Machining center milling thread
In this paper, the principle and processing characteristics of milling thread are studied. The factory example is used to illustrate the thread milling macro programming method, which makes the thread processing efficient and convenient. Traditional thread turning and taps and dies have not been able to meet the needs of efficient production. The method of milling the thread adopts the three-axis linkage numerical control machine tool for thread processing, which changes the processing method of the traditional thread, especially for processing large parts, and has achieved good results.
Keywords: machining center milling thread macro program
1 Principle and advantages of thread milling
Milling threads must select a CNC milling machine or machining center that can achieve three-axis linkage. The three-axis linkage milling thread is essentially a full circle in the XY plane. At the same time, the Z axis is reduced by one pitch for each full circle.
Advantages of thread milling:
(1) High processing accuracy and processing efficiency
Milling threading is performed using a three-axis CNC machine tool with a line speed of 80 to 200 m/min and is unaffected by materials.
(2) Good surface quality
Due to the high-speed rotation of the spindle during the thread milling process, the amount of the back-feeding knife is small, and the thread milling cutter blade is sharp, the cutting force generated during milling allows the iron filings to fly away from the workpiece surface quickly, so that a higher surface can be obtained. quality. According to different feed rates, milling parameters such as different speeds, it is also possible to artificially control the surface quality.
(3) Wide processing range and low cost
The same thread milling cutter can process the right-hand thread, and can also process the left-hand thread, that is, the internal thread can be processed, and the external thread can also be processed. Since only the tip portion participates in the milling, after the tool wears out, it can be reworked only by changing to the head block, saving tool costs.
(4) dimensional accuracy is easy to guarantee
During the thread milling process, each tool has a corresponding tool radius compensation value. Roughing, semi-finishing and finishing can be achieved by modifying the tool offset value during machining to obtain better thread size accuracy and surface quality.
(5) Low power requirements of the machine tool
The thread is machined by the tap. Due to the low cutting speed, the tool is all involved in cutting the thread, resulting in a large cutting force and a high torque requirement for the machine tool. Once the cutting speed is high and low, it is easy to cause the tap to break. Because only the tip portion of the thread is partially in contact with the workpiece during thread milling, the cutting force is small, the torque required to mill the thread is small, and the required machine power is much smaller.
(6) Tool breakage is easy to handle
When the tap is used, the tap is easily broken due to large cutting force, poor chip removal, wear, etc. If it is a large hole, it is slightly easier to take out the broken tap from the workpiece, and it is very troublesome if it is a small hole. With thread milling cutters, tool breakage rarely occurs. Once it occurs, it is relatively easy to remove the bad blade because its diameter must be smaller than the diameter of the hole.
(7) blind hole machining full size thread
When the conventional tap is used for threading, since the tap is in the manufacturing process, the bottom of the tap is responsible for the roughing of the thread, so that the tapped bottom of the tap is thicker when the tapping is performed. When using a thread milling cutter for thread milling, due to the blade form of the thread milling cutter, the tip point is not much different from the bottom of the holder, so that the thread is machined to full size during blind hole machining.
2 types of thread milling cutters
Thread milling cutters are divided into two types: machine clamp type and integral type.
(1) Machine-type thread milling cutter can be divided into single-tooth machine clamp and multi-tooth machine clamp thread milling cutter
(1) Single-tooth machine clamp thread milling cutter: The cutter structure is the same as the CNC internal thread turning tool and the blade and the turning tool can be used interchangeably.
(2) Multi-tooth machine clamp thread milling cutter (thread comb): There are multiple thread processing teeth on the blade, and multiple cutter teeth can be threaded at the same time during machining.
(2) Integral thread milling cutter: There are also a number of thread processing teeth on the blade, which is a fixed pitch thread milling cutter. The tool is made of solid carbide and has a high cutting speed and feed rate for a wide range of machining.
3 thread milling examples
The parts shown in Figure 1 are machined, and a single-edge thread milling cutter is used for threading. A general macro program is programmed for thread processing to improve the versatility of the machining and improve the threading efficiency.
Milling of internal threads with a thread milling cutter. Calculate the thread M30×1.5 bottom hole diameter=nominal diameter-1.0825×pitch=30-1.0825×1.5=28.376 mm through hole, the inner hole program is slightly. The milling of the internal thread, the programming origin is selected as the Z zero point on the inner thread hole, and the XY zero point is at the center of each internal thread hole. The internal machining of the four internal threads is completed by the G52 coordinate system offset command. :
O0001; (program name)
M06 T01 G54 G90 G40 M03 S1000 G0 X0 Y0 Z100.; (Program initialization)
Z5.; (quick positioning to the safety plane)
G01 Z0 F40; (tools enter the workpiece surface)
#1=0;(0 is assigned to local variable #1)
N10 #2=#1-1.5; (Assign #1-1.5 to local variable #2)
G42 G01 X-13.Y1.188 D01; (linear plus tool radius compensation)
G02 X0 Y14.188 R13.; (Arc cut)
G02 Z[#2] I-14.188; (Arc import radius)
#1 = #1-1.5;(Calculate loop height)
IF [#1GE-21] GOTO 10; (conditional statement, if #1 is greater than -21, jump to N10 to continue the program)
G02 X13. Y1.188 R13.; (Arc cut out workpiece)
G40 G01 X0; (cancel tool radius compensation)
G00 Z100.; (fast lifting knife)
X0 Y0; (tool returns to zero)
M30; (end of program)
Thread milling has become more and more widely used in machinery manufacturing, and its technology has become more and more mature. This processing method has shown its excellent processing performance, not only reduces the processing cost, but also greatly improves the processing efficiency and provides a powerful manufacturing. Protection. The use of a highly versatile macro program for thread milling makes it easier and more efficient to machine threads, which is a solution to the problem of thread machining.
If you have any mechine parts needs, please contact us:contact
If you want to see more CNC precision products, please click here： Product
If you want to see more news:News
Check out the latest company news on Twitter：twitter:@QianJmechanical