Threadmills are cutters used in CNC millling machines to cut internal and external threads.  The process is called “CNC Thread Milling.”  The other threading process for CNC Mills is Tapping.  On lathes, single point threading (turned threads) and taps are used.  The popularity of these methods is Tapping, Single Point Threading, and Thread Milling.

threadmill

A selection of threadmills.  Image courtesy of Harvey Tool.

CNC Thread Milling vs Tapping

Let’s get one thing out of the way up front–Tapping is faster than CNC Thread Milling.

That being the case, you might wonder why anyone ever uses CNC Thread Milling?  There are a number of advantages CNC Thread Milling has over Tapping that often make it the preferred choice including:

  • If you break a Threadmill, it won’t get stuck in the part.  Removing broken taps is painful, especially if the tap is embedded in a part that’s already been machined at considerable expense.  Thread milling is often preferred for expensive components and late stage machining for this reason.
  • The teeth of threadmills can be larger and stronger than taps because of the reduced need for chip clearance.  This makes them less likely to break.
  • Thread Milling is better for harder materials because you can cut the material in smaller steps, and speeds and feeds can span a wider range than a tap, which is limited by the pitch of the thread being tapped.
  • Chip clearance is easier because threadmills typically generate short, comma-shaped chips whereas taps can create long stringy chips that “bird nest”.
  • Thread Milling requires less horsepower than tapping, which may be an advantage for lighter-weight CNC machines.
  • The lower cutting forces of thread milling can be advantageous in long reach and thin wall applications where tool deflection and chatter are problems.
  • A single threadmill can be used to cut many thread sizes.  A separate tap will be needed for each thread size. On parts with multiple threads, there can be considerable toolchange savings with thread milling.  There is also savings in reducing the amount of tooling inventory that must be kept on hand for standard thread sizes.
  • You can thread mill odd-sized threads for proprietary applications.
  • A thread mill can be used to back chamfer the hole.
  • Thread mills have no need for special tension compression holders or tapping heads.  This is an advantage on CNC Machines that lack rigid tapping capability.
  • Taps get increasingly expensive as size increases.  At some point, threadmill cutters are cheaper than very large taps.
  • While coolant can be used, most manufacturers suggest dry machining is the first choice when thread milling.  Exceptions would be stainless steel (reduces work hardening), aluminum (reduces chip welding), and cast iron (to keep the dust down).  Otherwise, a good compressed air blast will be fine.

That’s quite a long list of advantages for thread mills that may make them perfect for your application instead of tapping.

Thread Mill Cutters

Spiral Flute Thread Mills (also called “Multi-Point” or “Multi-Form” Threadmills)

Spiral Flute Thread Mills can cut faster than Single Profile (or Single Point) Thread Mills because more than one thread can be cut by the multiple rows of teeth.  Spiral Flute Thread Mills can cut lefthand or righthand threads and it can vary the diameter of the threads, but they are limited to a single thread pitch governed by the spacing of their teeth.

Single Profile Thread Mills (also called Single Point Thread Mills)

single profile thread mill

A single profile thread mill.  Image courtesy of Lakeshore Carbide.

Single profile thread mills only have teeth to do one thread at a time.  Therefore, they can be used for a wide variety of threads by varying the depth of cut and the pitch of the thread helix.  Spiral Flute Thread Mills can only do one helix pitch because the distance between teeth is fixed.

Integrated Countersink

Many threadmill manufacturers offer versions with integrated countersinks at the top of the threadmill to eliminate the need for a tool change where countersinking or chamfering is desired (almost always!).

Solid Carbide vs Indexable Thread Mills

indexable thread mills

As with most any other tool type, Threadmills are available as indexable tooling with replaceable inserts.  A variety of types are available including Single Profile, Single Insert Spiral Flute, and Multiple Insert Spiral Flute.

The usual motivation for indexable tooling is cost–you can replace an insert rather than the entire tool.  However, as is the case with most indexable tooling types, the geometry and therefore the performance of equivalent solid carbide tooling is superior.  Therefore, indexable Threadmills are generally preferred only when doing large volumes of threading in relatively larger holes.

Choosing a Threadmill

Profile Distortion: Diameter

If the diameter of the thread mill is more than 70% of the diameter of the thread, the thread profile can be distorted, so be sure the thread mill is no larger.

Single Profile or Spiral Flute?

This choice will be based on whether you want to maximize flexibility for multiple thread sizes or reduce cutting forces as much as possible.  In either case, a Single Profile Thread Mill is preferable.  But, if those are not at issue, a Spiral Flute Thread Mill will generally cut faster as well as spreading wear over multiple flutes so the tool lasts longer.

Use the Manufacturer’s Help

All tooling catalogs for Threadmills are full of suggestions and guides to help you choose the right threadmill for your job.  They’ve also got support lines where you can call up and get a consultation.  Be sure to take advantage of these resources to help you choose the best cutter for your job.

Toolholders for Thread Milling

Most (but not all!) Threadmill manufacturers recommend set-screw type toolholders over ER Collet Chucks for Thread Milling.  If you plan to use a set-screw holder, make sure your Threadmills have the Weldon Shanks that maximize the effectiveness of the holder.  

= How to Thread Mill =

Thread Milling Feeds / Speeds + Thread Milling Calculator

Like anything else having the right Feeds and Speeds is very important when Thread Milling.  The Threadmills can be small, delicate, and inexpensive, so it’s no fun to break one.  The good news is our G-Wizard Feeds and Speeds Calculator does Threadmill Feeds and Speeds!

Here’s how it works:

Step 1: Choose machine and material

Step 2: Choose a threadmill for tool type

Threadmill calculator feeds and speeds

Step 3: Enter Tool Diameter and Flutes

Let’s say we’re going to cut a 1/2-20 internal thread.  Our rules for selecting a thread mill require no more than 70% of hole diameter for threadmill diameter.  So we want a threadmill that is no more than 0.350″ in diameter.  I like Lakeshore Carbide’s tooling (Carl is great to deal with), so I will go choose a threadmill from his online catalog.

I picked an uncoated threadmill and the specs say 0.350″ diameter, 4 flutes.

Step 4: Enter Cut Depth and Cut Width

I’m going to cut threads a 1/2″ deep in one pass, so I will set my Cut Depth to 0.500″.  Cut Depth is the difference between major and minor diameter of a 1/2-20 thread.  We can look that up on G-Wizard’s Thread Tab:

thread mill calculator

I’ll just use the Sharp-V height (0.0433″) because its easy.  In practice, our cut depth is a little less to allow for the flats.

That’s about all it takes to get some Feeds and Speeds back from G-Wizard:

Note that as the tips say, we could be going a lot faster rpm-wise, but it’s okay to go slower.  We’ll get better tool life too.  

If we wanted to take it a little easier, we can dial back the Tortoise-Hare slider more to the Tortoise side–whatever feels right for the situation. 

That’s all it takes.  If you’ve never tried G-Wizard, get on board with our 30-day free trial:

Writing Thread Milling G-Code and Thread Mill Program Generators

Helical Interpolation

CNC Thread Milling is possible because CNC Machines allow us to program Helical Interpolation.  This allows the cutter to follow a helical path that corresponds to the thread’s helix:

helical interpolation

A Helix programmed in G-Code…

Here’s a chapter to show you how to write helical interpolation in g-code that’s part of our Free GCode Programming Course.

Reverse Rotation vs Synchronous Milling

Assume clockwise spindle rotation.  The difference between reverse rotation and synchronous milling is a function of whether the thread mill’s helical motion is clockwise or counter-clockwise.  If the helix is clockwise like the spindle rotation, it is called “reverse rotation milling”.  Why that makes sense to call it reversed when the direction is the same, I don’t know!  But remember it that way.

Alternatively, we can think of synchronous rotation as down milling and reverse rotation as up milling.  As always, we prefer down-milling (aka Climb Milling) where the tool is feed in the direction of tool rotation.  It provides the lowest cutting forces and best surface finish.

If the direction of the helix (viewed from above) is counter-clockwise, it’s called synchronous milling.  

Synchronous Milling is usually preferred because it achieves lower cutting forces, improved chip formation, better tool life, and better surface finish.  But, there are specific conditions to consider when choosing which direction to cut:

reverse rotation synchronous milling

Reverse Rotation vs Synchronous Milling.  Image courtesy of Guhring.

Note the black arrows that show the direction the helix unfolds based on whether we’re cutting RH or LH threads and the direction of the helix.  When the arrow points up (blind holes in other words), we start at the bottom of the hole and thread to the top.  

Cylindrical vs Conical (Tapered or Pipe) Threads

Having established all of our directions of motion, the next consideration is whether we’re cutting a cylindrical or conical helix.  Tapered (Pipe) threads require a conical helix.  This is accomplished during programming by correcting the helix every 90 degrees.  Each 90 degree segment corrects its endpoint to account for the tapered thread helix.  For even greater accuracy, divide the arcs into 8 sections or 45 degrees each.

Thread Milling Entry Methods

We now understand the shape of the helix and the directions of motion.  How do we get the Threadmill Cutter into the thread so it can start cutting?

There are several methods:

  • Linear Plunge:  The Threadmill moves from center of hole to cutting with a straight linear plunge.  This method is simple to program but has mutliple drawbacks.  It creates the biggest loading on the tool and long chips.  Plus, there will be a small delay mark in the threads as the tool transitions from plunge to helical motion.  Therefore, this method is not recommended where accuracy is required or the threads are small.
  • Quarter Circle Entry:  We can program the Threadmill to ramp in via a quarter circle that gradually meshes into the thread helix over 90 degrees.  In this method, we make a linear motion to get the Threadmill close to engaging and then finish ramping in with the quarter circle arc move.  It’s advantage is simplicity plus improved performance over a simple linear plunge.  However, it is still only recommended when the Threadmill is quite a bit smaller than the hole.
  • 180 Degree Semicircle Entry:  Here the tool starts in the center of the hole and performs a semi-circular arc of 180 degrees to enter the cut.  This takes the most programming effort but produces the best results across the widest range of parameters. 

Troubleshooting Thread Milling

Problem Potential Cause and Solutions
Too much insert flank wear

Cutting speed too high:  Reduce speed or use a coated insert that can handle the speed.

Chips are too thin: Increase feedrate.

Insufficient coolant:  Increase coolant flow or aim the coolant better.

Cutting edge chipped

Chips are too thick: Reduce the feedrate or increase rpms at same feedrate.

Vibration: Check and improve workpiece and tool stability.

Material build up on cutting edge

Incorrect cutting speed:  Use proper speeds and feeds.

Unsuitable carbide grade;  Use a coating appropriate for the material.

Inadequate coolant:  Use a coolant that promotes lubrication with the material being cut and make sure there is adequate flow to the right spot.

Chatter or Vibration

Feed rate is too high:  Reduce the feedrate.

Profile is two deep: Perform the cut in two passes.

Thread length is two long:  Make multiple shorter passes to cover the full length.

Insufficient thread accuracy Tool deflection:  Reduce stickout and feedrate.
Chipping of non-cutting edges Vibration:  Check cutter and part stability.
 

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!

Easy Guide to Threadmills [ Calculator, Speeds/Feeds, & Programming ]
5 (100%) 1 vote