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

Button Cutter, Copy Mill, or Toroidal Cutter: Round Insert Milling Cutters

Apr 7, 2013   //   by Bob Warfield   //   Blog, FeedsSpeeds, Products  //  1 Comment
Tormach's Toroidal Cutter

Tormach’s Toroidal Cutter

Have you ever tried a button cutter for milling?

If so, you’ll know that these versatile tools can really do a good job for you.  There’s a lot to recommend round inserts as they have a number of properties that contribute to their success.  If you’ve used one turning, you’ll know that their large radius can yield some very nice surface finishes.  They can leave a good finish when milling too, but they have a number of other advantages.

Machinists know this and so do a lot of our customers:  Button Cutters, also called “Copy Mills” and “Toroidal Cutters”, are the number one most requested new tool type for G-Wizard Calculator on our User Suggestion Portal.

It seems that for whatever reasons, the physics of cutting favor circles.  HSM toolpaths do better than conventional paths by adopting loops rather than sharp corners.  And button cutters do well because corners on inserts are a weak point that can chip or break off.  You can load up a button cutter pretty hard and they’ll hang in there.  If you do manage to chip one, just rotate the insert until the chipped portion is not being used and keep going.

The physics of button cutters mean that some very special calculations have to be done when figuring their feeds and speeds.  There are several important issues to consider:

1.  Cuts should be made with a depth of cut less than the radius of the insert.  That means the diameter of the tool is a function of the depth of cut because of the radius that is the edge of the cutter, just like a ballnosed endmill.

2.  Toroidal cutters are subject to chip thinning in two dimensions.  Like any rotary cutter, if the width of the cut is less than half the diameter, chip thinning occurs.  There’s a diagram showing how this geometry works as part of our speeds and feeds tutorial.  It’s very important to consider chip thinning or your actual chipload may be lower than you expect and the tool can start rubbing, which will dramatically reduce cutter life.  However, when you not only have a rotating tool but one with round inserts, you get chip thinning in both the radial and axial planes.

3.  Because of their unique design, toroidal cutters can tolerate quite a bit more chipload than most other kinds of indexable cutter.  There’s no corner weakpoint that can be easily damaged by cuts that are too aggressive.  This is also true to a certain extent for bullnose endmills, which are just endmills whose bottom edge has been given a radius.  Think of them as button cutters whose round inserts have a really tiny radius.

4.  While the cutter pictured doesn’t do so, more exotic designs may also “lay down” the round insert slightly, introducing a lead angle on top of everything else that is going on with the geometry.

Suffice it to say that simple tables are not going to yield the best results.  You need to be prepared to do some extra calculating, or to use a calculator like our G-Wizard Software that does all that for you.

There is a lot else to recommend button cutters.  For example, they make great tools for helical interpolation of holes.  And, they tend to convert a lot more of the cutting force to the axial direction, which is the stiffest direction for most machines.  The lower the depth of cut, the more of the force is translated axially.  Lastly, when roughing out steps, you get a smooth scallop instead of a shoulder with a corner.  This can make life easier for your finishing cutter.

Before we leave the topic, let’s consider a few basics in terms of how to operate a button cutter:

1.  Try to keep at least a 75% stepover so the inserts spend a lot of their time in the cut.  This minimizes the chip thinning in one direction, but it’s okay since round inserts get chip thinning in the other direction.  The reason to maximize the stepover is that most of the wear and tear on the inserts is on entry into the cut.

2.  Speaking of entry into the cut, arcing in and helixing in are far preferably to plunging in.  Try our Conversational CNC Surfacing Wizard and Hole Wizard for some gentle tool paths when using one of the cutters for face milling or helical interpolating holes.

3.  Keep the depth of cut below the cutter radius.

4.  As you’re considering the best depth of cut, try to keep the width of cut relatively high (about 75% as mentioned in #1).  Keep depth of cut less than the insert radius.  In fact less is more with these cutters, so drop it down as far as you can while keeping acceptible Material Removal Rates.  You can play with these tradeoffs using G-Wizard Calculator to find the sweet spot.

Setting Up G-Wizard Calculator for a Button Cutter

Setting up a Button Cutter in G-Wizard is pretty simple.  We’ll use Tormach’s 25mm cutter as the example.   As mentioned, it has a 25mm diameter.  It uses a round insert with a 10mm radius.  So, choose an Indexable End or Facemill tool type, tell it how many inserts (3 for the Tormach) or flutes, and click the “Geometry” button.  Set it up as shown:

button cutter feeds speeds

Set up a button cutter as an endmill with a big corner radius…

Basically, you just want to set it up with the right diameter and corner radius.  BTW, I used a trick to do that.  The Tormach cutter uses metric dimensions and I was running in Imperial.  So, for the Cut Diameter, I entered “25/25.4” and hit Enter and it did the calculation right in the field.  You can also enter “25m” to convert mm to inches and 25i to convert inches to millimeters.

You’ll need to make sure you have G-Wizard Calculator version 1.8 or later as that’s where the corner radius feature was added.


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

1 Comment

  • Thanks for the tip about how to use GWizard to convert metric to inches and inches to metric. You should put that in the tips on start up.

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.