Thread Milling Techniques

via  OSG Tap & Die

Jan 2, 2023 editors note: This article has been updated with new drawings and videos since it's original publication date.

The machining technique for OSG’s thread mills have been developed for thread milling on a 3-Axis, 4-Axis and 5-Axis CNC controlled machine tool.

​The thread is processed by advancing one pitch feed per revolution in the axial direction, utilizing the planet-like rotation and revolution movements of the tool. Internal and external thread, right or left hand threads can all be produced with this one tool, simply by changing the direction of rotation and/or feed.  This process is called Helical Interpolation and will be explained in greater detail below.  

Threading Process

1. Move to edge (maintain clearance)
2. Cut with helical milling
3. Mill the circumference of the circle
4. Pull away from the edge
5. Remove tool

The transition between the start and the finish of the milling operation must be smooth, and the appropriate amount of feed is essential for minimizing milling resistance.

​There are many different methods for using this tool, but our research has shown that this technique provides the most precise and efficient operation.

Download OSG Thread Mill Software

---

Understanding Thread Mills

Figure 1. Helical Interpolation

Any three axis mill that is capable of helical interpolation can be used for thread milling. Helical interpolation involves three axes moving simultaneously. Two axes, 'X' and 'Y', move in a circular motion while the 'Z' axis moves in a linear motion.

​For example, the path from point A to point B (Figure 1) on the periphery of the cylinder combines a circular movement in the 'X-Y' plane with linear movement along the 'Z' axis. The 'X' and 'Y' circular motion will determine the diameter of the thread. The 'Z' axis linear motion will cut the pitch (or lead) of the thread.

Thread mills must completely enter the minor thread diameter before cutting the internal thread. (Figure 2)

Most all thread milling manufacturers' catalog lists the smallest internal thread that each thread mill can produce.

The same thread mill can also produce any larger size thread of that same pitch. Also, for small sizes, it is best to use our short series with the reduced length of cut whenever possible.

Figure 2. Thread mills must completely enter the minor thread diameter before cutting the internal thread.

All of the straight flute thread mills are for internal threads only. All of the staggered tooth thread mills will cut both the internal and external threads. The helical thread mills over 0.187 diameter will also cut both internal and external threads.

Staggered tooth thread mills have every other tooth removed in a staggered pattern; as the tool rotates the adjacent flute fills in for the tooth that was removed. This helps to reduce side cutting pressure, thus reducing chatter. This can be extremely beneficial in small external sizes and for set-ups that lack rigidity.

Helical fluted thread mills are also designed to reduce side cutting pressure by distributing the cutting pressure along a helical flute. Although these tools cost slightly more, their high performance design allows for less chatter and higher feed rates.

---

How to Use Thread Mills

To produce internal threads, drill the minor thread diameter to its appropriate size. Then, position the thread mill to the required depth. Next, mill either the 'X' or 'Y' axis to the required thread pitch diameter. With small sizes and with difficult to cut material, it may be necessary to remove the material in several passes. It is always best to "arc-in" and "arc-out" when thread milling.

Any "arc-in" and "arc-out" movements must have a corresponding 'Z'-axis motion during the 'X-Y' circular moves. For example, if the "arc-in" is over 90 degrees, the 'Z'-axis departure must be 1/4 of the thread pitch. (90 degrees is 1/4 of a circle).

• A right-hand thread is produced by orbiting in a counterclockwise direction while bringing the 'Z'-axis up one pitch per 360 degrees.
• A left-hand thread is produced by orbiting in a clockwise direction while bringing the 'Z' axis up one pitch per 360 degrees.
  

The entire process can be achieved by interpolating in a downward direction and reversing the orbit direction.

However, it is highly advisable to do so since the tools will have much less material to remove. If the tool is to be interpolated in an upward direction, spiral interpolation must be used.

The same surface feet per minute can be used for thread mills as for end mills of the same size. The feed rate must be slower, however, since thread milling often involves unfavorable length-to-diameter ratios. Also, keep in mind that the thread mills have more surface area contact than an end mill of equal length. Most CNC mills are programmed in inches per minute which is applied at the centerline of the spindle.

In internal applications, the outside diameter of the tool will be traveling faster than the centerline of the tool. The reverse is true for external applications. It is best to start out conservatively with feed rates and the number of passes required and adjust upward per good machining practice.

External threads (Figure 3) must have the major diameter milled to size before the thread mill is used. Right-hand threads are cut by interpolating up and in a counterclockwise direction. The same threads can be cut by interpolating down and changing the orbit direction.

​NPT threads are usually produced while interpolating the tool in a downward direction. Since these tools are crest cutting, it is not absolutely necessary to ream the internal minor diameter or mill the external diameter to size.

Figure 3. External Thread Milling

---

Troubleshooting Threadmilling

update August 2020:  OSG just released this new troubleshooting video that   further details some thread milling concepts.