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

The 12 Secrets of Machining Tough Materials on Small CNC Machines

Sep 9, 2015   //   by Bob Warfield   //   Beginner, Blog, FeedsSpeeds, Software, Techniques  //  No Comments

Machining difficult materials like Titanium and Stainless Steel is a scary business if you own a smaller CNC machine.  Even doing aluminum versus plastics and woods can be daunting.  Our article on machining aluminum for CNC Routers is one of the most popular we’ve ever done, for that reason.  But here is the surprising thing:

Provided your machine will achieve the correct feeds and speeds, you can successfully machine most any material you want.

I don’t say that lightly, and I will hasten to add that it isn’t just about feeds and speeds and that getting to the correct feeds and speeds may not be enough.  I should also add that successfully machining the material does not mean you’ll achieve the accuracy or surface finish of a high end Vertical Machining Center.  But, you can machine the material and you can get surprisingly good results.


The answer is that despite the fact you have a small machine rather than a full VMC, you still get to use some of the same tooling as that VMC.  You can pop a premium endmill into your machine and cut with it.  That’s not the whole battle, but it is hugely helpful.  The tool has the hard job–it’s stuck between your machine and that nasty tough material.  But, with proper feeds and speeds, the tool is already feeling more up to the task.  You’ve eliminated a big part of what’s different about your small machine and that VMC.  Keep minimizing those differences from the cutter’s perspective, and you’ll be doing well in no time.

Here’s what you need to do to be successful machining tough materials:

Start With a Decent Cutter Intended for Light Cuts

Like I said above, you can use the same cutters (barring not using cutters that are too big and aggressive) in your small machine as one can use with a VMC.  Buy a decent brand of carbide endmill.  It doesn’t need the ultimate solid green unobtanium coating, but make it carbide for rigidity and toughness.  A decent brand will have a little better geometry than a no-name.  You don’t want discount no-name cutters trying to bite into your difficult material–they’re not up to the job.

Another thing, use cutters intended for light cuts.  This is not so much an issue for endmills, but when looking at indexable tooling, you want the sharpest possible inserts.  In all likelihood, you may not even want indexable tooling for mills, but it works fine on small lathes.  On a light mill, forget a big (3″ is BIG for these machines) facemill with 6 inserts.  Try a flycutter or a smaller facemill.

For roughing, instead of a fancy indexable endmill, try a corncob (serrated rougher).  These work great on lighter machines if your machine will take one of a decent size.

Corncob roughers can be work well on small machines…

One really nice feature of these cutters is the serrations result in smaller chips, which makes it easier to keep the chips clear (see below).

Make Sure You Have Proper Feeds and Speeds and Run Them

One of the reasons difficult materials are difficult is they have smaller feeds and speeds sweet spots.  I have people ask all the time about listing more woods due to differences in wood hardnesses.  The reality is that not even the cutter makers deal with those differences because carbide is so much tougher than any wood that the differences do not matter.  You need a few categories to deal with other differences, but in general, Wood has a big sweet spot.  Plastics have big sweet spots.  Aluminum and Brass, easily machined metals, have big sweet spots.  Titanium and Stainless, not so much.

You can only hit those smaller more difficult sweet spots by having good Feeds and Speeds.  And here’s the thing–you are only going to get good feeds and speeds with a calculator.  You can’t hear the right feeds and speeds–if you could, there’d be CD’s you can buy and Boeing would make all their machinists train their ears with those CD’s.  You can hear when things are way wrong, but by then, that tough material has eaten the liver out of your tool.  It’s done and ready to pack up.

Plus, the conditions you’ll need to deal with the tough material, particularly on small machines, mean you need to deal with all the subtle nuances of calculating feeds and speeds.  For example, if you want to take lighter cuts, you had better account for chip thinning.  If you’re on a light machine, your Feeds and Speeds had better account for the shape of the machine’s Spindle Power Curve, lest it pick a range where the spindle is struggling without enough power.


Because of chip thinning, shallow cuts must be adjusted differently for Feeds and Speeds…

There is a long list of these things.  Our G-Wizard Feeds and Speeds Calculator considers more than 50 different variables in making its calculations.  You don’t want to try to mess with that yourself, even with a big Excel spreadsheet.

Start your cutter’s experience out right with good Feeds and Speeds that your machine is capable of achieving.

Deal With it When the Right Feeds and Speeds are Out of Your Machine’s Reach


The Feeds and Speeds Calculator must know your Machine’s Limits…

Another critical factor is that your machine be capable of achieving the desired Feeds and Speeds and that your calculator be capable of dealing with it when the ideal is unavailable.  This happens a lot with CNC Routers, perhaps especially on easy materials.  The reason is that the router’s spindle has very high rpm’s relative to the maximum feedrate available on the machine.

If we feed too slowly, the cutter plows along the surface, never digging deep enough to cleanly peel off a chip.  This is called rubbing.  If it happens on a tough material, the cutter gets very hot and will dull and then burn out quickly.  There’s a diagram below that shows the rubbing phenomenon better.  Another possibility is that your spindle is just too fast for the tough material.  This is one reason to use more premium tools.  A TiAlN coated carbide cutter actually prefers to be run warm.

You have to make sure the combination of your machine’s capabilities (min and max spindle rpm together with max feedrate) and the tooling’s capabilities mesh with the required feeds and speeds for the material.  You want a Feeds and Speeds Calculator that will warn you quickly when that’s not possible, and that can trade off various parameters successfully to turn a near miss of the sweet spot into a winning combination.  These are things G-Wizard excels at.

Sometimes, you just can’t get there from here.  The material’s properties are such that your machine won’t even get close.  For example, very hard materials are problematic for machines with very fast spindles in many cases.  If you can’t get there, you can’t get there, but there are a batch of useful tricks you can try that just might save the day.  We’ve put together an entire post about them that’s called, “What Now: My CNC Won’t Go Fast Enough or Slow Enough?”

What now?

Minimize Tool Deflection

Tool deflection is just plain bad!

Tools can deflect, and when they do it’s a bad thing.  We’ve often used the “bent endmill” as a logo device for this phenomenon.  Tool deflection is just plain bad for a number of reasons, including:

  • 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.

OK, we know deflection is bad and why, but what can we do about it?

First thing is to be able to tell when it is a risk.  Our G-Wizard Calculator will keep track of it for you and light up when it is too much:


Too much deflection shows up in Red in G-Wizard

Too much deflection shows up in Red in G-Wizard.  When you see that, you need to deal with it.

There are a lot of possible solutions, but in general, you can either change the tool setup or the cutting conditions.  Changing the tool setup might mean using a larger diameter tool or reducing tool stickout.  Changing the cutting conditions would mean reducing Cut Width or Cut Depth so there is not enough force to create excessive deflection.  G-Wizard has excellent tools to help you find the right Cut Depth and Cut Width that removes material well while minimizing tool deflection.  Once you’ve used them, you’ll wonder how you ever did without.

This stuff is particularly important with smaller machines because you’ll be using smaller cutters that are more prone to deflection.

Keep to the Fat Part of Your Spindle’s Power Curve

Have you ever stalled your machine’s spindle?  That leads to almost instant tool breakage.  Larger machines have automatic gear changes and fancy VFD’s that provide flatter power curves, but it is still important to pay attention to the shape of the power curve on them.  Small machines have few such luxuries so you really better have that power curve dialed in, or you had better seriously derate the power you think you’ve got on tap.  In fact, let’s talk about that business of derating right now:

Account for Machine Rigidity by Derating Your Power Curve

A really light machine has a lot of flex in its structure.  Machine deflection isn’t as bad as tool deflection, but it’s not good.  The thing is, deflection happens because we are applying enough force that it overcomes whatever rigidity the machine’s structure has available–so it moves.  Everything moves to a degree when we apply force.  Stick a Dial Test Indicator on a VMC spindle and chances are with a little leverage you can apply enough force to create a measurable deflection.  It’s just much harder to deflect the VMC than a small machine.

What that means is that if we reduce the force, we can reduce the deflection.  How much do we have to reduce it?  It turns out we can approximate that by looking at the relationship of work envelope (roughly, the size of the machine’s travels) versus its weight.  It’s an approximation, but it is a pretty good one.  The full details are discussed in our article, “What price machine rigidity?“, but what you need to know is that G-Wizard Calculator can automatically make this adjustment for small machines.

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

Use Decent Toolholders and Keep an Eye on Runout

Cutters generally fail in one of two ways:

  • If spun too fast relative to the material, they get too hot, they soften, they get dull very quickly, and they quit cutting.  This causes the chipload to rocket, which leads us to:
  • With too much chipload, they either can’t get rid of the chips and jam, or it just creates so much force it snaps the cutter.

I hate to see one of the poor little beasties lose its life this way.  Chipload kills faster than speed, and it is so much harder to stay on top of it.  Chipload is the thickness of the chips being peeled up.  Accurately calculating it is hard enough, but it gets worse.  You see, the actual chipload a cutter experiences is the sum of:

  • Chipload due to the cut.  This is the chipload we calculate in G-Wizard Calculator.
  • Chipload due to runout.
  • Chipload due to tool deflection.

Most machinists, especially beginners are totally focused on #1 and not even thinking about runout or deflection.  That’s why you can be bogeying along, making chips like a bandit, well within recommended chiploads, and all of a sudden PING!  There goes another cutter broken in half.  DOH!  I hate that.

Runout is somewhat relative to cutter size, if only because small cutters tolerate little chipload.  For the pro crowd, they say each 0.0001″ (one ten thousandth of an inch) of runout is worth 10% less tool life.  So 0.001″ of life should kill the cutter immediately, no?  Well, it may very well for small cutters.  I remember one day in the shop breaking 5 consecutive 1/8″ endmills due to runout.  First one I dialed down the feedrate.  Second one, I suspected something else.  Third one, I suspected my ER collet chuck and switched.  Fourth one, it broke again on a different chuck–time to put the DTI clock on it.  0.0014″ of runout–yuck!  That’s an awful lot.  No wonder EM’s were breaking.  Turned out it was due to a brand new ER collet from a name brand.  It came right out of the packaging with a runout defect.

Small machines, unfortunately, can have a fair amount of runout baked into the spindles and cheap toolholders.  Take an afternoon sometime, get out your 0.0001″ DTI, get a precision pin, and start checking runout on various toolholders, collets, and so on.  Clock the inside taper of your spindle to check its runout.  Know what you’re dealing with.  If it is too excessive, you may have to dial back chiploads to offset the problem.  You may identify a few “Bad Apple” collet chucks, collets, or other toolholders you can and should toss.

Use larger diameter tooling and avoid set scew style endmill holders for anything but 1/2″ and larger diameter cutters.  They have more runout.

Use Some Form of Coolant

Some materials require coolant, while some simply benefit from it.  Aluminum requires coolant, at least a mist, because it has a tendency to weld itself to the cutter.  Aluminum has an affinity for carbide, it seems.  The coolant in this case is acting as a lubricant.  Titanium and Stainless like coolant too, for different reasons.  Titanium doesn’t conduct heat very well, so the heat will tend to build up.  It’s hard to get it all to leave with the chips.  BTW, proper feeds and speeds will maximize the likelihood heat leaves with the chips–it’s just one more reason you have to have good feeds and speeds.  In the case of Stainless, good use of coolant will help reduce but not eliminate work hardening.  When you cut stainless, it wants to get harder, making it even harder to cut.

So use some form of liquid coolant, even as a mist, if you’re going after tough materials with an endmill.  Note that there is an issue called “Shock Cooling”.  The coolant can actually make matters worse for shock cooling.  The cutter gets real hot when making the chip, then it comes out and gets doused with cold coolant.  The shock of being alternately very hot and then cold creates small stress cracks which shorten tool life considerably.  The phenomenon is worse for indexable (tooling that uses inserts) tooling, it’s worse the hotter the tool gets, and it is worse the more of a single rotation the cutter is inside the cut where coolant can’t get to it.  Minimize all these things for better results.

Be Totally Paranoid About Keeping Chips Clear

This is something I tell people with small machines over and over again–you have to be totally paranoid about clearing chips.  Let’s consider stainless steel.  Each and every chip has become work hardened.  Imagine taking bits of carbide and scattering them over the cut so your tool is repeatedly slamming into those little landmines.  Work hardened isn’t quite that bad, but it is no picnic.  Recutting chips just makes your tool’s job harder than it has to be.  Whether you used an air blast, mist, or flood coolant, make sure you are successfully clearing chips as fast as they are being made.  Some things to think about:

  •  A dribble of flood may do much more poorly than a decent air blast.  If the chips sink to the bottom of a pool of flood, it takes a lot of pressure to get them back out of there.
  • Aim matters a lot.  Position the nozzle so it does the most good.  You will quickly see it takes multiple nozzles to do the most good no matter which way you are cutting.

There’s a reason why the inside of a good VMC looks like a high pressure car wash when it’s running–they understand the importance of clearing chips!

Maximize Setup Rigidity

You’ve got tool deflection under control, CHECK!  You’ve derated spindle power to account for machine rigidity, CHECK!  There’s no more flex left to worry about, right?


The workpiece and workholding may still flex, and that’s bad.  One could right a giant treatise about how to maximize workholding rigidity.  Cutting features with thin walls is a special world of pain all its own where chatter is near impossible to avoid.  But, there are things you can do to improve setup rigidity and they’re very important on small machines.  Fundamentally, they boil down to leaving as little of the part having out in the wind unsupported as possible.  This requires various measures to achieve, but here are some quick examples:

  • For plate work, think about vacuum fixtures, glues, and waxes that grab as much of the bottom surface of the plate as possible.
  • For vise work, figure out how to support the part properly.  It may help to use blocks to support parts not being machined:

Give that tall thin plate a little extra support…

  • On lathes, use a tailstock if the part sticks more than 3-4x its diameter out of the chuck.

This list could go on a long time, but you get the idea.

Take Light Cuts, But Not Too Light

Ah yes, all things in moderation.  Our first tendency with a small machine is to take lighter cuts.  I frequently hear beginners cry that they can’t believe their machine will survive the Feeds and Speeds G-Wizard recommends!  The truth is, G-Wizard is fairly conservative, but you may wish to dial it back even more.  The key is to figure out how to dial it back correctly.  If you simply take too light a cut, you will encourage rubbing.  The depth of cut is too shallow relative to the sharpness of the tool’s edge, so it ploughs along on top leaving a nasty surface finish, rubbing more than cutting, getting way too hot, and generally making its life much worse than a normal cut would’ve been.

If the cut isn’t deep enough relative to the cutter’s edge, you get rubbing and the tool burns up quickly…

G-Wizard’s answer is a thing we call the “Tortoise-Hare Slider:”


The Tortoise-Hare Slider…

“Full Hare” is what the tooling makers would recommend for roughing.  It’s more aggressive than settings to the left, but it isn’t really hare-raising (sorry!) levels of aggression.  I’ll be writing a separate post soon that tells how to do that.  For now, recognize that even on a small mill, full hare may be fine.  But if you want to back off, either because you’re seeing problems or because you want to start out easy, just move the slider towards the Tortoise.  It will do the appropriate things to improve tool life, improve surface finish, and avoid rubbing.  A special note–“Full Tortoise” is what G-Wizard determines is the slowest you should go without inducing rubbing.  It will result in the finest surface finish without rubbing, and is quite handy to have.

Derating your spindle power for machine rigidity will automatically result in lighter cuts as G-Wizard will have less horsepower to work with.  Lastly, on the Setup page you have a couple of controls to work with.  One will apply a fixed percentage to spindle rpm when feeds and speeds are calculated.  Perhaps you’d like to go for 90% of recommended to extend tool life.  There is a similar control to reduce feedrates.  All in all, I prefer the Tortoise Hare slider to fixed percentages, but you have multiple tools to choose from.

Enter the Cut Properly (Use Decent CAM!)

A lot of the worst damage to tools and tool life comes from how the cut is entered.  It can be very jarring to the tool if not done properly.  There are a few things to consider, but it all depends on what your CAM package can do for you.  It’s important to be aware of your CAM’s capabilities and if you are evaluating CAM, be sure to check for these things.

First, when milling, entry to cut out a pocket is typically done by plunging, ramping, or helixing into the cut.  The easiest thing on the cutter is helixing, followed by ramping, followed by plunging being the least desireable.  It all has to do with how long the cutter making how wide a cut and how much of the wear can be spread over the maximum flute length.  With plunging, only the bottom of the endmill cuts and the wear goes there all the way down the hole.  With ramping, you get a full width cut for as long a distance as it takes to ramp down to depth.  With a helix, you generally will open things up so the whole diameter isn’t cutting the soonest, and that’s why it is the most gentle approach.  Another thing to think about is coolant access and chip clearing.  Helixing, again, opens things up so you can clear chips and apply coolant that soonest.

One more to think about is using a twist drill to make a big enough hole to start a pocket.

Second, with work hardening materials like stainless, get down to depth as quickly as possible.  A shallow ramp or helix angle will give work hardening more opportunity.

Next, make sure your CAM has different feeds and speeds for entry versus the actual cutting.  Entry speeds must be slower!  Plunge speeds are typically a lot slower, while Ramping and Helixing are only slightly slower.  G-Wizard can figure the right Feeds and Speeds for all three, but it does no good if your CAM program won’t let you put them in.  Actually, that’s not quite true, you could use G-Wizard Editor to insert them at the proper place in the gcode if needed.

There are more CAM-related entry issues to consider.  If you’re going to face mill or profile an edge, you generally want to arc into the cut.  Going straight in is a bad idea.  Much more on this sort of thing is available in our Feeds and Speeds Course in the chapter on, “Toolpath Considerations.”

Be Patient!

I’m sure that’s a lot to digest, but cutting difficult materials requires some care.  The most important thing is to be patient.  I know of many folks who have produced outstanding results, even saleable products, out of tough materials like Stainless and Titanium.  It can’t be done as quickly as on a bigger machine, but it can be done quickly enough.  So be patient, learn the tricks, and pretty soon you’ll be getting results you hadn’t dreamed were even possible on your small CNC.  We’re here to do what we can to help.  We put out the information, and we offer Free Trials on our CNC Software so you can try it for yourself and see some of the things I’ve been talking about.


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

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.