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

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

Machining trapezoidal threads on CNC lathes has 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 to introduce 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 is 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 processing technology.

Trapezoidal Threads, Thread Cutting, High-Speed Turning

Selection of Machining Process

As shown in Figure 1, when machining trapezoidal threads on a CNC lathe, the three-jaw chuck adopts 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 practice has proved that the economical CNC lathe cannot be used on the thread cutting instructions G32, G92, transfering to straight entered or straight into the method of grooving to processing, even if many magazines in recent years is 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.

Trapezoidal Threads, Thread Cutting, High-Speed Turning

Introduction To The G76 Directive

G76 instruction is inclined cutting, because of the unilateral edge processing, the tool load is small, chip removal is easy, and the 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.Trapezoidal Threads, Thread Cutting, High-Speed Turning

G76 instruction of tool feeding route and tool feeding distribution

Annealing, Normalizing, Quenching, Tempering

G76 thread cutting compound cycle instruction process demonstration

Trapezoidal Threads, Thread Cutting, High-Speed Turning

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,¢ refer 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 is retreated.

a—Angle of threaded tool tip(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 finish, radius values,millimetre.

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—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 tool tip angle into a circular arc shape, which can strengthen the strength of the tool tip, 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 zero point of rough and fine turning tool Z direction.The geometric shapes of rough and fine turning tools are as follows:

Trapezoidal Threads, Thread Cutting, High-Speed Turning

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 servo drive system and the interpolation operation speed of 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.

Trapezoidal Threads, Thread Cutting, High-Speed Turning

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 YIJIN Hardware experts help. 

Now if you find this information helpful, share it with your friends, family, and colleagues.

If you like this post, let us know by comment below, if you want to add-on information about this topic, comment the information. We will consider the information if it is relevant.

Thank you for reading.

2022-01-20T17:33:08+08:00