Chasing Threads on a CNC Lathe

14 seconds by cncdivi

Chasing Threads on a CNC Lathe

This is part of our series on CNC Lathe Programming.

Repairing threads is a crucial operation for many machinists, either due to the shop handling repair services, or because work needs readjustment for some reason. Manual lathe thread chasing is easy because the machinist has total control over the operation, but when it comes to a CNC, a lot of machinists believe that it’s simply not feasible.

The good news is that it is possible to chase threads on a CNC.  In fact, it can even be easy as some machines have a built-in option to do exactly that.  For machines that don’t have a built-in option to chase threads, it takes a little more work, and that’s what we’re here to talk about.

I’m going to walk through a few approaches discussed around the web, but let’s start from a basic assumption: the spindle is synchronized to the feed via an encoder (or index pulse for some lathes).  That encoder is fixed, so our task is to find the fixed point the lathe is synchronized to and then perturb the tool tip using offsets until that point is tracking our thread properly.

Let’s describe the situation from the viewpoint of a manual lathe.  Let’s suppose you had a lathe where the splitnut could never be unlocked.  You can vary the feedrate, but you can’t unlock.  The tool will therefore always be synchronized at the same point.  How would you go about chasing threads on such a machine?


Dialing the Threads in Visually

The most commonly suggested approach, is the following:

1.  Program a G76 threading cycle that will match your thread.

2.  Chuck up your part, but set the machine up so the X offset is large enough it will only be cutting air–not the material.

3.  Run the cycle very slowly and observe whether the tool is tracking the threads properly.  Adjust the Z offset until it is.

4.  When all is good, you’re ready to run the full thread cycle with the X offset such that the threads will be recut.

You’ll probably want a simple plunge cycle so you can see clearly that the tool tip is headed to the right spot.

This works reasonably well with large outside threads, but can be pretty difficult with small threads, ID threads, and threads that require very tight tolerances.

Seems to me you could make a probe macro based on this principle that ought to work pretty well and be very fast and automatic.

If it was me, I would combine these two methods and start with this approach and then do a quick visual check using the first approach to be sure everything looked lined up properly.


Measure and Align

An approach I liked better I will call measure and align.  Cut a sample thread in the machine of the same spec as the ones you want to chase.  Measure the distance from a chuck jaw face to the root of one of the threads with a set of dial calipers.  This establishes the relationship between a chuck jaw and a thread, and it should be constant.  I’d make sure to use the same chuck jaw each time for measurement.

Now chuck up your piece whose threads are to be chased.  Measure the distance from jaw to thread root.  In all likelihood it will be different than your first measurement.  Apply an offset in Z to make it the same and you’re ready to chase.


Alternatives for Chasing LOTS of Threads:  Custom Tooling Aids

Suppose you have to repair threads a lot, perhaps because you’re working in the Oil Industry.  Further, let’s suppose only a few sizes have to be dealt with.  When this is the case, you can afford to make some special tooling.

Insert a piece of stock in your lathe and thread it.  Put a cap, but, or other inside threaded piece on and tighten it down.  Touch off a feature on the cap or nut and record the Z.  Make a toolholder that can hold the cap or nut in the lathe turret at the exact position it is in.  You’ll need to clamp the nut in the toolholder without removing or disturbing nut or threaded piece.

Now you know that if you thread your workpiece into the nut on the toolholder, move the toolholder to the Z you recorded, and clamp the part in the chuck it will be threaded in the same way every time.  Any arrangement of your special tool that guarantees the threads are positioned at the same angle around the Z axis and the same Z distance can guarantee the threads will be chased properly.

Of course you can use male threads instead of a female cap or nut to chase inside threads.  And, rather than mount the special tool to a toolholder, you could also set things up so you position the turret and use it as a stop for where the end of the nut has to wind up.  Another approach would be to use only male threads on the special tool since you can mesh them with either male or female threads on the workpiece.  Just move the turret to the fixed Z position where the meshing tool’s threads properly meshed with a test thread and then adjust the workpiece in the chuck until it has meshed.  Come to that, you could try doing the same with your threading insert, but the mesh method will be more accurate with multiple threads.

BTW, if you’re going to be doing this kind of work, or really any kind of work with threads, you need to make sure you have all the thread dimension information at your fingertips.  Check out our G-Wizard Thread Calculator.  It covers dozens of thread families, from the common UN and ISO profiles to much harder to find information.

See Also

Speeds and Feeds Calculator Lathe


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!

5/5 - (2 votes)

Recently updated on June 26th, 2024 at 03:48 pm