Threading is a method of machining various internal and external threads with threading tools. Thread cutting is the most efficient and economical processing method for processing threaded parts.
What are the Processing Methods for Internal Threads?
Thread Machining or production refers to the process or production of machining large quantities of threaded parts with an automatic multi-axis tool. The processing methods of internal threads include tapping, extrusion, milling, turning, and grinding.
Tapping of Internal Threads:
Tapping is an effective and commonly used machining method. Tapping is a continuous cutting process, and the workpiece material is cut off by sequentially arranged cutting edges. The final thread size can be obtained in one pass. Taps are specially produced according to the major diameter, minor diameter, and pitch diameter of the thread. Because taps must perform roughing and finishing in one pass, large amounts of chips must be efficiently expelled and can create excessive pressure that can lead to thread quality problems or damage to the tap. Spiral flute taps feature variable lead flutes for excellent chip control.
When tapping, special attention should be paid to chip control. When machining workpiece materials with low hardness, high viscosity, and easy-to-produce long strips of chips. These strands of chips have the potential to form clumps around the tap or accumulate in the flutes, causing the tap to break in the hole. Aluminum, carbon steel, and 300 series stainless steel are often the most challenging workpiece materials for chip control. Taps can process almost any workpiece material with a hardness lower than HRC50, and some taps can even process workpiece materials with hardness as high as HRC65.
Pore size is another factor to consider. Most end users can only tap holes with a diameter of less than 16mm. If the hole diameter exceeds 16mm, they will face the problem of whether the machine tool has enough power to turn the tap. When the diameter of the screw hole is less than 6.35mm, due to the limited chip space and the low strength of the small-diameter tap, the tapping process is prone to problems.
In addition, the length of the internal thread that the tap can process can usually reach more than 3 times its diameter. For deep hole threads, taps tend to be faster than single-tooth thread mills. If the chips are successfully expelled out of the hole, the tapped hole can be tapped to a depth allowed by the tap design. Since the diameter and pitch are fixed, a tap cannot process screw holes of different specifications. Since the contact area between the tap and the hole wall is large during tapping, and a large cutting force will be generated, the tap may be broken and stuck in the hole, causing the workpiece to be scrapped. Tapping places high demands on lubricants to complete machining efficiently.
Extrusion of Internal Thread:
By transferring workpiece material, extruded taps can machine internal threads up to 4 times the diameter. Since no chips are generated, there is no need to worry about the formation of chip clumps. However, extrusion processing of threads requires that the hardness of the workpiece should be limited to below about HRC40. In addition, due to the need to transfer the material, the workpiece material must have good ductility. Extrusion taps are typically less than 19mm in diameter and can be as small as 0.5mm. The larger the diameter of the tap, the greater the frictional force generated during processing, and the higher the power requirement of the machine tool.
Compared with cutting taps, extruded taps are more rigid and less likely to break. The pressure acting on a cutting tap is a tangential force through its polygonal surface, while the pressure acting on an extrusion tap is a radial force towards the center of the tap and is therefore much greater than the tangential force.
Extruded threads are stronger than machined threads because extruded taps form threads by compressing the grain structure of the workpiece material. Compared with cutting tapping, extrusion tapping requires the machine tool to have greater torque and power, higher requirements for workpiece clamping stability, and the force required to transfer workpiece material is greater than cutting workpiece material. The drilling accuracy requirements for screw holes are also higher.
However, extruded threads are not acceptable in the medical industry and the aerospace industry. The small diameter of the thread formed by extrusion tapping is defective, and the aerospace industry does not allow sharp points at the small diameter of the thread. However, this defect does not affect the tensile strength of the thread, so it is still widely used for general-purpose parts.
Milling of Internal Threads:
Thread milling cutters use helical interpolation to cut internal and external threads, and most CNC machine tools have the function of thread milling. Thread milling can be done with solid carbide thread mills or indexable insert thread mills. Multi-tooth thread mills can cut a full-depth thread with one rotation around the hole, while single-tooth thread mills have cutting edges on only one face, so they can only cut one thread at a time. However, most thread mills have multiple teeth.
Thread milling is suitable for machining workpiece materials with a hardness below HRC65 and has excellent versatility. A variety of workpiece materials can usually be machined with one or two different coating thread mills. Chip control in thread milling is less difficult, and thread milling is an interrupted cut. Broken short chips can be formed regardless of the chip characteristics of the workpiece material. Thread mills cover a wide range of machining sizes, from 0–80-gauge threads to the largest diameter threads. The optimum hole depth suitable for thread milling should be controlled within about 2.5 times the hole diameter. The cutting force of thread milling is not balanced. If the milling length is too large, the large radial cutting force will form a great lateral pressure. This will cause problems such as the deflection of the milling cutter, chipping of the cutting edge, etc., and may even lead to the small size of the milling cutter being broken.
However, single-tooth thread mills can machine deeper tapped holes, even 20 times the depth of the hole. Since all cutting takes place at the end of the cutter, there is no problem with tool deflection. Thread milling has many advantages. A single cutter can machine a series of tapped holes with the same pitch and different diameters, while a single-tooth cutter can machine holes with multiple pitches and diameters. In addition, both blind holes and through holes can be machined with a single thread mill, and both right-hand and left-hand threads can be machined. Because the thread mill is flat-bottomed, it can machine a complete thread close to the bottom of a blind hole. Even if the cutter breaks, it is unlikely that the part will be scrapped, and the thread mill can be combined with other hole-making tools to form a composite tool.
Flat-bottom thread mills produce full threads at the bottom of blind holes. Milling threads have a longer cycle time than tapping. Because milling threads requires special programming, some users may be reluctant to use this machining method. But this kind of program is not complicated and can be compiled with many CNC programming software. Some companies still prefer tapping because they don’t want the operator to intervene in the process, and thread milling requires the operator to make some compensating adjustments to the machine tool. The diameter of the milling cutter will gradually decrease due to normal wear, and to maintain the proper machining size, the operator must compensate for tool wear by adjusting. It is necessary to measure the thread tolerance and adjust the processing parameters according to the measured wear amount. The operator can only test the thread with the gauge regularly. If the test result is unqualified, the tap needs to be replaced.
Turning of Internal Threads:
Another way to machine internal threads is on a multi-spindle machine tool or lathe with an indexable insert or integral mini boring tool. This machining can be done with either single-tooth or multi-tooth inserts. Multi-tooth inserts have multiple teeth on each cutting edge, and each subsequent tooth has a greater depth of cut than the previous one. Using multi-tooth inserts reduces the number of passes required to complete the threading process. However, multi-tooth inserts are more expensive, so they are more advantageous for mass production, but not for small batch processing.
Thread-turning inserts can process both internal and external threads. Internal threads can be turned with integral boring tools. When turning a thread with a single-tooth tool, the user can use a full profile or partial profile insert, which can machine a complete thread profile. Machining with this insert requires a separate insert for each pitch.
Full profile inserts produce stronger and more precise threads in fewer passes than partial profile inserts because the insert can simultaneously produce major, minor, and pitch diameters of the thread. The thread turned by some profile inserts has no crest, and some profile inserts have only one tooth, so threads with different pitches can be machined with different cutting depths. This thread has a sharp crest radius, which reduces the strength of the coarse thread and takes longer for the machine.
Thread turning with indexable tools can be performed in a wide range of sizes, from the largest diameter to tapped holes as small as 6mm. Screw holes with a diameter of less than 6mm need to be machined with solid carbide tools, and the minimum diameter that can be machined can reach about 1.25mm. Thread turning tools with steel shanks are suitable for machining screw holes with a depth of no more than 3 times the diameter of the hole, while thread turning tools with a carbide shank can machine holes with a depth of 4-5 times the diameter of the hole. Thread turning can also process a variety of workpiece materials, and can turn threads on workpieces or superalloys with a hardness of HRC50. However, due to the high hardness and abrasiveness of these materials, tool life can be shortened.
Grinding of Internal Thread:
Thread grinding is a high-precision machining method and an effective choice for precision internal threads with tight tolerances. A variety of internal threads, grooves, bearing races, and other related part features can be machined on a grinder. Typical parts that can be machined with an internal thread grinder include thread ring gauges, roller nuts, ball screws, and more.
Internal thread grinding requires special grinding machines. To grind a thread with a precise tooth profile, the installation position of the grinding wheel of the machine tool must be inclined according to the helix angle of the thread, which requires a rotation axis, and most general-purpose grinders do not have this condition. The A-axis parallel grinding method can be used, and the modified multi-tooth grinding wheel is directly inserted into the workpiece to grind the external thread, but the internal thread grinding requires a single-tooth grinding wheel installed on the A-axis according to the helix angle.
The inner diameter of thread grinding with better processing economy is usually 10-525mm. The rule of thumb for grinding deep hole internal threads is that the ratio of the length to the diameter of the grinding wheel shaft does not exceed 7:1. The challenge in grinding deep-hole internal threads is the mutual constraint between the helix angle and the hole diameter. As the thread length increases and the bore diameter decreases, it is difficult to grind the workpiece with a large helix angle because the grinding axis is more likely to collide with the workpiece. Chip control for internal thread grinding involves flushing the grinding zone with coolant. Also, due to the limited space in the inner hole, it is quite difficult to get the coolant to reach the grinding zone in the direction of rotation of the grinding wheel without preventing the grinding wheel and grinding shaft from entering the small hole.
The machining accuracy of internal thread grinding is high, and the grinding wheel can be accurately reshaped, and after the grinding wheel is formed, it can be quickly reshaped as needed. In addition, internal thread grinding can increase productivity. Grinding wheels can be re-dressed for threads of different shapes without having to replace other grinding wheels. An internal thread grinder with excellent machining performance must have good rigidity and thermal stability, high shaft motion accuracy, accurate closed-loop position feedback, and a temperature-controlled precision spindle.