Thread Mills
A thread mill is similar to an endmill, but with the profile of a thread on the side. Modern CNC machines can helically interpolate all three axes to mill a thread profile into a workpiece. The operator can use the machine’s cutter compensation feature to very precisely control the thread’s major diameter. As the tool wears, offset adjustments will allow you to continue cutting good threads, as long as the form is still good. Thread mills typically produce more threaded holes per tool than taps, for this reason.
Thread mills can also produce threads on the outside of a boss. Be aware that not all thread forms have the same specifications for internal and external versions. Some threads may require a unique thread mill for the internal and external versions.
Haas solid carbide thread mills allow threading of a range of hole sizes, in a wide range of materials, using the same thread mill.
These tools are titanium aluminum nitride (TiAlN) coated, solid carbide cutters with cylindrical shanks, and they feature a hole through the center of the tool to take advantage of through-tool coolant.
This is especially beneficial for removing swarf when threading blind holes, and to lubricate and cool the cutter.
Thread Milling Direction and Programming Guide
These are right-hand cutting tools, meaning they must be programmed with an M03 Spindle On-Forward command on milling machines. These cutters can produce internal right-hand or left-hand threads. The difference is in the programming technique. The circular interpolation motion must be accompanied by a helical motion of the Z-axis equal to 1 pitch of the thread being cut. Positive motion in the Z-axis (moving Z upward) produces a right-hand thread, while negative motion (moving Z downward) produces a left-hand thread.
Thread Milling vs. Tapping
Thread mills differ from taps, because they have a smaller diameter than the thread size produced. The thread mill cutter must be able to enter the drilled hole, and then interpolate the thread profile. Because offset adjustments can be used to compensate for tool wear – as long as the thread form is still good – thread mills typically produce more threaded holes per tool than taps.
It also can be very expensive to remove a broken tap from a workpiece, especially if that workpiece is large. Broken thread mills are easily removed, and often, a new thread mill can be used to finish threading the hole, saving the part from having to be scrapped.
Adaptability
- Mill a variety of thread sizes with a thread mill of the same pitch.
- One thread mill can cut left or right-handed threads.
- A single thread mill can cut many materials.
- Thread mills cut usable threads right to the bottom of a hole.
- Different fit classes can be achieved with one thread mill
- Thread milling does not require a high torque spindle
Improve Results
- Cutter Compensation adjustments on milling machines allows for minute adjustments to hold tight tolerances.
- Thread mills are much more durable with less chance of braking compared to taps.
- Thread mills provide superior chip control over tapping applications.
KEYS TO SUCCESSFUL THREAD MILLING
- Always program climb milling for better surface finish and improved tool life. Climb milling generates less heat and less tool deflection, which leads to vibration.
- Always program the spindle in the forward direction (M03).
- For internal right-hand threads, program the helical interpolation direction with counterclockwise arcs (G03), with the Z-axis starting at the deepest point, and feeding up (Z positive) by the amount of the pitch of the thread.
- For internal left-hand threads, program the helical interpolation direction with counterclockwise arcs (G03), with the Z-axis starting above the deepest point, and feeding down (Z negative) by the amount of the pitch of the thread.
- For external right-hand threads, program the helical interpolation direction with clockwise arcs (G02), with the Z-axis starting above the deepest point, and feeding down (Z negative) by the amount of the pitch of the thread.
- For external left-hand threads, program the helical interpolation direction with clockwise arcs (G02), with the Z-axis starting at the deepest point, and feeding up (Z positive) by the amount of the pitch of the thread.
- Thread mills cut with the side of the tool, so it is very important to use the most rigid toolholders. Typically, a collet chuck does not provide the necessary rigidity to cut high-quality threads. We recommend using a hydraulic chuck, milling chuck, or shrink-fit toolholder. An endmill holder may be used with caution, but might require modifications to speed and feed recommendations, to avoid chatter and excessive tool deflection.
FEEDRATE FOR THREAD MILLING
- The feedrate when thread milling is very important. You should not use the same calculated feed-per-minute feedrate as you would for an endmill cutting in a straight line. Because the tool path of a thread mill is typically a very small radius, the outer cutting edges are traveling much faster relative to the center of the cutter.
- The term “faster” may be misleading; I should say, the edge is traveling much farther in the exact same amount of time. Therefore, we need to perform an additional calculation, based on the difference between the major diameter of the thread and the diameter of the thread mill. The formulas are on the SPEEDS & FEEDS chart for individual thread mill cutters.
By the way, this calculation is not just for thread milling, but can be used in any application where feed-per-minute is used, and the toolpath makes small radial motions.