All Shop Floor Operations References

Thread Milling

Tuesday June 08, 1999
This paper covers the key elements of thread milling on a 3 axis CNC machining center. It is to the point in explaining how the process works, as well as its advantages and disadvantages.

Thread milling, as described in this paper, is performed in a machining center, vertical or horizontal. The machine must have the ability to control all 3 axes simultaneously
to perform the Helical Interpolation necessary to mill the thread.

Some of the advantages are:   

  • The cutter runs at the optimum speed for the material.
  • The spindle runs at a constant speed with no reversal necessary.     
  • The thread size can be adjusted in tenths by off-setting the path of the cutter.         
  • A thread can be produced to full depth ½ pitch from the bottom of a blind hole in production.     
  • The chips produced by the cutter are very small, easily washed away with coolant.    
  • The process is very fast, usually faster than tapping.   
  • The same cutter can be used to produce many different thread sizes. Example: 3/4"-16, 7/8"-16, 13/16"-16, 1"-16; with the same tool.     
  • A small machine can produce a very large thread. Example: 4"-16. This thread is too large to tap in most machining centers.     
  • The cutter can be made to control the major, pitch, and minor diameters.    
  • The process works on internal or external threads.       
  • The thread start can be controlled.     
  • Cutters can be resharpened.     
  • A right or left hand thread can be done with the same cutter.    
  • Some threads can be run dry.

The major disadvantage is cutter cost. It costs about $200.00 for a thread mill to produce a 3/8"-24 internal thread. A tapered thread mill to produce a 1/2"-14 NPTF thread costs about $390.00. At Roberts, we thread milled 1/2"-14 NPTF in 304 stainless steel and got 500 pieces per cutter before resharpening.

The second disadvantage is about 2 diameters is the maximum practical depth. Milling a thread with 16 teeth per inch requires a cutter with 16 teeth per inch that is smaller than the minor diameter of the thread on an internal thread. Actually a cutter about 2/3 - 3/4 of the minor diameter is better because it gives room for chips. 

The cutter is inserted into the hole in the part to full thread depth on center line. With a right hand cutter, the normal type, the cutter is programmed to arc into the inside diameter of the hole to meet the actual major diameter of the internal thread with the OD of the cutter, and traveling around the inside diameter to the left. It is best to climb cut with the thread mill. Then the Helical Interpolation mode is used to circle the inside diameter of the thread to the left 1 plus 1/8 turn while backing away from the part 1 pitch in exactly 1 turn. The extra 1/8 turn is to insure a good thread without start or stop marks. When finished, the cutter is arced back to the center line of the thread to leave the part without a mark on the thread. A left hand thread is started 1-1/8 threads from the bottom and projected into the part while milling to the left. 

External threads can be milled using an insert type cutter. Example: At Roberts we milled a 1/2-NPTF external thread with a 1¼" O.D. cutter with 5 inserts. The cutter body
was about $400.00 and the inserts were $40.00 each in tin coated carbide. Inserts cost less in the long run and can be run faster with longer tool life.

The cutter is placed outside of the part to clear the part and 1 thread from the end of the thread. The O.D. of the cutter is moved tangent to the minor diameter of the thread
to start, then 1 turn + 5° around the part to the right to climb cut while advancing the tool 1 pitch in 1 turn around the part. Then the cutter is moved tangent from the part.

The story is more complex when milling tapered pipe threads because the actual path is a cone with the 1°-47' angle in the Z direction.

Contact Information