There are certain technical difficulties in machining trapezoidal threads on CNC lathes, especially in high-speed cutting. It is not easy to observe and control during machining, and the safety and reliability are also poor. This requires correct tool geometry and processing technology. An efficient and feasible processing method is introduced.
Whether on an ordinary lathe or on a CNC lathe, there is always a great technical difficulty in processing trapezoidal threads for students in secondary and higher vocational schools, especially in the high-speed turning of trapezoidal threads on a CNC lathe. Most books and textbooks do not introduce special topics. It is difficult for students to master their fine calculation and reasonable processing technology. The author will focus on the high-speed turning method of trapezoidal thread according to the examination questions of senior workers in Hunan Province in recent years and in combination with his own experience and experience.
1、 Selection of processing methods
As shown in Figure 1, when machining trapezoidal threads on the CNC lathe, the three jaw chuck adopts the method of one clamp and one top. For the convenience of tool setting and programming, the program origin is set at the center point of the right end face of the workpiece. In addition, a tool setting template is also made to facilitate the accuracy of the Z direction when changing tools in rough and fine turning. It should be pointed out that because of the high-speed machining of trapezoidal threads, cemented carbide tools are selected.
When turning trapezoidal thread at high speed, due to the excessive thread pitch, in order to prevent "knife pricking" and "blade breakage", it is required that the cutting force should not be too large when machining trapezoidal thread, and the tool should not cut on three sides at the same time. Through years of practice, the author has proved that the straight cutting method or straight grooving method can not be used for processing with thread cutting commands G32 and G92 on the economic NC lathe. Even though the method of using G92 combined with the left and right swing of subprogram introduced in many magazines in recent years is not the best method for layered cutting. Although this method theoretically can reduce the force during cutting, it ignores that most of our commonly used lathes are economic NC lathes, However, the control system of economical CNC lathe is semi closed loop, so that the servo system can not keep up with the numerical requirements of the CNC system when swinging left and right, thus changing the machining pitch. Considering the comprehensive programming and processing, combined with practical experience, I think it is a better, safe, reliable and easy method to use the thread cutting compound cycle command G76 to process.
2、 Introduction to G76 instruction
G76 instruction is oblique cutting. Because of single side edge machining, the tool load is small, chip removal is easy, and the cutting depth is decreasing. General large pitch thread processing.
1. G76 command's feed route and feed distribution. (Figure 2)
Group diagram: schematic diagram of trapezoidal thread processing parameters
Feed rate per time=h/√ n-1 × √ ¢, where h is the total height of the thread, n is the number of feedings, ¢ is the first feedrate=△ d, is the second feedrate=1, and the third and more feedrates=X-1
2. Format:
G76 P（m）（r）（a） Q（⊿dmin） R（d）
G76 X（U） Z（W） R（i） P（k） Q（⊿d ） F(L)
Including:
M - number of finishing repetitions, which can be 1-99 times.
R - chamfer amount at the end of thread (oblique tool retraction), 00-99 units, taking 01, it is 0.11 × Lead.
A - Angle of thread tip (thread profile angle). 80, 60, 55, 30, 29 and 0 degrees can be selected.
△ dmin - minimum back cut during cutting, radius value, μ m.
D - finishing allowance, radius value, mm.
I - Radius difference of thread part, radius value, μ m.
K - thread depth, h=0 65 × Pitch (P) calculation, microns.
△ d - first cutting depth, radius value, μ m.
L - Thread lead, micrometer.
3、 Selection of tool geometry
According to the conditions of high-speed turning trapezoidal thread, the helix angle is calculated first, so that the geometric angle of the tool can be grinded correctly. The helix angle is a=[P/(d)]=arctan [5/(3.14 × 25.5)]=3.82, so it is appropriate to select 6-8 degrees for the left rear corner and 2 degrees for the right rear corner; In order to facilitate chip removal, the tool is not easy to be damaged. The front angle is 6-8 degrees, making the tool sharper and conducive to chip breaking. It is particularly pointed out that I have used two tools for rough and fine turning. As rough machining is easy to damage and wear the turning tool, I grind the sharp corner edge of the rough turning tool into an arc shape, which can strengthen the strength of the tool tip. Even if the rough machining amount is too large, there is a certain safety factor, while the finish machining is completely in accordance with the thread shape. Attention should be paid to the accuracy of zero point when setting the rough and finish turning tools in Z direction. The geometric shapes of rough and finish turning tools are as follows:
4、 Preparation of procedures.
This article only describes the programming of trapezoidal thread, as follows:
%0003;
N10 G90 G95;
N20 M3 S350 T0505;
N30 G0 X35. Z-10.;
N40 G76 P020030 Q20 R0.02
G76 X22.3 Z-94. P2750 Q329 F5.
N50 G0 X120. Z200.;
N60 M5;
N70 M30;
5、 Precautions for processing with thread compound cutting cycle G76.
When machining trapezoidal thread with CNC lathe, due to the change of its transmission chain, in principle, its speed should be able to ensure that when the spindle rotates for one cycle, the tool will shift a lead along the direction of the main feed shaft, which should not be limited, but will be affected by the following aspects:
1. The screw pitch/lead value of the command in the thread processing program section is equivalent to the feed speed expressed in the feed rate per revolution. If the spindle speed of the machine tool is selected too high, the converted feed speed must greatly exceed the maximum feed rate allowed by the machine tool parameters. At this time, the machine tool will process according to the "limit screw pitch" (limit screw pitch=maximum feed rate/speed).
2. The tool will be constrained by the frequency rise/fall of the servo drive system and the interpolation speed of the NC device throughout its displacement. The pitch of some threads may not meet the requirements due to the "lead" and "lag" caused by the main feed motion due to the reason that the frequency rise/fall characteristic cannot meet the processing requirements; The thread turning must be realized by the synchronous operation function of the spindle, that is, the spindle pulse generator encoder is required for thread turning. When the spindle speed is too high, the positioning pulse sent by the encoder (that is, a reference pulse signal sent out when the spindle rotates for one cycle) may cause "overshoot", especially when the quality of the encoder is unstable, which will cause the thread of the workpiece to be disorderly buckled.
Therefore, when turning trapezoidal thread, the spindle speed shall be selected according to the following principles:
1. Under the condition of ensuring production efficiency and normal cutting, the maximum processing speed should be obtained according to the calculation formula of "limit pitch", and the lower spindle speed should be selected;
2. When the lead in length and cut out length in the thread processing program section are small, relatively low spindle speed is selected;
3. When the allowable working speed specified by the encoder exceeds the maximum spindle speed specified by the machine tool, a higher spindle speed can be selected as far as possible;
4. In general, the spindle speed during thread turning shall be determined according to the calculation formula specified in the machine tool or NC system manual.
It should also be noted that:
1. As the spindle speed may change and the correct thread pitch may not be cut, do not use the constant surface cutting speed control command G96 during thread cutting.
2. During thread cutting, the feed rate multiplier is invalid (fixed at 100%), and the speed is fixed at 100%.
3. Chamfer or rounding cannot be specified in the previous segment of the thread cutting segment.
4. Generally, due to the hysteresis of the servo system and other reasons, incorrect leads will be generated at the starting and ending points of thread cutting. Therefore, the starting and ending points of the thread should be longer than the specified thread length.
