Introduce several thread processing methods commonly used in CNC machining centers(2)

　2. CNC thread milling method

　　2.1 Features of thread milling

　　 Thread milling is the use of thread milling tools, three-axis machining center linkage, that is, X, Y axis arc interpolation, Z axis linear feed milling method to process threads.

　　Thread milling is mainly used for the processing of large hole threads and threaded holes of difficult-to-machine materials. It mainly has the following characteristics:

　　⑴ Fast processing speed, high efficiency and high processing precision. The tool material is generally cemented carbide material, and the tool travel speed is fast. The manufacturing precision of the tool is high, so the thread precision of milling is high.

　　⑵ The range of milling tools is wide. As long as the pitch is the same, no matter whether it is a threaded thread or a right-hand thread, one tool can be used, which is helpful to reduce the cost of the tool.

　　⑶ Milling is easy to remove chips and cool, and has better cutting conditions than taps. It is especially suitable for thread processing of difficult-to-machine materials such as aluminum, copper, and stainless steel.

　　 is especially suitable for the thread processing of large parts and parts of precious materials, which can ensure the quality of thread processing and the safety of the workpiece.

　　⑷ Because there is no tool tip guide, it is suitable for processing blind holes with short threaded bottom holes and holes without undercuts.

　　2.2 Classification of thread milling tools

　　 Thread milling tools can be divided into two types, one is a machine-clamped carbide blade milling cutter, and the other is a solid carbide milling cutter. The machine clamp tool has a wide range of applications. It can process holes with thread depth less than the length of the blade, or holes with thread depth greater than the length of the blade. Integral carbide milling cutters are generally used to machine holes with thread depth less than the tool length.

　　2.3 CNC programming for thread milling

　　 The programming of thread milling tools is different from the programming of other tools. If the machining program is programmed incorrectly, it is easy to cause tool damage or thread processing errors. The following points should be noted when compiling:

　　⑴ First of all, the threaded bottom hole should be processed well, the small diameter hole should be processed with a drill, and the larger hole should be boring to ensure the accuracy of the threaded bottom hole.

　　⑵ When the tool cuts in and cuts out, the arc trajectory should be adopted, usually 1/2 circle for cutting in or out, and the Z-axis direction should travel 1/2 pitch to ensure the thread shape. The tool radius compensation value should be brought in at this time.

　　 ⑶ X, Y axis circular interpolation one circle, the spindle should travel a pitch along the Z axis direction, otherwise, it will cause random threading.

　　⑷ Specific example program: thread milling cutter diameter is Φ16, threaded hole is M48×1.5, threaded hole depth is 14.

　　The processing procedure is as follows:

　　 (The threaded bottom hole program is omitted, the hole should be boring bottom hole)

　　 G0 G90 G54 X0 Y0

　　 G0 Z10 M3 S1400 M8

　　 G0 Z-14.75 infeed to the deepest thread

　　 G01 G41 X-16 Y0 F2000 Move to the feed position, add radius compensation

　　 G03 X24 Y0 Z-14 I20 J0 F500 Use 1/2 circle arc when cutting

　　 G03 X24 Y0 Z0 I-24 J0 F400 Cut the entire thread

　　 G03 X-16 Y0 Z0.75 I-20 J0 F500 Cut out with 1/2 circle arc when cutting out G01 G40 X0 Y0 Return to the center, cancel radius compensation G0 Z100 M30

　　3. Pick button method

　　3.1 Features of the pick method

　　 Sometimes large threaded holes can be encountered on box parts. In the absence of taps and thread milling cutters, a method similar to that of a lathe can be used.

　　 Install a thread turning tool on the boring bar to boring threads.

　　3.2 Precautions for picking method

　　⑴ After the spindle starts, there should be a delay time to ensure that the spindle reaches the rated speed.

　　⑵ When retracting, if it is a hand-ground threaded tool, since the tool cannot be sharpened symmetrically, reverse retraction cannot be used. The spindle must be oriented, the tool moves radially, and then retract.

　　⑶ The tool holder must be manufactured accurately, especially the slot position must be consistent. If they are inconsistent, multi-tool bar processing cannot be used. Otherwise it will cause random deductions.

　　⑷ Even if it is a very thin buckle, it cannot be made with one cut when picking the buckle, otherwise it will cause tooth loss and poor surface roughness. At least two cuts should be made.

　　⑸ The processing efficiency is low, and it is only suitable for single-piece small batches, special pitch threads and no corresponding tools.

　　 4. Summary

　　 To sum up, the methods of CNC machining threads mainly include tap processing, milling processing and picking method. Tap processing and milling are the main processing methods. The picking method is only a temporary emergency method.

　　Only by correctly selecting thread processing methods and processing tools, can the efficiency and quality of thread processing be effectively improved, the use efficiency of cnc processing can be improved, and the processing cost should be reduced. Every CNC processing technician should be proficient.