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.

Versatility

• Able to thread a range of hole sizes with the same thread mill
• The same thread mill can produce right- and left-hand threads with a simple program change
• The thread mill can produce threads in a wide range of materials
• Capable of producing full threads to the bottom of a hole
• The same thread mill can produce any class of fit
• Low cutting forces make thread mills a perfect solution for lower-power machines

Process Improvement

• Hold tight-tolerance pitch diameters with programmed offset changes
• Very low chance of scrap, with the ease of removing broken tools from the workpiece
• No issues with chip control; short chips eliminate the bird-nesting typically associated with spiral flute taps
• Excellent thread finish, with greater control over cutting conditions than with tapping

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.