CNC threading.

Single-point threading with inserts or thread rolling are both good choices.

There are many methods of producing threads. Utilizing CNC turning can be one of the most productive and versatile, depending on workpiece size and the production quantities desired.

In general CNC turning, threads are produced by using a single-point insert, taking numerous passes at decreasing depths of cut or by thread rolling using a LMT-Fette-style head and three hardened steel rolls. Single-point threading for internal and external threads can thread workpieces up the capacity of the lathe diameter of stock handled, whether bar or chucking machine. Thread rolling is typically used in production situations for smaller sized threads, typically 1[inch] in diameter or less.

The thread rolling method utilizes a metal-forming process, which actually displaces the metal. The thread rolls form the metal from the root of the thread form into the actual major diameter. Therefore, it is extremely important that the size of pre-formed blanks or stock is held to size tolerance. If the turned diameter is too small, the roll forming process will not fill out the crest of the thread. If the flank diameter is too small, the thread crest "overfills."

When thread rolling is done properly, the thread that is formed is extremely strong. The actual forces to thread roll are contained within the thread rolling head itself. Once engaged on the part, the thread rolling head self-feeds forward until the Z axis movement of the machine stops. Once the machine axis reaches the desired depth, the process of arresting the movement results in the head opening automatically. The head has to be reset to the closed position prior to running another workpiece. There are ways to "automate" resetting the head with tripping mechanisms or even a powered piston device.

Some points about thread rolling: A thread should not be "re-rolled" as the process workhardens the material. One disadvantage of thread rolling is that the tooling is quite large so that adjacent stations on the turret typically lack the clearance to use other tooling. Tapered threads are the most difficult to thread roll due to the complete contact of the rolling head. Thread rolling, however, is by far the fastest method of thread production on a CNC lathe.

For CNC turning, the single-point insert method is usually the first choice. An insert design is available to produce each individual thread profile. This insert style is called a "full form" style and includes the correct root and crest radius. This full thread form will result in a quality thread form, but initially it will cost more because a specific insert will be needed for each individual thread form - individual thread forms must be purchased for both outside diameters and inside diameters. The so-called universal insert may leave a crest with a burr that will have to be removed. For reference, please note that a left hand outside diameter threading insert can be substituted for a right hand internal insert.

Compound plunge angle. The programming methods for standard threads utilize a "compound" angle of approach of the insert down the thread flank. The position of the Z axis start point will change with each thread pass. The programmer must calculate this position for each successive threading pass depth. The term "compound" is derived from the compound slide utilized on an engine lathe when threading. The CNC program takes several passes to remove the material, each pass reducing the actual "X" value. The reduction in each pass is to allow for the fact that the threading insert is actually contacting a greater area of the thread as the depth increases. Consult pass depth charts for various materials for radius values and double them for diameter values. Many programmers duplicate the last thread pass as a spring pass to remove any deflection that may have occurred.

The standard compound angle is 29 deg, ensuring that most of the cutting action is on the front flank of the threading insert. This produces a chip from the front of the insert and is recommended for the majority of threading in standard steel. Modified plunge angles of 10 to 20 deg should be used when threading the tougher materials, such as 316 stainless or Hastelloy. By using a plunge angle of 14 deg, the programmer ensures that the majority of cutting is still carried out by the front of the insert; at the same time, the trailing edge of the insert still removes a small amount of material ensuring that workhardening does not take place.

To program a plunge angle, the Z starting point will need to change for each pass. This thread start dimension should be at least 0.300[inches] from the thread start position to allow sufficient room for the slideway to accelerate to the correct linear speed for the threading operation.

If a normal 29-deg angle is used on a material that has a tendency to workharden, the rear edge of the insert will "rub" down the flank, producing a hard surface that will considerably shorten tool life. The alternative method is a central plunge, removing the same amount of material from both the leading and trailing edges of the threading tool. If the modified plunge angle doesn't perform, the central plunge should be tried.

The central plunge removes stock with both flanks of the insert and is recommended when threading aluminum. The programming method for this will utilize the G76 code only once, as the thread starting point is constant.

An important exception. An Acme thread is 29 deg included angle. The plunge angle to produce an Acme thread must not exceed 14 deg. Failure to program this angle (again using the G76 code) will result in the threading tool producing an incorrect back flank angle.

Threading speeds. Threading can be carried out at high cutting speeds corresponding to the turning sfpm selected. The choice of cutting speeds needs to include the evaluation of the physical limitations of the machine tool. This limitation is a function of the acceleration and deceleration capabilities of the axis drives fitted to the machine. The machine tool builder should be consulted about the threading capabilities for each style of machine tool. Newer machines with high performance servodrives will operate at faster Z-axis drives. With many machines, the maximum Z-axis travel rate value is 100 ipm, though newer machines with high performance servodrives will operate at faster Z-axis drive rates.

The threading cycle is always programmed in G97 direct rpm. The programmer will calculate the actual G97 speed from the recommended constant surface speed. When the running the machine, the control will monitor the actual speed and axis movement. If the machine is fitted with manual override on the spindle speed, the operator must ensure that this is set at 100%. If this setting is changed, the control will accelerate the spindle for the actual threading pass. However, the actual pitch position will probably not match, ensuring that the thread will not "pitch in." Normally, this will result in a scrapped part.

Cutting helix angles. The production of smaller thread diameters for helix angles requires the selection of the correct shim seat. The standard shim in many types of "laydown" threading tools is 1.5 deg. This is suitable for the majority of threading applications. For the production of high helix angle threads, a special shim seat is recommended. This special shim seat ensures that the threading insert is in the normal plane to the thread helix angle. Each threading supplier will provide a chart that illustrates which shim seat part number should be selected for each particular application.

It is even possible to reduce tooling costs for cutting right hand and left hand threaded nuts by programming the right hand thread using an M03 command and threading toward the spindle. To produce the left hand thread a reverse angle shim was used and the threading cycle was programmed to cut away (Z axis + direction move) from the spindle. This produced a satisfactory left hand thread. Consult the tooling book for the correct shim style for each application.

Steve Rose has developed hands-on training materials aimed at CNC machine operators, programmers, and setup people. For more information about training from Rose Training Systems, Highland Hts, OH, call [phone] or visit Rose Training on the Internet: http://www.rose-training.com.