Categories

 

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

Subscribe

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!

 

GCode is Complicated
G-Wizard Makes it Easy

Why Use a Single Flute End Mill?

Dec 23, 2012   //   by Bob Warfield   //   Beginner, Blog, CNC Router, FeedsSpeeds, Techniques  //  4 Comments

when to use a single flute end millThere 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 two or three.  If that’s the case, when would it ever make sense to use a single flute end mill?  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.  Therefore, 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.

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 simply, 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 endmill can take 4 cuts at a given chipload (chip thickness) while a 2 flute only takes half as many.  So the 4 flute might have 2x the MRR.  This is why we see cutters with many flutes become popular in challenging materials that only allow fairly slow surface speeds.  That’s 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 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 at 6000 rpm or 4 times by a four flute 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 chipload, 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 a single flute?

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 chiploads 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 a long 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 neccessary 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 chiploads.

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.

Update, 7/16/2014

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.

 

 

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:

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

Why Use a Single Flute End Mill?
Rate this post

4 Comments

  • i know that certain material prefer certain # of flute to be used to rough out material. can someone tell me what is a good number of flute used to rough out 316 ss

  • At a previous employer we had many Single Lip Cutter Grinders and made many ball and bullet nose cutters for Mold work. The rigidity supplied by the minor diameter often out performed any bought cutter. As to heat, the single flute with extra rake and clearance but without a thin flute also dissipated heat well. The finishes were superb!

  • Great article! I don’t know what I’d do without a single flute in 3003 or 5052 aluminum. Two and three flutes have a tendency for chip welding. I can even run the single flutes dry!

  • Datron micro cutters are great. But you have to learn on the job. I’ve been using them over and 15 years and they offer no data to help with speeds and feeds. It’s a case of suck it and see. Once you find the sweet spot though, the longevity is fantastic

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!

Home

Software

  GW Calculator

  GW Editor

  Gearotic

  Conversational

  Deals and Steals

CNC Blog

  Software

  Techniques

  Beginner

  Cool

  Projects

 

Cookbooks

     Feeds and Speeds

     G-Code Tutorial

     CNC Machining & Manufacturing

     DIY CNC Cookbook

     CNC Dictionary

CNC Projects

Resources

     Machinist's Search

     Videos

     Online Groups

     Individuals

     Reference Data

     Books

     CNC Dictionary

     Suppliers

     Tool Brands

Workshop

     Hall of Fame

     Organization: Soon!

 

About

     Customers

     Partners

     Our History

     Privacy Policy

 
All material © 2016, CNCCookbook, Inc.