Thread Milling Primer

May 6, 2024 9:27 am

Thread milling is a machining process used to produce threads in holes or on the external surfaces of a workpiece. It involves cutting a thread using a unique milling cutter that moves in a helical path. Thread milling can be a complex and challenging application for many, as it requires relatively complex programming and expensive tools. Because of that, many people opt for the more straightforward solution of tapping, but if you invest the time and effort to master thread milling, you will discover that it brings many advantages.

Thread Milling Advantages

  • Savings on tool inventory: The same cutter can be used for right-hand and left-hand threads. Threads with different diameters can be made with the same tool as long as the pitch is the same.
  • Precision: The CNC program and tool offsetting allows for precise control over thread size and tolerance.
  • Process reliability: Minimal risk for machin stops as the cutting forces are low and the chips are short.
  • Machine “health”: Thread milling extends machine spindle life compared to tapping because spindle rotation doesn’t need to stop and reverse every thread.

Now that we understand the advantages, let’s delve into the machining process and CNC program.

The Basic Thread Milling Toolpath

A spiral movement is required to perform a thread milling operation. Helical interpolation is a CNC toolpath along a helical path. This spiral motion combines circular movement (G02 or G03) in the XY plane with a simultaneous linear motion in the Z direction.

The Z distance from point A to B equals the pitch.

The diameter machined by the tip of the cutting tool is the thread’s major diameter in internal threads or the thread’s minor diameter in external threads.

If you are unfamiliar with G02/G03, watch the video below to get up to speed.

Tool/Thread Configuration and how it affects the program structure

  • Single Tooth: In this scenario, the tool makes a continuous toolpath, completing numerous full rotations according to the thread’s length divided by the pitch. The advantages are that less load is exerted on the tool, and that the tool is cheaper. The disadvantage is that this configuration yields the longest cycle time.

  • Multi Tooth (Cutter length Longer than thread): This scenario has two major advantages and is the first choice except when the load can be sustained. The cycle time is the shortest, and the CNC program is the simplest. This is because the tool only needs to make a single 360° movement to complete the operation. However, it should be noted that the tool comes with a higher price tag and experiences greater loads.

  • Multi Tooth (Cutter length Shorter than thread): When the thread is very long, or the load is too high, it is necessary to use this configuration. However, it comes with two main disadvantages. The CNC program is more complicated, and there might be a slight mismatch between iterations as the operation is not continuous.

TIP: You can use this Threadmilling Gcode Generator and check out how the program looks like in different scenarios.

Climb or Conventional milling?

Climb milling is typically preferred over conventional milling for machining threads due to lower cutter load, longer tool life, and better surface finish. However, there are situations where conventional milling is more appropriate.

  • If the machine does not compensate for backlash, the cutting force direction in conventional milling closes the backlash gap.
  • When machining cast iron or hardened materials because, the cut begins below the material’s surface.

CNC Program Directions

To determine the required directions, there are three factors to consider: handness (right or left), thread type (external or internal), and milling method (climb or conventional). Use the table below to figure out the required directions for your configuration.

Cutter Diameter Selection

Thread turning produces perfect thread geometry, while thread milling creates a slightly distorted thread geometry. The distortion is influenced by the cutter diameter, pitch, and thread diameter. A smaller cutter provides the most precise thread profile, but it must be balanced with cutter stiffness.

Internal Thread Milling:

  •  Recommended: 50%-70% of the thread diameter.
  • Never more than 85% of the pre-drilled hole.

External Thread Milling:

  •  Recommended: 70%-100% of the thread diameter.
  • If profile accuracy is not crucial, using a larger cutter can boost productivity.

Radial Passes

When the thread profile becomes deeper, it is advisable to divide the operation into several radial passes to lessen the burden on the cutter. By increasing the number of passes, you can enhance the tool life, surface quality, and production stability. However, this will also result in a slower cycle time.

Use the table below as a starting point for the number of radial passes and adjust according to your specific application.

 

(*) All images provided courtesy of MachiningDoctor.com

Leave a Reply