutter is decided by the Cut Width and Cut Depth you choose? Taken together, the two are huge determiners of how well chips can be cleared. Our ability (or inability for deep cuts) to clear chips determines how much we have to slow down the cut from the optimum values we might otherwise choose. Modern HSM Toolpaths are also highly sensitive to optimizing Cut Depth and Cut Width.
So we should minimize both and radically increase feedrates, right? Not so fast! There are pros and cons on both sides–let’s look at the pros of increasing cut depth or cut width.
Deeper cut depth makes chip clearance harder, but it spreads wear over more of the flute length which can be critical for tool life. It reduces wasted motion as we step down over and over to reach the full depth of a pocket. That’s all good, right? But, a Deeper Cut Depth can make it harder to pull the chips up and out of the hole. So the deeper we go, the more we slow down to help get the chips out.
Now more Cut Width removes material faster, but it also makes it harder to clear the chips. Worst case is drilling a hole–chips can only go up and out to escape. The less Cut Width we have, the more circumference of the cutter is open to air, and the chips can be flung out that way.
However, if we use too little Cut Width, we encounter a phenomenon called “Radial Chip Thinning.” It makes us move the cutter faster than expected to achieve a target chip load because the geometry of small cut widths results in smaller chips in an odd way (explained more fully in our Free Feeds and Speeds Course).
There’s a lot more at work than the factors I’ve mentioned. When you choose a Cut Depth and Cut Width you’re locking down a number of trade offs and constraints on the Feeds and Speeds that you’re probably unaware of. The game is all but won or lost by the right choice, yet most CNC’ers are not choosing their Cut Depth and Cut Width in any particularly scientific way. They may use very fancy tools to choose Feeds and Speeds, but if the Cut Depth and Cut Width aren’t similarly optimized, you’re wasting your time–you simply get can’t the best results.
Simple rules of thumb can’t capture such nuance, but our G-Wizard software has 2 different tools that make it easy to choose good values for Cut Depth and Cut Width so the rest of your Feeds and Speeds calculations will be singing in 3 part harmony. My favorite is CADCAM Wizards because it is so quick and easy. It asks very few questions and returns a complete Roughing and Finishing Feeds and Speeds Recipe for all common CAM operations (hence the name CADCAM Wizards).
Here’s a video that shows how they work:
CADCAM Wizards work their magic by testing hundreds of combinations against the G-Wizard Cutting Physics Engine to determine the best set of trade offs for the holistic cut recipe. That’s not something you can do in a spreadsheet or with your yellow pad and scientific calculator, particularly not as quickly and easily as CADCAM Wizards does the job.
Treating Feeds and Speeds as Tables or Databases
Speaking of CAM, yellow pads, spreadsheets, and scientific calculators, I run across so many CAM programs and CNC’ers who want to view Feeds and Speeds as tables or databases. I guess they’re so used to seeing tables in tooling catalogs that it seems like the right way to think about Feeds and Speeds, but it is absolutely one of the worst ways to think about it.
Here’s the thing–the physics of Feeds and Speeds are much more complicated than any simple set of tables can express. But tooling manufacturers have to tell you something, and at least until recently, they felt they had to tell you something in a paper tooling catalog. So they over simplified it, boiled it down to tables, and hoped for the best.
The problem is the tables can’t accurately reflect the whole story. You can see clear as day that they know they’re not telling the whole story when they provide a range of answers. I’m looking at a catalog right now that says the Surface Speed (SFM) range for Aluminum with their endmills should be 500 – 1000 SFM. Nowhere does it say how I’m supposed to decide which one it is, yet that’s a 2x range. They can’t be more precise than that because tables can’t account for enough variables to be very precise. We see something similar with chip loads.
If you think about it, each table is 2 dimensional and therefore handles 2 variables. G-Wizard considers over 50 variables as it’s making Feeds and Speeds Calculations. Every single one of them impacts the outcome. How many variables are you considering? The average table is good for 2 variables. If you’re cranking the data through a sophisticated Excel spreadsheet, you might pick up a few more. But what’s the effect of the ones you’re still missing? It’s huge!
Then there’s the CAM table approach. Most CAM software wants to create a database of feeds and speeds that have worked in the past. The results look just like tables because that’s all a database is–electronic tables.
In this case, you’ve got tables that typically account for Tool Type and Material, and they’ll tell you the Cut Width, Cut Depth, Feeds, and Speeds that have worked in the past. Great!
- How sure are you that they’ll work in the future? BTW, these tables don’t account for chatter, which can come and go based on factors the tables don’t capture. The exact type of toolholder and stickout of the tool matter hugely. So does the exact machine (not just the make and model) because every spindle’s bearings are preloaded and setup a little differently.
- What about all the variables associated with each machine? What if you have more than one kind of machine in your shop? Tables are again, quite limited for dealing with this situation.
- What about deflection (you’ll hear more about it below), which I call, “The Silent Tool Killer.” Most of the time machinists are unaware of deflection unless they use a feeds and speeds calculator (not tables!). The tables typically don’t capture it. Suppose you’re using someone else’s tables, even someone else in your shop. How do you know the values don’t result in deflection that’ll kill 25% of your tool life needlessly? Unless you plug it into a calculator to double check, you’ll probably never know what’s going on.
You may want to try cutting speed formulas in a spreadsheet, but this isn’t much better. There are many pitfalls associated with the usual cutting speed formulas.
I could go on like this for ages. Good machinists don’t use tables or databases for their speeds and feeds. They use Feeds and Speeds calculators. And our customers have told us the reason why in straight up numbers.
Based on the feedback of our customers, the impact of using a Feeds and Speeds Calculator can be extremely large. They started out using these simpler methods and report large increases in their results with G-Wizard:
These are the kinds of results our customers tell us they get from G-Wizard…
Ignoring Tool Deflection
Tool Deflection: Silent Killer of Tools and Productivity?
It may be surprising to learn, but tool deflection may be the biggest silent killer of tools out there. Most CNC’ers are not even aware how much Tool Deflection they’re dealing with on a particular cut–you have to use a Feeds and Speeds Calculator that tells you this figure before you know. Once you do know it, you’re probably not real sure what it means or how much is too much.
Here’s a graph that shows the impact of tool runout as a percentage of chipload versus tool life:
Remember, runout (mentioned above) and deflection are additive. Now, a typical 1/8″ carbide endmill might have a total chipload allowance of 0.001″–a thousandth of an inch.
According to the chart, if the sum of runout and chipload is just 0.0005″, or 5 ten thousandths of an inch, we can reduce tool life by up to 40%. Pretty sensitive, eh? There’s not much margin for error. And just think, without a feeds and speeds calculator, most folks don’t even check the deflection.
Let me give you a couple of pointers on how to deal with Tool Deflection.
First, a good Feeds and Speeds Calculator like our G-Wizard will tell you exactly how much deflection you’re getting and it will warn you when there is too much.
Second, it will give you tools to deal with the problem of Deflection. G-Wizard has a Rigidity Calculator that can help you determine the effect on rigidity of tool diameter, stickout, and material (Carbide vs HSS). It has a Cut Optimizer that will tell you how much Cut Depth you can have for any given Cut Width and vice versa. And it has CADCAM Wizards, which will automatically run through hundreds of combinations to find the optimal pairing of Cut Width and Cut Depth for best efficiency. Here are some good pointers to help you learn more about these tools:
- 11 Feeds and Speeds Considerations for Lightweight CNC Routers: Has an awesome discussion of the Rigidity Calculator and uses it to show how to choose sturdier cutters for your job.
- Tool Deflection Sourcebook: Everything you ever wanted to know about Tool Deflection and more in this in-depth article.
- 2 Tools for Calculating Cut Depth and Cut Width: Nice easy walk-through of how to use Cut Optimizer and CADCAM Wizards.
Check these articles out, and remember, you can’t get tools like these anywhere else but CNCCookbook’s G-Wizard Calculator.
Not Taking Advantage of all the Great Tips Out There
In school, they teach feeds and speeds as a set of simple formulas–here’s how to calculate rpm from surface speed and tool diameter. Here’s how you calculate chip load. If you’re lucky, they get past those few basic formulas we can find anywhere (like Wikipedia) and on into the next level of detail. That next level of detail boils down to adjustments that have to be made to the formulas so they reflect reality, rather than the ideal that is theory. For example, if the Cut Width is less than half the tool diameter, you must adjust the feedrate to account for radial chip thinning.
That next level of minutia adds a couple of dozen additional formulas you must apply and a bunch of new variables. For graduate level work, perhaps they’ll get into the next level of complexity which will involve optimizing some of these variables relative to one another, something G-Wizard does extremely well that is unique in the Feeds and Speeds world.
But there is yet one more level of knowledge to be had. Once we understand how all those different variables and formulas interact (or once we let our Feeds and Speeds Calculator worry about that), we come to realize that the world of Feeds and Speeds is far from uniform. It’s a tangled landscape with many interesting cul de sacs, side streets, and neighborhoods. We talked about the rubbing phenomenon above. That’s one interesting neighborhood, the one you reach if you allow chip load to fall too low relative to the tool’s sharpness. There are many more. Here are some examples:
- Above a certain threshold of Cut Width, it is advantageous to switch from Climb Milling to Conventional Milling. It turns out that while most CNC’ers always Climb Mill, they’re missing out on cases where Conventional Milling actually results in superior geometry. The reasons are vaguely similar to those that cause Chip Thinning.
- Drilling Deep Holes, where depth is measured in tool diameters, can be something of a Black Art. There are a variety of little neighborhoods where one technique works better than another–peck drilling, parabolic flutes, how far to retract, how often to retract, and so on, all play a role.
- You can substantially change the rules if you can introduce High Pressure Coolant, and especially Through Spindle Coolant.
- Even just precisely aiming the Coolant using a Programmable Coolant Nozzle can afford you advantage.
- How your spindle’s power curve matches up to the rpm and surface speed trade offs of your tool and material combination matter. The point of maximum material removal may not be the ideal point for the tool. Instead, it might be shifted towards the place where your spindle makes maximum power.
- There are peculiar combinations of soft material and spindle limitations where HSS can actually remove more material than carbide.
I can go on like this for some time. There are literally hundreds of these little nuggets out there, waiting for a CNC’er to discover and take advantage of. You see them in tooling catalogs which mention dozens of them. Others you have to discover for yourself by experimenting with combinations. Some are so subtle, you’d never find them unless you have help from software that’s trying devilishly hard to maximize the combinations.
When I first started the journey that resulted in G-Wizard, one of my biggest challenges was trying to figure out how I would remember all of these helpful little rules. There were so many of them, and every time I opened a Tooling Catalog, more would spill out. I finally gave up and decided I wanted software to remember these things for me. It should tell me the best hints and tips once it saw which neighborhood I was in by virtue of the parameters I entered. That’s how G-Wizard’s Tips feature was born.
Take advantage of all those nuggets. Leaf through the technical sections of your Tooling Catalogs–that’s what they are there for. Or get a Digital Assistant like G-Wizard that will remember them for you and remind when they’re applicable. I’ve gone through some 250 tooling catalogs now, combing them for such tips to add to G-Wizard. I still get excited to go through the next one I get my hands on too!
Choosing “Good Enough” Feeds and Speeds
Come on, is that really good enough for your fireworks celebration?
A lot of folks figure what they’re doing for Feeds and Speeds is good enough. After all, you’re not breaking too many tools, you’re making money on machining jobs, and the cut sounds good, isn’t that enough?
Typically only the Beginners step up with a desire to solve the problem well because they don’t already have a solution they perceive is working. But the Beginners will have their only flavor of Good Enough that comes in the form of insistence on free tools. For Experts to change what they’re doing they either have to be that rare highly competitive breed who are always thirsty for more advantage, or they have to be handed a job with new materials or tooling they’re unfamiliar with.
But here’s the thing–it’s really not hard to do better and the benefits of doing better can be quite large for almost any CNC’er. We’ve traveled through some of the less traveled Feeds and Speeds roads in the discussion above. I hope you can see there’s probably a lot you’re not considering if you don’t use a sophisticated Feeds and Speeds Calculator.
Spreadsheets and Tables don’t do enough. They can seriously reduce tool breakage, but that leaves a lot of room for further valuable improvements. If you’re getting half the tool life that’s possible (and that our customers tell us was the typical improvement they got), you probably don’t notice it. Tools go for quite a while before breaking, BUT THEY COULD GO A LOT FURTHER STILL!
If your surface finish is decent, you probably don’t think about it. Yet, if you could improve it, you might save a lot of time by reducing the amount of work that happens after the part comes off the machine. Then there is your time spent, whether on a job that takes longer than it should, or time spent wrestling with handbooks, tooling catalogs, calculators and spreadsheets. Time that could be put to better use.
I have folks tell me they don’t need anything better because they can hear good feeds and speeds. You can hear really really bad feeds and speeds, but you can’t hear good feeds and speeds. The range of combinations your ear will tell you is a good one is much larger than the optimal combinations. If you could hear good feeds and speeds, you could buy ear training CD’s and companies like Boeing would make all their machinists listen to them. You’d have to take an ear test to get a good job. But none of that exists.
Hobbyists frequently tell me they can’t afford a tool like G-Wizard. They’ve purchased or built a machine for at least $1000 and probably a lot more. They’re buying cutters for that machine and the average price of a cutter is a significant fraction of a 1 year subscription to G-Wizard (good for a 1 HP spindle for life!). If they save even one cutter during the course of that year from an untimely demise, they’ve mostly paid for it. And they’re certainly the ones most likely to be breaking cutters and most in need of help. Did you learn everything you needed to know and broke only 1 cutter in the process?
They feel time is free and not something they should try to save. Yet, they have many projects they’d like to get made and not enough time to do them all.
For Pros and Hobbyists alike, improving your Feeds and Speeds is one of the cheapest and easiest productivity hacks you can make.
Bonus Mistake: Thinking You Can Tune Feeds and Speeds By Ear
Can you hear good feeds and speeds?
Oh if only it were that easy!
Many Old School machinists claim you can hear when feeds and speeds are right, but here’s the reality:
You can only hear really bad feeds and speeds, and then only sometimes.
What’s that mean?
Well, if the cut sounds bad it almost certainly is. But if it sounds good, it may easily be quite bad. The problem is that there are a host of factors that don’t really make any distinctive sounds. Too much deflection can radically shorten the life of a tool long before it affects the sound of a cut very much. Same with runout.
Too little chipload causes rubbing, which again is bad for tool life, and it makes little or no sound.
Mediocre speeds and feeds leave a lot of money and tool life on the table, but they don’t sound appreciably different than really excellent feeds and speeds.
I could go on, but perhaps a little thought experiment would serve better. Think about what would happen if you could hear feeds and speeds. If it was true, you’d be able to buy CD sets designed to “ear train” machinists. They’d play examples of good cuts and bad cuts. Major manufacturers would give all incoming machinists special feeds and speeds hearing tests. Because, why hire someone who can’t hear the difference between good and bad feeds and speeds?
The reality is you can’t buy machinist’s ear training CD’s and shops aren’t testing machinist’s hearing that way.
There you have it: 7 common feeds and speeds mistakes plus an 8th bonus mistake. Avoid them and you’re on your way to better feeds and speeds. And the good news is now that you know what they are, they’re easy to avoid!
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!
Recently updated on August 18th, 2023 at 04:10 pm
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.