Common Thread Machining Methods For CNC Machining Centers

Thread machining is one of the very important applications of CNC machining centers. The machining quality and efficiency of threads will directly affect the machining quality of parts and the production efficiency of machining centers.

With the improvement of the performance of cnc machining centers and the improvement of cutting tools, the methods of thread processing are constantly improving, and the accuracy and efficiency of thread machining are gradually improving. In order to enable technologists to reasonably choose thread processing methods in processing, improve production efficiency and avoid quality accidents, several thread machining methods commonly used in cnc machining centers in practice are summarized as follows:

Tap Machining Method

1 Classification And Characteristics Of Tap Processing

Using taps to process threaded holes is the most common processing method. It is mainly suitable for threaded holes with small diameters (D<30) and low hole position accuracy.

In the 1980s, threaded holes all adopted flexible tapping methods, that is, flexible tapping chucks were used to clamp the taps. The tapping chucks could be used for axial compensation to compensate for the advance caused by the asynchronous feed of the machine tool and the spindle speed. Give the error to ensure the correct pitch. The flexible tapping chuck has a complex structure, high cost, easy damage, and low processing efficiency. In recent years, the performance of cnc machining centers has gradually improved, and rigid tapping has become the basic configuration of cnc machining centers.

Therefore, rigid tapping has become the main method of thread processing at present.

That is, the tap is clamped by a rigid spring chuck, and the spindle feed and spindle speed are controlled by the machine tool to keep the same.

Compared with the flexible tapping chuck, the spring chuck has a simple structure, low price, and a wide range of uses. In addition to clamping taps, it can also clamp end mills, drills and other tools, which can reduce tool costs. At the same time, rigid tapping can be used for high-speed cutting, which improves the efficiency of the machining center and reduces manufacturing costs.

2 Determination Of The Threaded Bottom Hole Before Tapping

The processing of the threaded bottom hole has a great influence on the life of the tap and the quality of thread processing. Generally, the diameter of the threaded bottom hole drill bit is selected close to the upper limit of the threaded bottom hole diameter tolerance.

For example, the diameter of the bottom hole of the M8 threaded hole is Ф6.7+0.27mm, and the drill bit diameter is Ф6.9mm. In this way, the machining allowance of the tap can be reduced, the load of the tap can be reduced, and the service life of the tap can be increased.

3 Selection Of Taps

When selecting a tap, first of all, you must select the corresponding tap according to the material to be processed. The tool company produces different types of taps according to the different materials to be processed. Pay special attention to the selection.

Compared with milling cutters and boring cutters, taps are very sensitive to the processed materials. For example, using taps for machining cast iron to process aluminum parts can easily cause thread loss, random buckles or even tap breaks, resulting in scrapped workpieces. Secondly, pay attention to the difference between through-hole taps and blind-hole taps. The leading end of the through-hole taps is longer, and the chip removal is the front chip removal. The leading end of the blind hole is shorter, and the chip removal is rear chip removal. For blind holes with through-hole taps, the thread processing depth cannot be guaranteed. Furthermore, if a flexible tapping chuck is used, the diameter of the tap shank and the width of the square should be the same as that of the tapping chuck; the diameter of the shank of the tap for rigid tapping should be the same as the diameter of the spring collet. In short, only a reasonable choice of taps can ensure smooth processing.

4 CNC Programming For Tap Processing

The programming of tap processing is relatively simple. Now the machining center generally solidifies the tapping subroutine, and only needs to assign each parameter. But it should be noted that, because the numerical control system is different, the subroutine format is different, and the meaning of some parameters is different.

For example, for the SIEMEN840C control system, its programming format is: G84 X_Y_R2_ R3_R4_R5_R6_R7_R8_R9_R10_R13_. Only these 12 parameters need to be assigned during programming.

thread machining

Thread Milling

1 Features Of Thread Milling

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

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

⑴ High processing speed, high efficiency and high processing precision. The tool material is generally hard alloy material, and the cutting speed is fast. The manufacturing precision of the tool is high, so the thread milling precision is high.

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

⑶ Milling is easy to remove chips and cool. Compared with taps, the cutting performance is better. It is especially suitable for thread processing of aluminum, copper, stainless steel and other difficult-to-machine materials. It is especially suitable for thread processing of large parts and components of precious materials. Ensure the quality of thread processing and the safety of the workpiece.

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

2 Classification Of Thread Milling Tools

Thread milling tools can be divided into two types, one is a machine-clamped cemented carbide blade milling cutter, and the other is an integral cemented carbide milling cutter. The machine clamp tool has a wide range of applications. It can process holes with a thread depth less than the length of the blade, or holes with a 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.

3 CNC Programming Of 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 machining errors. Pay attention to the following points 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 cutting in and out, the tool should adopt the arc trajectory, 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 week, 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 procedure 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 in

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



1 The Characteristics 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 lathe picking can be used.

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

The company used to process a batch of parts, the thread is M52x1.5, the position is 0.1mm (see Figure 1), because the position requirements are high, the threaded hole is large, it is impossible to use taps for processing, and there is no thread milling cutter, after testing , The pick-and-button method is used to ensure the processing requirements.

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 the tool is retracted.

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.

3 Specific Example Procedures

N5 G90 G54 G0 X0 Y0

N10 Z15

N15 S100 M3 M8

N20 G04 X5 delay to make the spindle reach the rated speed

N25 G33 Z-50 K1.5 Buckle

N30 M19 Spindle orientation

N35 G0 X-2 Giving knife

N40 G0 Z15 Retract tool

Leave a Reply

Your email address will not be published. Required fields are marked *