The traditional thread processing method uses tap to tap the thread, which is inefficient and difficult to ensure the thread processing accuracy, and it is very easy to scrap the workpiece after the tap is broken.
In modern thread machining, milling method has been gradually adopted to replace the traditional machining method.
It has the advantage of high machining efficiency.
The machining accuracy of thread can be well controlled by selecting cutting tools and adjusting machining parameters;
The tool has good versatility.
For the threaded holes with the same pitch and different diameters, it needs more than one tool to process the tap.
However, if the thread milling tool is used, one tool can be used;
With high processing safety, the spiral interpolation milling method does not need to worry about the negative effects caused by tool damage.
The thread milling is shown in fig. 5-87.
Fig. 5-87 schematic diagram of thread milling
（1） Characteristics and application of thread milling
As a new thread processing technology, thread milling has unique advantages and more flexible use and applications than tapping.
(1) High processing efficiency.
The thread milling cutter not only has high milling speed, but also its multi groove design increases the number of cutting edges, which can easily improve the feed speed, which can greatly improve the machining efficiency.
In the processing of long thread, the blade with longer cutting edge can be selected to reduce the axial feed distance (equivalent to shortening the thread) to further improve the processing efficiency.
(2) High surface quality and dimensional accuracy.
The thread milling cutter has a high cutting speed, and a small cutting force makes the cutting surface very smooth;
The fine chips can be easily flushed out of the workpiece by the cutting fluid without scratching the machined surface.
It is suitable for the workpiece with high thread accuracy requirements.
(3) Good stability, safe and reliable.
Because the thread milling cutter is gradually cutting into the material, it produces less cutting force and rarely breaks the cutter.
Even if there is a broken cutter, because the diameter of the milling cutter is much smaller than the threaded hole, the broken part can be easily removed from the part without damaging the part.
(4) Wide range of applications.
The thread milling cutter is flexible to use and can be applied to a variety of working conditions.
For example, the same thread milling cutter can be used to process left-hand thread or right-hand thread;
Both external and internal threads can be machined.
The diameter of the thread milling cutter is smaller than that of the hole, and the cutter must be reversed to obtain a complete and accurate thread depth.
Thread milling is a new advanced processing technology with a wide range of applications, but it also has certain limitations:
1) A 3-axis CNC machine tool is required.
2) Although its cost is lower than tap in batch processing, a single thread milling cutter is more expensive than tap.
3) The programming of thread milling is troublesome, which is one of the important factors that limit its wide application.
（2） Selection of thread milling cutter
With the popularization of CNC machine tools, thread milling technology is more and more used in the mechanical manufacturing industry.
Thread milling is to use the 3-axis linkage of the NC machine tool to perform spiral interpolation milling with the thread milling cutter to form the thread.
Each cycle of circular motion of the cutter on the horizontal plane moves a pitch in a straight line in the vertical plane.
At present, there are many kinds of thread milling cutters used.
The characteristics of several common thread milling cutters are as follows.
1. Ordinary clamp type thread milling cutter
The clamp type thread milling cutter is mainly used for milling large diameter internal threads and external threads.
Because the blade is easy to manufacture and low in price, its impact resistance is slightly worse than that of the integral thread milling cutter.
Therefore, the tool is often recommended for processing aluminum alloy materials.
Its structure is similar to that of ordinary machine clamp milling cutter, and it is composed of reusable cutter bar and easily replaceable blade.
When selecting the clamp type thread milling cutter, the cutter bar with larger diameter and the material of appropriate blade shall be selected as far as possible according to the diameter, depth and workpiece material of the processed thread.
As shown in fig. 5-88, it is an ordinary multi edge machine clamp thread milling cutter.
Fig. 5-88 ordinary multi edge machine clamp thread milling cutter
2. Clamp type thread comb milling cutter
As shown in fig. 5-89, the thread comb milling cutter is mainly used to process triangular internal cylindrical threads and conical threads with short length and small pitch.
Pay attention to the selection of milling cutter diameter when selecting the thread comb milling cutter.
The contact arc between the milling cutter and the workpiece is very small, and the expansion of the tooth groove of the workpiece is not obvious.
It is best to choose a milling cutter with larger diameter, but considering the factors such as manufacturing convenience and economy, it is not suitable to choose a milling cutter with larger diameter.
When milling the internal thread, the contact arc between the milling cutter and the workpiece is longer, and with the increase of the diameter of the milling cutter, the contact arc will increase significantly, and the expansion of the thread slots will increase significantly.
Therefore, the milling cutter with appropriate diameter should be selected.
If the milling cutter diameter is not selected properly, the accuracy of thread profile will be affected.
When machining different materials, the rake angle and addendum rake angle of the thread comb milling cutter are also different (see table 5-23).
Fig. 5-89 thread comb milling cutter
Table 5-23 geometric parameters of thread comb milling cutter
|
Parameter |
Workpiece material |
||
|
Hard steel |
Medium mild steel and brass |
Aluminum and light alloy |
|
|
Front angle y0（°） |
0~4 |
8 |
22 |
|
Addendum rear angle a0（°） |
8~12 |
8~12 |
8~12 |
According to the different materials of the machined parts, the cutting parameters of the thread comb milling cutter are also different.
The selection of cutting parameters for parts with different materials is shown in table 5-24.
Table 5-24 selection of cutting parameters for parts with different materials
| Material of machined parts | Feed rate per tooth fz/ (mm/z) | Cutting speed vc/ (m/min) |
| Carbon steel | 0.05~0.23 | 150~330 |
| Stainless steel | 0.05~0.16 | 135~220 |
| Cast iron | 0.05~0.23 | 130~220 |
| Superalloy | 0.05~0.10 | 25~60 |
Note: the above cutting parameters can be adjusted according to the actual machining.
3. Ordinary integral thread milling cutter
Integral thread milling cutters (Fig. 5-90) are mostly made of integral cemented carbide materials, and some are coated.
The integral thread milling cutter has a compact structure, which is more suitable for machining medium and small diameter threads.
There are also integral thread milling cutters for machining taper threads.
This kind of cutter has good rigidity, especially the integral thread milling cutter with spiral groove, which can effectively reduce the cutting load and improve the machining efficiency when machining high hardness materials.
The cutting edge of the integral thread milling cutter is full of thread processing teeth, and the whole thread processing can be completed by processing along the spiral line for one week. There is no need for layered processing like the clamp type cutter, so the processing efficiency is high, but the price is relatively expensive.
This kind of tap is often used for machining small and medium diameter threads.
Fig. 5-90 common integral thread milling cutter
4. Integral thread milling cutter with chamfer function
The structure of the integral thread milling cutter with chamfer function (Fig. 5-91) is similar to that of the ordinary integral thread milling cutter, but there is a special chamfer edge at the root (or end) of the cutting edge, which can process the thread end chamfer while processing the thread.
There are three ways to process chamfers. When the tool diameter is large enough, the chamfering edge can be directly used to spot face the chamfer.
The method is limited to chamfering the hole of internal thread.
When the tool diameter is small, the chamfer edge can be used to process the chamfer through circular motion.
However, when using the chamfer edge at the root of the cutting edge for chamfering, it should be noted that there should be a certain gap between the thread cutting part of the tool and the thread to avoid interference.
If the processed thread depth is less than the effective cutting length of the tool, the tool will not be able to realize the chamfer function.
Therefore, when selecting the tool, ensure that its effective cutting length matches the thread depth.
Fig. 5-91 integral thread milling cutter with chamfer function
5. Thread drill and milling cutter
The thread drill and milling cutter (see Fig. 5-92) is made of integral cemented carbide and is an efficient tool for machining medium and small diameter internal threads.
The thread drill and milling cutter can drill the thread bottom hole, chamfer the orifice and process the internal thread at one time, reducing the number of tools used.
But the disadvantage of this kind of cutting tool is its poor versatility and high price.
The tool consists of a drilling part of the head, a thread milling part in the middle and a chamfer edge at the root of the cutting edge.
The diameter of the drilling part is the bottom diameter of the thread that the tool can process.
See Fig. 5-93 for thread processing process.
Limited by the diameter of drilling part, a thread drill and milling cutter can only process one specification of internal thread.
When selecting the thread drill and milling cutter, not only the specification of the machined thread hole, but also the matching between the effective machining length of the cutter and the depth of the machined hole should be paid attention to, otherwise the chamfering function cannot be realized.
Fig. 5-92 thread drill and milling cutter
Fig. 5-93 machining process of thread drill and milling cutter
6. Deep thread milling tool
The deep thread mil
e cutting depth of a general thread milling cutter is about twice its cutter body diameter, and the use of a single tooth deep thread milling cutter can better overcome the above shortcomings.
Because the cutting force is reduced, the thread processing depth can be greatly improved (see L1 in fig. 5-94).
Fig. 5-94 deep thread milling tool
7. Thread milling tool
The universality and efficiency of the system is a prominent contradiction of thread milling cutter. Some tools with composite functions (such as thread drill milling cutter) have high machining efficiency but poor universality, while the efficiency of tools with good universality is often not high.
To solve this problem, a modular thread milling tool system (see Fig. 5-95) is developed.
The tool is uniformly composed of a tool handle, a countersink chamfer edge and a general thread milling cutter.
Different types of countersink chamfer edges and thread milling cutters can be selected according to the processing requirements.
The tool system has good versatility and high machining efficiency, but the tool cost is high.
The above briefly introduces the functions and characteristics of several common thread milling tools.
Fig. 5-95 thread milling tool system
（3） Problems and Countermeasures of thread milling
Like other milling cutters, thread milling cutters will encounter blade wear, edge collapse, chip buildup and other phenomena during milling.
Table 5-25 shows several common problems and corresponding solutions in thread milling.
Table 5-25 problems and Countermeasures in thread milling
| Problem | Possible causes | Resolvent |
| Excessive blade flank wear | Cutting speed too high | Reduce cutting speed |
| Chip too thin | Increase feed rate | |
| Insufficient cutting fluid | Increase cutting fluid flow / pressure | |
Cutting edge collapse | Chip too thick | Decrease the feed rate use the tangential arc method to increase the spindle speed |
| Vibration | Check rigidity | |
Chip buildup on cutting edge | Cutting speed too low | Increase cutting speed |
| Chip thickness too small | Increase feed rate | |
Chatter / vibration | Feed rate too high | Decrease feed rate |
| Too deep profile (coarse thread) | Perform two cuts, each time increasing a certain back cutting amount, perform two cuts, each time cutting only half of the thread length | |
| Thread length too long | Perform two cuts, cutting only half the thread length each time | |
| Insufficient thread accuracy | Tool deviation | Reduce the feed rate and perform a “zero” cut |