Detailed explanation of thread milling

With the progress of the times, CNC industry is more and more widely used in large and medium-sized mechanical processing industries in my country. For thread processing of some large parts, traditional thread turning and taps and dies can no longer meet the needs of production. Today, when CNC milling machines or machining centers are widely used, the use of three-axis linkage machine tools for thread processing has changed the thread processing method and achieved good results.

1. Spiral milling inner hole

1. Processing range

For blind holes or through holes with larger diameters, spiral milling is often used because twist drills are too slow or cannot be used. And because the tool selected for this method does not have a bottom edge, it is more suitable for processing with small cutting depth, high speed and high feed.

2. Processing characteristics

Spiral milling is a processing method based on the spiral cutting method. There is a characteristic in spiral milling: for every spiral milling circle, the tool moves a cutting height in the Z-axis direction.

3. Selection of thread milling cutter

Select a 16mm three-edge indexable milling cutter, tool speed S=3000r/min, feed rate F=2500mm/min.

4. Description

This method is very unique in spiral milling inner holes. The essence of its programming is to compile a subroutine with a cutter height as the spiral line height, and complete the milling of the entire hole by cyclically calling the spiral line subroutine. The hole processing of this method is not affected by factors such as milling cutter specifications, so it is ideal for use on CNC milling machines and machining centers.

5. Application examples and program writing

In the part drawing shown in Figure 1, a bottom through hole with thread M36×1.5mm is to be machined.

First, the bottom hole diameter of the thread M36×1.5mm is calculated as: nominal diameter-1.0825×P(pitch)=36-1.0825×1.5=33.75mm. Confirm that the machining blank of the part is 80mm×80mm×30mm 45 steel, and the selected tool is a 16mm three-edge indexable milling cutter, the tool speed S=3000r/min, and the feed rate F=2500mm/min. The arc lead-in point is A (Figure 2), and the tool compensation is established in the 0A segment. The arc lead-out point is B, and the tool compensation is cancelled in the 0B segment.

The reference program is written as follows (the reference programs involved in this article have been verified and used in the FANUC system).

The main program is as follows.

%(Program start character)

O0001;(main program name)

T1; (The tool is a 16mm end mill)

G80G40G69; (cancel fixed cycle, tool radius compensation and rotation command)

G90G54G00X0Y0M03S3000;(Program initialization)

G43Z50.0 H01; (No. 1 tool length compensation)

Z5.0; (fast moving point positioning)

G01Z0F50;(Working progress)

G41D01G01X-6.875Y10.0; (D01=8.0, tool compensation is established in 0A segment)

G03X-16.875Y0R10; (arc import R10)

M98P100L16; (call subroutine O100, call times 16 times)

G90G03X-6.875Y-10R10.0;(smoothing contour for one week)

G40G01X0Y0;(Cancel tool compensation)

G0Z50.0;(Exit)

M05; (spindle stop)

M30; (The program ends and returns to the program header)

% (Program end character)

The subroutine is as follows.

%(Program start character)

O100;(subroutine)

G91G03I16.875Z-2.0F2500; (Use incremental coordinate values ​​to program, the tool moves 2mm downward in the Z-axis direction for each revolution)

M99; (return to main program)

% (Program end character)

The inner hole is processed by the spiral cutting method, and cylindrical workpieces can also be processed according to this programming idea.

2. Single-edge thread milling cutter thread processing

1. Processing range

The same thread milling cutter can mill both left-hand and right-hand threads, both internal and external threads, and is not affected by pitch and thread specifications.

2. Processing characteristics

Single-edge thread milling cutter is a processing method based on the spiral cutting method. The principle of thread milling is: for each milling circle of the thread milling cutter, the tool moves one lead in the Z-axis direction (one pitch for single line).

3. Selection of thread milling cutter

Select a 16mm single-edge thread milling cutter, tool speed S=1800r/min, feed rate F=300mm/min.

4. Description

This method is very unique in thread milling. The essence of its programming is to compile a helical line of a lead into a subroutine. By repeatedly calling the helical line subroutine for processing, the milling of the entire thread can be completed. The thread processing using this method is not affected by parameters such as milling cutter pitch and thread specifications, so it is widely used in CNC milling machines and machining centers.

5. Application examples and program writing

Continue to process the M36×1.5mm thread of the workpiece shown in Figure 1, as shown in Figure 3, the arc lead-in point is A, tool compensation is established in segment 0A, the arc lead-out point is B, and tool compensation is canceled in segment 0B. The thread processing program written according to the idea is as follows.

The main program is as follows.

%(Program start character)

O0002;(main program name)

T2; (Tool No. 2 is a 16mm thread milling cutter)

G80G40G69; (cancel fixed cycle, tool radius compensation and rotation command)

G90G54G00X0Y0M03S1800;(Program initialization)

G43Z50.0H02;(No. 2 tool length compensation)

Z5.0; (fast moving point positioning)

G01Z0F50;(Working to Z0)

G42D02G01X-8Y-10.0; (D02=Rprg, the programming value of the corner radius of the thread milling cutter, and the tool compensation is established in the 0A segment)

G02X-18.0Y0R10; (arc import R10)

M98P200L14; (call subroutine O200, call times 14 times)

G90G02X-8.0Y10R10.0; (arc export R10)

G40G01X0Y0;(Cancel tool compensation)

G0Z50.0;(Exit)

M05; (spindle stop)

M30; (The program ends and returns to the program header)

% (Program end character)

The subroutine is as follows.

%(Program start character)

O200;(subroutine)

G91G02I18.0Z-1.50F300; (Use incremental coordinate values ​​to program. The tool moves downward along the Z axis by a pitch of P=1.5mm every time it runs one circle)

M99; (return to main program)

% (Program end character)

This example describes how to use a single-edge thread milling cutter to machine internal threads. Similarly, a similar method can be used to program external threads.

3. Multi-edge thread milling cutter thread processing

1. Processing range

The same thread milling cutter can mill both left-hand and right-hand threads, as well as internal and external threads. It is mainly used in situations where production efficiency is high.

2. Processing characteristics

Each milling cutter has a value, which is the programming value of the tool fillet radius, that is, the tool radius compensation value when milling threads. When thread milling, the general processing depth can be completed in one time, but if it is required to be milled in multiple times, it can be completed by modifying the tool compensation value.

3. Selection of thread milling cutter

The effective length of the thread milling cutter is generally greater than 20mm, the pitch of the multi-edge thread milling cutter is 1.5mm, the tool speed S=1200r/min, and the feed rate F=100mm/min.

4. Description

This method is very efficient in thread milling and the program writing is also very simple. The essence of its programming is: the thread milling cutter imports (or exports) 1/4 circle in the XOY plane, and the thread is officially processed for 1 circle; when it is imported (or exported) 1/4 circle in the Z-axis direction, the tool runs 1/4 pitch, and when the thread is officially processed for 1 circle, the tool runs 1 pitch in the Z-axis direction. By ensuring that each effective tooth on the multi-blade thread milling cutter participates in milling at the same time, the milling of the entire thread is completed. The focus of thread processing in this method is reflected in the selection of the pitch of the milling cutter: when it is required to process a thread of a certain pitch, a corresponding thread milling cutter must be selected. At the same time, this method is affected by factors such as the pitch of the milling cutter and the thread specification, but due to its high processing efficiency, it is widely used in CNC milling machines and machining centers.

5. Application example program writing

As shown in Figure 1, when the workpiece has a right-hand thread of M36×1.5mm, the effective depth of the thread is 20mm. In specific processing, milling is performed from bottom to top, the tool is introduced 180°, and at the same time moves 0.5 pitch in the Z-axis direction. After milling the thread for one circle, the tool moves 1 pitch in the Z-axis direction, and then leads out 180°, and the tool moves another 0.5 pitch. When milling left-hand threads, the tool should be milled from top to bottom. As shown in Figure 3, the introduction point is point B, the OB segment is to establish tool compensation, the export point is point A, and the OA segment cancels tool compensation.

%(Program start character)

O0003;(main program name)

T3; (Tool No. 3 is a multi-edge thread milling cutter with a taper of 16mm)

G80G40G69; (cancel fixed cycle, tool radius compensation and rotation command)

G90G54G00X0Y0M03S1200;(Program initialization)

G43Z50.0H03;(No. 3 tool length compensation)

Z5.0; (fast moving point positioning)

G01Z-30.375F100; (Working to the lowest point of the thread Z-30.375)

G41D01G01X-8.0Y10.0; (D01=Rprg, this value is the programming value of the tool corner radius)

G03X-18.0Y0Z-30.0R10.0; (Due to the introduction of 1/4 arc, the movement in the Z direction moves 1/4 pitch, -30.375 rises to -30)

G03X-18.0Y10Z-28.5R18.0; (the effective milling thread length Z moves upward by one pitch)

G03X-8.0Y-10.0Z-28.125R10; (introducing a 1/4 arc, moving in the Z direction by 1/4 pitch from -28.5 to -28.125)

G40G01X0Y0;(Cancel tool compensation)

G00Z50.0;(Exit)

M05; (spindle stop)

M30; (The program ends and returns to the program header)

% (Program end character)

Similarly, the program for the external thread example can be written in a similar way.

IV. Conclusion

This article briefly discusses the methods of thread milling with thread milling cutters and explains the different programming methods for thread milling with thread milling cutters. It has certain guiding significance for those engaged in CNC teaching and scientific research, especially CNC milling workers and machining center operators on the production line.