Thread CNC Machining and Programming

The traditional thread processing methods are mainly: the external thread is turned with a thread turning tool, and the thread profile can be cut out by multiple passes while working, and the production efficiency is low; the internal thread adopts tap tapping, and the thread bottom must be put into operation. The hole is machined and then the tool is changed for processing. 

The auxiliary time is long. With the development of numerical control technology, the machining methods of CNC milling threads gradually replace the traditional thread processing methods. Compared with the traditional thread processing method, the efficiency of thread milling and machining accuracy have been improved. 

Especially for some threads with special structural requirements, such as threads without transition buckles or undercuts, the use of thread milling shows its advantages. Therefore, for mass-produced threads, NC milling threads is a new process that has a great promotion value. 1 Thread milling cutters and their technological characteristics There are many types of milling cutters for threading, and various thread milling cutters have different processing characteristics. The disk-shaped thread milling cutter disk-shaped thread milling cutter is shown in Fig. 

1(a). When working, the milling cutter axis and the workpiece axis are inclined. The workpiece thread medium-diameter lead angle enters, the workpiece rotates once, and the workpiece and the milling cutter are opposite to each other. Move one pitch. It is usually possible to cut out the required threads in a single pass. The schematic diagram of the work is shown in Fig. 

1(b). In order to improve the smoothness of milling, the number of teeth should be multi-toothed and made into the wrong tooth form in order to improve the cutting conditions on both sides of the blade. The disc-shaped thread milling cutter is mainly used for milling larger pitch and longer length threads, such as single or double trapezoidal thread and worm.

Comb thread milling cutter comb thread milling cutter can be seen as a combination of several disk-shaped thread milling cutters, as shown in Figure 

2. During machining, the milling cutter is parallel to the workpiece axis, and the milling cutter and the workpiece are in full contact along the thread. Therefore, when the workpiece is rotated once during cutting, the workpiece and the milling cutter move axially by one pitch, and the desired thread can be cut out. Comb thread milling cutters are mainly used for machining triangular inner and outer cylindrical threads and conical threads with short length and small pitch. In order to increase the production efficiency, the compound thread milling cutter can cut out the thread at one time without changing the tool. The thread milling cutter can be used as shown in Figure 

3(a). The surface of the cutting edge of the thread drilling cutter is somewhat like a tap. Actually, unlike a tap, there is no spiral lift on the tool, and the spiral in the machining is realized by the movement of the machine tool. A schematic diagram of the operation when milling a thread with a thread cutter is shown in Fig. 

3(b). The steps are: Step 1, the thread drilling cutter is quickly moved to the workpiece safety plane; Step 2, the thread drilling cutter drills to Hole depth size; Step 3, the thread drilling cutter is lifted to the thread depth dimension; Step 4, the thread drilling cutter starts with the arc cutting thread; Step 5, the thread drilling cutter makes X, Y around the thread axis. The direction of the interpolation movement, while making parallel to the axis +Z direction of movement, that is, each axis running 360 °, along the +Z direction will increase a pitch, tool three-axis linkage trajectory for a spiral; Step 6, The thread drilling cutter retracts the tool from the starting point with a circular arc. At the 7th step, the thread drilling cutter quickly retreats to the workpiece safety plane and prepares to process the next hole. The trajectory of the milling thread of the thread drilling cutter is shown in Figure 

4. 2 Thread Milling Programming Now the M20 × 1.5 right-handed internal thread milling example illustrates the threading programming method. Workpiece material: Cast iron; Thread bottom hole diameter: Di18.38mm; Thread diameter: Do=20mm; Thread length: L=25mm; Pitch: P=1.5mm; Tool: Carbide thread milling cutter; Milling cutter diameter D2= 10mm; Milling method: Climbing; Cutting speed 50m/min; Milling feed: 0.1mm/teeth. The parameter calculation spindle speed is: n=(1000v)/(D2p)=(1000×50)/(10x3.14)=1592(r/min) The number of cutter teeth z=1, the feed per tooth f=0.1mm The feed speed at the cutting edge of the milling cutter is: v1=fzn=0.1×1×1592=159.2(mm/min) The feed speed of the milling cutter center is: v2=v1(D0-D2)/D0=159.2×(20) -10)/20=79.6 (mm/min) Set the safety distance CL=0.5mm, and cut in the arc radius: Re=(Ri-CL)2+R02=(9.19-0.5)2+102=8.78 2R0 2× 10 cut into the arc angle: b = 180 ° - arcsin [(Ri-CL) / Re) = 180 °-arcsin [(9.19-0.5) / 8.78] = 180 °-84.12 ° = 95.88 ° cut into the arc The Z-axis displacement is: Za=Pa/360°=1.5×90°/360°=0.375(mm) The coordinates of the start point of the cutting arc are: {X=0 Y=-Ri+CL=-9.19+0.5=-8.68 Z =-(L-Za)=-(25+0.375)=-25.375 Thread milling program (FUNUC system) % N10 G90 G00 G57 X0. Y0. N20 G43 H10 Z0. M3 S1592 N30 G91 G00 X0. Y0. Z-25.375 N40 G41 D60 X0. Y-8.68 Z0. N50 G03 X10. Y8.68 Z0.375 R8.78 F79.6 N60 G03 X0. Y0. Z1.5 I-10. J0. N70 G03 X-10. Y8.68 Z0.375 R8.78 N80 G00 G40 X0. Y-8.68 Z0. N90 G49 G57 G00 Z200. M5 N100 M30