Welcome to the Thread Milling CAM tip from our CAM Programming Tip Series. Thread Milling is a productive solution for threading holes and bosses. Learn how to master this technique and produce higher quality threads.

Learn more about Thread Milling solutions from Sandvik Coromant.

Calculate results of this technique with our Thread Milling Calculator.

If you have trouble viewing the video posted above, please watch on the Sandvik Coromant YouTube Page.

VIDEO TRANSCRIPTION:

Thread Milling is an ideal option for the threading of both holes and bosses. Instead of using a turning tool or tapping tool to produce a thread, a milling tool is used to helical interpolate a thread to a specified depth and pitch. Depending on the application, this threading technique can yield better quality threads and higher productivity than its alternatives.

While not as widely used as thread turning, it has the primary advantage of being able to thread non-rotational parts, plus large components that are difficult to machine on a lathe. Thread milling uses lower cutting forces making it ideal for machining long overhangs or thin walled components. Thread milling can also be applied closer to the shoulder in blind holes making a relief groove not needed unlike that in thread turning.

Thread milling has many advantages over tapping as well. A range of thread diameter sizes and pitches can be used by the same tool. Plus left- and right-hand threads can be accommodated with the same insert, unlike a tapping tool.

Taps are known for breaking off inside the hole. A thread mill is more secure, has better chip control, and uses less cutting forces than a tap.

Due to a thread mill’s shape it can also achieve full bottom hole threading without the need to drill to an extra depth. Thread mills can also be programmed with radius compensation and with no-coolant in many cases, making them more adaptable.

To produce a thread, thread milling helical ramps a feature with each revolution equaling the pitch of the thread desired. This requires the use of a machine tool capable of simultaneous x, y, and z-axis movement. Also when selecting a thread mill for an ID thread, the diameter of the thread mill should be no more than 70% of the diameter of the hole.

Care must also be taken when calculating the feedrate. Most toolpath feedrates are calculated by the centerline of the tool, which when thread milling internal threads, means the periphary feedrate is faster than the centerline feedrate. It will need to be adjusted to compensate for this effect, and reduce the chance for tool vibration or tool-life issues.

This thread milling calculator is available for use from Sandvik Coromant. Simply input the parameters of the thread to be milled, and the calculator will output important information such as peripheral and centerline feedrates, estimated cut time, programming radius, and axial and radial deviation of the thread. This information can be of great value for accurate programming, predicting productivity, and for checking that the dimensional tolerance of the thread will be acceptable.

To CAM Program this technique in Siemens NX6 CAM software, there are 2 primary choices: The ‘Thread Milling Operation’, or manually driving the toolpath with the ‘Fixed Contour Operation’. Note that in NX7.5, there is also a ‘Hole Milling Operation’ used for creating threads — which is ideal for feature-based machining, as well as an updated ‘thread milling operation’ with a more user-friendly interface.

With the ‘Thread Milling Operation,’ first create a threaded feature in the ‘Modeling Application’. Specify the parameters of the thread desired. In this example, a threaded hole is created.

Next in the ‘Manufacturing Application,’ create a thread tool with the same pitch specified as that of the thread feature.

For NX6 CAM programming, follow these steps to produce a thread milling toolpath: Specify the number of start&ends, the pitch, the engage&retract, and then select the hole geometry on the screen. Finally, use ‘Axis Control’ to select the thread direction.

For NX7.5, users this can be controlled by an updated ‘thread milling operation’ with a more user-friendly command box.

Optionally, for producing simple threads the ‘fixed contour operation’ can be used. First in the ‘Modeling Application’ create a helix with the same diameter, pitch, and length desire to drive a thread tool.

Next in the ‘manufacturing application’ use the ‘fixed contour operation’ with ‘Curve/Point’ as the ‘drive method’. Select the helix as the drive curve, selecting the desired end of the helix as the start point for the thread mill.

Here we can see each of the these threaded hole examples being machined by the ‘thread Milling operation’ and ‘fixed contour operation’ in NX.

For more information about implementing this technique or any other CAM questions, please contact your local Sandvik Coromant representative.