Real Thing Sharing: Methods of CNC High-Speed Turning Trapezoidal Threads

Machining trapezoidal threads on CNC lathes have certain technical difficulties, especially in high-speed cutting. It is not easy to observe and control during processing, and its safety and reliability are also poor. This requires correct tool geometry and processing technology. Today, YIJIN Hardware introduces an effective and feasible method of trapezoidal thread processing.

Regardless of whether it is on a normal lathe or a CNC lathe, machining trapezoidal threads are always difficult for general technicians, especially for high-speed turning of trapezoidal threads on a CNC lathe. Most books and textbooks do not cover topics. Therefore, it is difficult to grasp its fine calculation and reasonable Trapezoidal Threads processing technology.

Methods of CNC High-Speed Turning Trapezoidal Threads

Selection of Machining Process

As shown in Figure 1, when machining trapezoidal threads on a CNC lathe, the three-jaw chuck adopts the one-clamp and one-top method. For the convenience of tool setting and programming, the program origin is set at the center point of the right end surface of the workpiece. A self-made tool setting template is also made to facilitate the accuracy of the Z direction when changing the tool for rough and fine turning. It should be pointed out that, because it is high-speed processing trapezoidal thread, so the choice of carbide tool.

When turning the trapezoidal thread at high speed, because the pitch is too large, in order to prevent the phenomenon of “breaking edge” and “tipping”, the cutting force can not be too large when processing the trapezoidal thread, and the tool can not cut on three sides at the same time. YIJIN Hardware through many years of practice has proved that the economical CNC lathe cannot be used on the thread cutting instructions G32, G92, transferring to straight entered or straight into the method of grooving to processing, even if many magazines in recent years have been introduced about using G92 combines the subroutine of the swing method for layered cutting is not the best method, although in theory, this method when the cutting force is small, but it ignores that most of our commonly used lathes are economical CNC lathes. The economical CNC lathe control system is a semi-closed loop so that the servo system cannot keep up with the numerical requirements of the CNC system when it swings around so that the processing pitch changes. Considering comprehensive programming and machining, combined with practical experience, our company believes that using thread cutting compound cycle instruction G76 to process is a better effect, safe, reliable, and feasible method.

Introduction To The G76 Directive

G76 instruction is inclined to cut, because of the unilateral edge processing, the tool load is small, chip removal is easy, and the thread cutting depth is decreasing. General use of large pitch thread processing.

1. G76 instruction of tool feeding route and tool feeding distribution, shown in Figure 2.

G76 instruction of tool feeding route and tool feeding distribution

G76 instruction of tool feeding route and tool feeding distribution

G76 thread cutting compound cycle instruction process demonstration

G76 thread cutting compound cycle instruction process demonstration

Photos: Trapezoidal thread processing each parameter schematic

Photos: Trapezoidal thread processing each parameter schematic

Feed per time=h/√n-1×√¢, H is the total height of the threaded teeth,n is the number of feeds,¢ refers to the fist feed=⊿d, s is the second feed=1, the third and more feeds=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—Finishing repeat times, can be 1~99 times.

r—Chamfering of thread tail(Inclined to return),00~99 units, if 01 is taken, 0.11× lead retreats.

a—Angle of the threaded tooltip(Thread profile angle).80, 60, 55, 30, 29, 0 degrees can be selected.

⊿dmin—Minimum amount of back cutting tool, radius values, micron.

d— allowance for the finish, radius values, millimeter.

i—Radius difference of thread part, radius values, micron.

k—Depth of thread, calculate according to h=0 65×pitch (P), micron.

⊿d—The first deep cut, radius values, micron.

L—a lead of screw thread, micron.

Tool Geometry Selection

According to the condition of high-speed turning trapezoidal thread, the spiral Angle is calculated first in order to correctly grind the geometric Angle of the tool. Helical angle a=[P/(d)]=arctan[5/(3.14×25.5)]= 3.82, therefore, it is more appropriate to choose 6-8 degrees for the left rear angle and 2 degrees for the right rear angle; In order to facilitate chip removal and the tool is not easy to damage, the rake angle is 6-8 degrees to make the tool sharper and conducive to chip breaking. It is especially pointed out that our company uses two tools for rough and fine turning. It is easy to turn the tool due to rough machining. Damage and wear, so our company grinds the rough turning tooltip angle into a circular arc shape, which can strengthen the strength of the tooltip, even if the roughing amount is too large, there is a certain insurance coefficient, and the finishing process is completely in accordance with the thread shape. Attention should be paid to the accuracy of the zero point of rough and fine turning tool Z direction. The geometric shapes of rough and fine turning tools are as follows:

The geometric shapes of rough and fine turning tools

The geometric shapes of rough and fine turning tools

Programming

This article only talks about the compilation of the trapezoidal thread part of the program, 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;

Points Needing Attention When Using Thread Compound Cutting Cycle G76

1) When machining trapezoidal threads on a CNC lathe, due to the change of its transmission chain, in principle, its speed can ensure that the tool moves one lead in the direction of the main feed axis for each revolution of the spindle. It should not be restricted, but will be affected by the following aspects:

The pitch/lead value of the instructions in the thread machining program section is equivalent to the feed speed expressed by the feed per revolution. If the spindle speed of the machine tool is selected too high, the feed speed after conversion must greatly exceed the maximum feed allowed by the parameters of the machine tool.

At this time, machine tools will be processed in accordance with the “limit pitch” (limit pitch = maximum feed/speed).

2) The tool will be constrained by the up/down frequency of the servo drive system and the interpolation operation speed of the CNC device during its displacement. Because the rising/falling frequency characteristics can not meet the machining needs, the pitch of some screw teeth may not meet the requirements due to the “advance” and “lag” caused by the main feed movement. The turning thread must be realized through the synchronous operation function of the spindle, that is, the turning thread requires the spindle pulse generator encoder. When the spindle speed is selected too high, the positioning pulse sent by the encoder (that is, a reference pulse signal sent every time the spindle rotates) may “overshoot”, especially when the quality of the encoder is unstable. Lead to random buckles in the thread of the workpiece.

Therefore, when turning trapezoidal threads, the spindle speed selection should follow the following principles:

①Under the condition of ensuring production efficiency and normal cutting, the maximum machining speed should be obtained according to the calculation formula of “limit pitch”, and the lower spindle speed should be selected;

②When the lead-in length and the cut-out length in the thread processing block are small, choose a relatively low spindle speed;

③When the allowable working speed specified by the encoder exceeds the maximum speed of the spindle specified by the machine tool, a higher spindle speed can be selected as much as possible;

④Under normal circumstances, the spindle speed during threading should be determined according to the calculation formula specified in the machine tool or CNC system manual.

Also, Note:

①As the spindle speed changes, the correct pitch may not be cut, so do not use the constant surface cutting speed control command G96 during thread cutting.

②During thread cutting, the feed rate is invalid (fixed at 100%) and the speed is fixed at 100%.

③Chamfering or rounding cannot be specified in the preceding section of a thread cutting section.

④Generally, due to the lag of the servo system, an incorrect lead will be generated at the start and end of thread cutting. Therefore, the start and end positions of the thread should be longer than the specified thread length.

We hope this information will help you. For more new information Click Here and get the YIJIN Hardware expert’s help.

Thank you for reading.

 

Leave a Reply

Get a quote
Email
Phone