Thread Milling requires the use of a machining center capable of helical interpolation. This means that the machine must be capable of three axes simultaneous movement. Two of the axes perform circular interpolation, while the third axis moves perpendicular to the circular plane. On most CNC controls this is achieved with a G02, or a G03 code. There are other factors to consider when using a Thread Mill, the most important being fixturing, and tool length extension. Due to the cutting action of a Thread Mill the forces acting on the part differ greatly than those due to tapping. The more rigidly the part is fastened to the fixture the faster you can Thread Mill. The speeds and feeds are maximized when vibration of the part and fixture is minimized. The next factor of the utmost importance is the tool, and tool holder. Speeds and feeds are reduced depending on the distance a tool is held from the spindle face. A positive lock end mill style holder is always recommended. Never use a collet style holder for a Thread Mill. If you consider the rigidity of your fixture, and the distance of the tool from gauge line, you should not have a problem with any thread milling operation.
Tool Body and Insert Selection for Advent Tool Replaceable Insert Thread Mill
1. Select the thread form you desire to thread mill. (1.5" - 12UN internal)
2. Choose the tool body that will cut the thread form you need. (tool# 15-TA-01-F5)
3. Check the diameter of tool with inserts. This depends on the thread form on the insert.
4. Compare proper diameter of tool with minor diameter of thread, or drill size. The cutter diameter must not exceed minor diameter of thread, or drill size. (1.5" - 12UN minor diameter = 1.41")
5. Find insert style that fits body chosen.
6. Order insert by applying form to insert style. (insert# ATM-410A12)
Feed Rate Calculation
Due to the circular motion of the cutter as it forms a thread the actual feed rate at the cutting edge will be different from that which is programmed at the center of the tool. For an internal thread the feed rate at the edge increases as the cutter diameter increases. For an external thread the feed rate at the edge decreases as the cutter diameter increases. This can be shown as a direct relation between the size if the circle the cutter moves around, and the size of the circle cut.
Internal thread: F1 = F2 X ((Dw - Dc )/Dw)
External thread: F1 = F2 X ((Dw + Dc )/Dw)
F1 = Programmed feed rate at the tool center (in/min)
F2 = Actual feed rate at the cutting edge
Dw = Diameter of the work piece, or thread diameter
Dc = Cutter diameter
The actual feed rate is calculated using the standard formula : F = (RPM) X (Chip load) X (No. of teeth)
Thread Mill Programming
The simplest method to produce a thread form using an Advent Thread Mill is as follows:
1. The center of the hole being the X-Y zero point. Move the cutter to the center of the hole, then to the thread depth required.
2. Move the cutter over a small distance (usually about .02”towards the three-o’clock position) to call up your cutter compensation.
3. Machine in a counter-clockwise direction generating a 1/2 circle and ending at the full thread depth at the nine-o’clock position. Simultaneously moving 1/2 pitch in the Z direction. The direction of the Z movement will determine the handedness of the thread.
4. Produce your thread by generating 1 full circle (counter-clockwise) around the center, while moving 1 full pitch in the Z direction.
5. After the full form has been machined, return to your starting position near the center of the hole. This is done by generating another 1/2 circle (counter-clockwise) combined with a 1/2 pitch move in Z direction.
6. Return to your hole center, and exit the hole.
Thread Mill Process - Internal Thread
1: Z rapids in minus direction to depth
1-2: Rapid in Y-axis to within 0.05 of minor diameter from pos. 1 to 2 and picks up cutter compensation.
2-3: Feed from pos. 2 to 3 lead in as Z is moved up in the + direction 1/2 thread pitch
3-4: Feeds 1 revolution from pos. 3 as Z is moved up in the + direction one thread pitch
4-5: Feeds from pos. 4 to 5 lead out to the center of the hole as Z is moved up in the + direction 1/2 thread pitch all at a higher feed rate
5: Z will rapid to the top of the hole and remove cutter compensation