G-Wizard Calculator:
Fast, Easy, Reliable Feeds and Speeds


Join 50,000+ 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!


GCode is Complicated
G-Wizard Makes it Easy

15 Reasons Cutters Get Broken on Small Machines

Sep 21, 2015   //   by Bob Warfield   //   Blog, FeedsSpeeds, Manual, Techniques  //  5 Comments

Nobody likes breaking cutters, but beginners seem to dread it the most.  That little “tink”, the broken cutter tip flies across the room, and suddenly you’re unhappy.  I’ve helped out a lot of beginners here at CNCCookbook, and in particular, I’ve helped diagnose a lot of recurring problems.  A certain amount of it just goes with the territory–“I broke this cutter because your G-Wizard gave feeds and speeds that were too aggressive for my machine!”  I always try to run these cases to ground so that if there really is a problem with G-Wizard, I can recalibrate it.  I am happy to save, we haven’t traced a broken cutter problem to G-Wizard in a very long time (knock on wood!).  In fact, there are so many G-Wizard users, that I wouldn’t get much sleep if I did ship a version with a problem like that until I fixed it.

Feeds and Speeds can be an issue, and we’ll talk about the likely ways to get into trouble on a small machine with Feeds and Speeds, but there are a lot of other problems that come up.  If you’re breaking too many cutters, go through the list and see whether you can find some underlying problems that are easily cured.

Inadequate Lubrication

Certain materials require lubrication–no ifs, ands, buts or maybes!

Aluminum is an excellent example, and the endmill on the right is clogged with gooey aluminum.  If you’re cutting aluminum successfully without any form of lubrication, you’re leading a charmed life.  In all likelihood, you are running very shallow depths of cut on the aluminum and you have some way of getting rid of the chips before they come in contact with the cutter again.  I’ve seen this work for CNC Routers that have good vacuum chip evacuation, but it’s hard to ever cut very deep in aluminum without some form of lubrication.  The reason is that the aluminum wants to weld itself to your cutter.

It doesn’t take a lot–a mister may be the best solution if your machine is not in a proper enclosure.  I have seen people even stand by spritzing the cutter with WD40 at periodic intervals.  That can work, but it’s tedious and not very consistent.  The mister is better and they’re not that expensive.

Too Much Runout

Runout is a common problem for small machines.  The spindle and toolholder will each have some sort of runout component.  If the toolholder involves a collet, the collet will have its own runout.

Runout is nothing more than the tendency for the cutter to rotate a little off-center rather than exactly along its axis.  The problem with runout is it changes the chipload (thickness of chips being cut) and forces the flutes on the part of the revolution that sticks out to do more than their share of the work.  Having fewer flutes on the cutter doing a lot more work than you intended is obviously a great way to stress out and ultimately break the cutter.

Less expensive machines and toolholders often have a lot more runout than you’d like.  Sometimes you can isolate it to a particular toolholder that wasn’t machined well and just needs to be junked.  Fortunately, it isn’t hard to measure runout.  We’ve written a number of articles about it that you can search for or click this link to track down.

Once you measure your runout, you’ll be wondering, “How much runout is too much?”  There’s no concise answer–it all adds up.  Think of runout as being added to the chipload of your cutter.  Whatever that recommended chipload may be (G-Wizard Feeds and Speeds Calculator will give you that), think of the Runout as a percentage of the chipload.  If it’s more than 5-10%, it’s probably causing you problems.

What can you do about runout if you have too much?

First thing is measure it for all your toolholders and get rid of the most egregious runout toolholders.  Sorry, I know they cost money, but they have quality problems and cutters are expensive too.  On a suspected bad toolholder, be sure to try it with several collets–it could be just the collet that needs replacing.

If you still don’t have runout under control, clean everything meticulously.  Chips and dust can add up to runout too.

Did all that and still not happy?  Well, you can still do a couple of things.  First, you could reduce the chipload you’re willing to run by an amount equal to the excess runout.  That’ll take care of breaking cutters and it isn’t hard to do if you use a Feeds and Speeds Calculator like G-Wizard.  Second, you may want to try “clocking” your toolholders.  This is the practice of rotating the toolholder in the spindle before tightening it so that the runout of the spindle and the toolholder partially counteract each other.  You’ll need a reference mark on the spindle and another on the toolholder to be able to do this well.  Mark the tool holder so that lining up the toolholder mark with the spindle mark yields minimum runout.

It’s kind of a pain to do this, but it will yield results and sometimes the small CNC Machines may make us work a little harder to get our best results.

Wrong Tool:  Too Many Flutes

Are you pocketing aluminum with 4 flutes?  That’s going to cause problems.  Aluminum chips wind up bigger than most other materials.  There isn’t enough room between flutes in a 4 flute cutter for the chips to escape, so they bind up, jam, and eventually break your cutter.  Use 2 or 3 flute cutters with aluminum, or even a single flute cutter.  Cast aluminum can cause more problems than wrought aluminum.  If it is too gummy and sticky, use fewer flutes.

Wrong Tool:  Plunging a Non-Center-Cutting Endmill

Not all endmills can cut at their very center.  The flutes have to go through the center of the tip.  If yours can’t and you plunge it straight down, it won’t get very far before it jams.

Improper Feeds and Speeds

Yep, you can definitely get into trouble with improper Feeds and Speeds.  You are using a Feeds and Speeds Calculator, right?  You do know you can’t actually hear proper feeds and speeds or feel them, despite what many old timers may claim?  Let’s assume you are using a Calculator.  You can still get into some trouble depending on the Calculator.  You’re unlikely to be going too fast if you used a Calculator properly, but beginners very often go too slow.

Come again?  How can going too slow get me into trouble?

Welcome to the wonderful world of Feeds and Speeds Sweet Spots, where you had better have dialed in that special Goldilocks “just write” combination of Feeds and Speeds.  Here’s the Sweet Spot diagram from our free Feeds and Speeds Course:


Too much or too little of either spindle rpms or feedrate leads to trouble.  In this case, slow feedrates can lead to rubbing because chiploads are too low.  Remember, the chipload is the thickness of the chip that the cutter slices off each time.  If that thickness is too small relative to the sharpness of the cutter’s edge, it can’t get under the chip to slice it off cleanly.  It rubs and scrapes it off, which generates a lot of heat and is hard on the tool.  Here’s a graphical diagram of what causes rubbing:

The bottom cutter is starting to rub–its edge can’t get under the chip to slice it of cleanly…

Fortunately, G-Wizard Calculator will warn you when you’re getting too close to rubbing territory.

Another way to get into trouble with a Feeds and Speeds Calculator is to give it too much information.  We’ve all had bosses that micro-manage us too much.  They want to control every little detail.  In G-Wizard, each time you override something it could calculate, it shows a little padlock:


The little padlock means G-Wizard can’t change this value…

If you get enough padlocks showing, G-Wizard is hamstrung–it no longer controls enough variables to find the best answers for you.  Beginners should probably try to steer clear of padlocking values until they understand enough about Feeds and Speeds to know when it is beneficial to take more control.

Not Paranoid Enough About Chip Clearing

After lubrication, the first thing I want to know when someone has a problem is how they’re clearing the chips.  You want to be extremely paranoid about chip clearing.  Imagine each chip is a little hardened carbide land mine just waiting to chip and damage your cutter.  If that were true, you’d work hard to get them out of there, wouldn’t you?

They seem so harmless, why not let them pile up and ignore them?  After all, they’ve already been sliced and diced to be small.  There are several problems:

  • The bigger the pile of chips the harder it is for new chips to get out of the way.  Why make your cutter fight to get chips out of the way?
  • If your material work hardens, the business about each chip being a hardened carbide land mine is closer to the truth than you might think.  You definitely want to clear chips from such materials as best you can.
  • With proper feeds and speeds, those chips are carrying away heat from the cut that can damage the cutter and also cause your material to grow from thermal expansion (bad for accuracy).  Getting them out of there helps get the heat out of there too.  You want your cutter to get cool clean air and possibly some coolant when it isn’t actually peeling off chips.  Hard for it to get that if it is up to its ears in old chips.
  • Those chips are going to bang and scrape around in the cut.  Imagine one getting caught between cutter and wall of cut.  All that is not just bad for the cutter, it’s also bad for the surface finish of your part.

So, repeat after me, “I will be totally paranoid about chip clearing!”

Now how to do that?

You need either flood coolant or mist/air that is strong enough to clear the chips.

You need to take care that the nozzle is aimed properly for the cut.

Higher pressure, higher volume, and more nozzles are all things that can help you to clear the chips better.

Machine Not Rigid Enough for Cut

Any machine will move if pushed–nothing is infinitely rigid.  But small machines are particularly flexible.  It’s hard for the cutter to do its job well if the machine is flexing all over the place.  Depending on which direction the cutting forces are pushing, a flexible machine might allow the cutter to be pushed into the wall of material forcing it to cut more deeply than expected.  This is common when Climb Milling, for example.  As you can imagine, when that happens, the cutter’s life is particularly difficult and it may break.

There is an answer to a lack of machine rigidity (apart from adding material to make the machine more rigid, of course).  We can derate the horsepower of the machine until the forces being generated relative to the rigidity of the machine are balanced to a more “normal” level.  This will minimize flex and let things proceed more smoothly.  G-Wizard Calculator can be set up to automatically perform horsepower derating based on machine rigidity.

Here is a video that discusses both the machine rigidity adjustments and the spindle power curve adjustments in G-Wizard:

Setup Not Rigid Enough for Cut

If the part slips because it isn’t being held tightly enough, chances are you will break a cutter.  It takes a certain amount of experience to know how to make your setups as rigid as possible, so be on the lookout for the tricks of the trade.

Cut Entry is Too Rough

When machining tough materials, sometimes just getting the cutter started into the cut is crucial.  Too rough an entry chips the cutter and things go downhill from there.  The gentlest entry will be a helical spiral, followed by ramping down, with a straight plunge being the toughest on the cutter.  Slow down the feeds and speeds during entry for tough materials too.

Stalled Spindle

If the power being absorbed by the cutter exceeds the power available from the spindle, you’ll stall the spindle.  This almost always results in a broken cutter since the machine has no idea the spindle stalled and keeps merrily feeding along.

To avoid stalling the spindle you’ll need to be sure to use Feeds and Speeds Calculations that factor your spindle power curve into the equation.  Most spindles, especially on smaller machines, have peaks and valleys.  The machine may say 3 HP in the specs, but you can be sure there are certain rpm ranges where the available power is much less.  With G-Wizard, it will automatically dial things back when you’re in one of those valleys and there is less spindle power available.

Part Zero is Wrong

CNC Machines are blind–they have no idea where you part is on the table.  So is your CAM software.  Both assume Part Zero, the coordinates 0, 0, 0 on a mill, are the same.  In other words, the CAM software expects its idea of Part Zero and how the part lines up relative to that point to be identical to how things are really setup on the machine.  But what if they aren’t?  You’ve got problems.

There are a variety of ways to set up Part Zero, just make sure you’re using one that works for you.  While you’re at it, make sure you’ve properly homed the machine when you started it up.

Tool Length Offset is Wrong

Tool Length Offset is much the same situation as Part Zero.  The Machine has no idea where the tip of the tool is other than what you tell it for the Tool Length Offset.  With multiple tools, you really should be setting up your Tool Table properly with these lengths.  Even if you touch off every single tool, make sure its done correctly.  If the tip is a half inch lower than the machine things, that cutter is not going to have a long and happy life.

Unknown Material

Professionals are often called on for what’s called “Traceability.”  They have to be able to prove that the material they made a part from is the material specified.  Hobbyists often scrounge material.  It gets hoarded, perhaps it is mismarked, perhaps we never really knew what we had in the bin–just a nice looking rod that’s clearly some sort of steel.  It was cheap, so we assume it is probably cheap steel–perhaps a mild steel of some kind.  We stick it on the machine and that’s where the trouble starts as we discover that despite doing everything we should, we’re suddenly breaking cutters.  Perhaps the material is harder than expected.  Perhaps that ordinary looking “mild” steel is really a nasty grade of stainless steel that work hardens if you just look at it funny.

If you encounter an unknown material, you can at least establish the broad category fairly successfully–is it steel?  Aluminum?  Brass?  And so on.  If it is steel but non-magnetic, it is very likely stainless steel. If it is cutting poorly, select a material in your Feeds and Speeds Calculator that’s from the same family but fairly hard.  Slow your rpms way down, and use a carbide cutter.

That will often get you through it.

Too Much Backlash

We’ve talked about Runout, Machine Rigidity, and Setup Rigidity as ways that unwanted motion can ruin a cut.  Backlash is another.  Always be aware of how much backlash your machine has.  Check it every few months or when there are signs of trouble.  The double nuts on your ballscrews may need adjustment.  For the right kind of cut (Climb Milling, anyone), the cutter can be sucked deeper into the cut by Backlash with predictably unhappy results.

Diagnosing and eliminating backlash can help you to minimize these issues.

Too Much Tool Deflection

I’ve saved one of the best ones for last–Tool Deflection.  If we apply force to the tool, it will bend, not as much as, but similar in spirit to this:

As mentioned with some of the other bending and flexing problems, the exact nature of the bend will vary, but it can cause the cutter to be pushed into a deeper cut against the wall of the material.  In addition, there are other bad side effects:

  • It is additive to chipload and runout and can break a tool in a hurry.  See below for more on that.
  • Ever bent the paper clip too many times until it broke?  Tool deflection does the same to an endmill.  Once per rpm it deflects in a particular direction.  That’s a lot of bending and it will shorten the life of the tool.
  • Deflection is like tapping the side of the endmill with a little hammer once a rotation.  Imagine the vibration that causes.  If it happens to resonate with the rest of what’s going on, you get what’s called “Chatter.”  Chatter ruins surface finish and destroys tool life.  If the tool doesn’t deflect, there can be no chatter.
  • Deflection means inaccuracy.  An endmill can’t cut accurately if it is deflected away from where the g-code expects it to be.
  • Surprising side effects.  I saw a case one time where deflection allowed a tiny wall to form when making a pocket that prevented coolant from getting into the cut.  The cutter broke not long after.

Tool deflection is manageable, especially if you use a Feeds and Speeds Calculator that’s set up to deal with it, like our G-Wizard Software.  The smaller the cutter diameter and the longer the cutter relative to that diameter, the more likely you’ll have tool deflection problems.  Fortunately, we have a great article that walks you through what to do about Tool Deflection.


Look, cutters are going to break from time to time.  But by looking into the various issues we’ve raised here, you can tremendously minimize the likelihood.  There are more tips available still for various specialized situations such as CNC Routers and Aluminum, Micro-Milling with very small cutters, or trying to cut difficult materials with a small CNC machine.

It’s all doable, and you’ll find that once you know the techniques, you don’t break very many cutters.



Like what you read on CNCCookbook?

Join 50,000+ 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:

Full Name
Email *
100% Privacy: We will never Spam you!

Rate this post


  • Seems to me that “This is common when Climb Milling” should refer to conventional milling instead. When you run into a 90 deg corner it pulls into the corner. Climb milling creates problems if the motors are too weak to hold back the cutter from pulling itself along the wall too fast, but at least it is pushing away from the finished part and may break the cutter without scrapping the part.

    • Ken, think of climb milling as if it is a pinch roller trying to push or pull along the workpiece. With climb, it pulls in the direction of travel. So if you are headed into a corner, it’s climb milling that will pull the cutter into the corner further than conventional.

      There’s a picture in this article that shows the force vectors:

      Climb pulls into the cut more deeply while conventional pushes back against the cut.

  • Another common event involving climb milling: A tall thin wall which needs the end cut will bend into the cutter if it is climb cut. Calassic positive feedback loop, the further it pulls the harder the next flute hits. Soon one or more things must break.

  • I was getting dramatically shorter life on my miniature carbide end mills (0.015” dia) during cold, dry winter months in my un-heated shop. I first thought the cold temperature was at fault – it was indirectly.

    One night I checked on a job running, but left the shop lights off. I noticed sparks coming off the end mill. It looked like a tiny sparkler. Was it dull? Nope. Static electricity!

    My mill is belt driven. There was a very high electrical resistance ( 6 megohm) between the spindle and the mill table. The tip of the EM became a spark gap for the static electricity generated by the belt. In effect, I had an EDM machine eating away my miniature end mills. Although they looked OK under magnification, I’m convinced the cutting edges were compromised.

    Luckily the static electricity never interfered with the stepper controller – all jobs ended with the mill back at zero positions.

    After adding a braded wire from the spindle housing to the table, the sparks disappeared and the EM life returned to normal.


    • Wow, Ed, fascinating story. I bet you were shocked to see those sparks and wondered what the heck?!??

Leave a comment


Do you want to be a better CNC'er?

Get Better Tool Life, Surface Finish, and Material Removal Rates.


Start Now, It's Free!



  GW Calculator

  GW Editor



  Deals and Steals

CNC Blog








     Feeds and Speeds

     G-Code Tutorial

     CNC Machining & Manufacturing

     DIY CNC Cookbook

     CNC Dictionary

CNC Projects


     Machinist's Search


     Online Groups


     Reference Data


     CNC Dictionary


     Tool Brands


     Hall of Fame

     Organization: Soon!





     Our History

     Privacy Policy

All material © 2016, CNCCookbook, Inc.