xiehe model

Common thread machining methods in CNC machining centers

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

With the improvement of the performance of CNC machining centers and the improvement of tools, the method of threading has been continuously improved, and the accuracy and efficiency of threading have also been gradually improved. In order to make the technicians reasonably choose the thread processing method in processing, improve the production efficiency and avoid quality accidents, several thread processing methods commonly used in the practice of CNC machining centers are summarized as follows:

Tap processing method

1 Classification and characteristics of tap processing

Using a tap to machine a threaded hole is the most common machining method. It is mainly suitable for threaded holes with small diameter (D<30) and low hole position accuracy.

In the 1980s, the threaded holes all adopted the flexible tapping method, that is, the flexible tapping chuck was used to clamp the tap. The tapping chuck can be used for axial compensation to compensate for the feed caused by different step feeds and spindle speeds of the machine tool. Errors are given to ensure correct pitch. The flexible tapping chuck has 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 and remain unchanged.

Compared with flexible tapping chucks, spring chucks are simple in structure, low in price and widely used. 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 the manufacturing cost.

2 Determination of threaded bottom hole before tapping

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

For example, the diameter of the bottom hole of the M8 threaded hole is Ф6.7+0.27mm, and the diameter of the drill bit 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 improved.

3 Choice of taps

When choosing a tap, first select the corresponding tap according to the material to be processed. Tool companies produce different types of taps depending on the material being processed. Pay special attention to selection.

Compared with milling cutters and boring tools, taps are very sensitive to the machining material. For example, machining aluminum parts with taps for processing cast iron can easily cause threads to fall off, snap or even break the taps, resulting in scrapped workpieces. Second, pay attention to the difference between through-hole taps and blind-hole taps. The front end of the through hole tap is longer, and the chip removal is the front end chip removal. The front end of the blind hole is short, and the chip evacuation is rear chip evacuation. For blind holes with through-hole taps, the threading depth cannot be guaranteed. In addition, if using a flexible tapping chuck, 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 selection of taps can ensure the smooth progress of processing.

4 NC programming for tapping

The programming of tapping processing is relatively simple. Now the machining center generally solidifies the tapping subroutine, and only needs to assign values to each parameter. However, it should be noted that due to different CNC systems, the subprogram formats are different, and the meanings of some parameters are also different.

For example, 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.

Threading

Thread milling

1 Characteristics of thread milling

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

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

⑴ Fast processing speed, high efficiency and high processing precision. The tool material is generally cemented carbide material, and the cutting speed is fast. The tool is manufactured with high precision, so the thread milling precision is high.

⑵ The milling cutter has a wide range of applications. As long as the pitch is the same, whether it is a left-hand thread or a right-hand thread, one tool can be used, which is beneficial to reduce tool costs.

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

⑷ Since there is no tool lead, it is suitable for processing blind holes with short threaded bottom holes and holes without undercuts.

2 Classification of thread milling cutters

Thread milling cutters can be divided into two types, one is a machine-clamped carbide insert milling cutter, and the other is an integral carbide milling cutter. Machine tool fixtures have a wide range of applications. It can machine holes with a thread depth less than the insert length, or holes with a thread depth greater than the insert length. Solid carbide milling cutters are generally used to machine holes with a thread depth less than the tool length.

3 CNC programming for thread milling

Programming of thread mills is different from programming of other tools. If the machining program is programmed incorrectly, it is easy to cause tool damage or thread machining errors. When compiling, pay attention to the following points:

⑴ First of all, the threaded bottom hole should be processed well, the small diameter hole should be processed with a drill bit, and the larger hole should be drilled to ensure the accuracy of the threaded bottom hole.

(2) When cutting in and out, the tool should adopt a circular arc trajectory, generally 1/2 circle for cutting in or cutting out, and 1/2 pitch in the Z-axis direction to ensure the shape of the thread. In this case, the tool radius compensation value should be brought in.

⑶ X, Y axis circular interpolation, the spindle should move one pitch along the Z axis direction, otherwise it will cause random teeth.

⑷ Specific example program: the diameter of the thread milling cutter is Φ16, the threaded hole is M48×1.5, and the depth of the threaded hole is 14.

The handler is as follows:

(The threaded bottom hole program is omitted, and the hole should be a drilled 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 and add radius compensation

G03 X24 Y0 Z-14 I20 J0 F500 Use 1/2 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 When cutting out, use 1/2 arc to cut out G01 G40 X0 Y0 Return to center, cancel radius compensation

G0 Z100

M30

Pick

1 Features of Pick method

Sometimes large threaded holes are encountered on box parts. In the absence of taps and thread mills, a method similar to lathe pick-up can be used.

Install the thread turning tool on the boring bar for thread boring.

The company used to process a batch of parts, the thread is M52x1.5, and the position is 0.1mm (see Figure 1). Due to the high position requirements and the large threaded hole, it is impossible to use a tap to process it, and there is no thread milling cutter. After testing, the grabbing method was adopted. , to ensure the processing requirements.

2 Precautions for picking methods

⑴ After the spindle starts, there should be a delay time to ensure that the spindle reaches the rated speed.

(2) When retracting the tool, if it is a hand-grinding thread tool, since the tool cannot be sharpened symmetrically, reverse retraction cannot be used. The spindle must be oriented, the tool moves radially, and the tool retracts.

⑶ The manufacture of the tool holder must be accurate, especially the slot positions must be consistent. If they are inconsistent, multi-toolbar processing cannot be used. Otherwise, random points will be deducted.

⑷ Even if the buckle is very thin, it cannot be cut across the board when picking it, 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.