The straight thread cutter X advances intermittently to the depth of the teeth (Figure 2a). When the trapezoidal thread is machined in this way, all three sides of the thread turning tool participate in the cutting process, which results in difficulty in machining removal of chips, an increase in cutting force and cutting heat, and severe wear of the tool tip. When the feed amount is too large, “knife” and “knife” may also occur. This method of CNC lathes can be implemented with the G92 command, but it is clear that this method is not desirable.
The oblique turning thread cutter feeds obliquely into the depth of the teeth along the direction of the angle of the teeth (Fig. 2b). When the trapezoidal thread is machined in this way, the thread turning tool always has only one side edge to participate in the cutting, so that the chip removal is relatively smooth, the force and the heat condition of the cutting edge are improved, and it is not easy to cause the "knife" phenomenon during turning. This method can be implemented on CNC lathes using the G76 command. The staggered cutting thread tool feeds tooth depths along staggered gaps in the direction of the angle of the teeth (Figure 2c). This method is similar to the oblique method, and can also be implemented on a CNC lathe using the G76 command.
Grooving Knife Rough Grooving Method This method uses a grooving knife to roughly cut out the thread groove ((Fig. 2d), and uses a trapezoidal thread turning tool to machine both sides of the thread. The programming and machining of this method is difficult on CNC lathes. achieve.
3. Trapezoidal thread measurement
Trapezoidal thread measurement integrated measurement, three-needle measurement, and single-needle measurement three. The integrated measurement is measured with a thread gauge. The three-needle measurement and single-needle measurement of the middle diameter are shown in Fig. 3 and are calculated as follows:
M=d2+4.864dD-1.866P (dD indicates the diameter of the measuring probe, P indicates the pitch.)
A=(M+d0)/2 (where d0 represents the actual outside diameter of the workpiece)
Second, trapezoidal thread programming examples
Example: As shown in Figure 4 trapezoidal thread, trial G76 instruction preparation processing program.
1. Calculate the size of the trapezoidal thread and check the table to determine its tolerance large diameter d = 360–0.375;
Medium diameter d2=d-0.5P=36-3=33, check table to determine its tolerance, so d2=33–0.118 –0.453
The tooth height h3 = 0.5P + ac = 3.5;
The path d3=d-2 h3=29, check the table to determine its tolerance, so d3=290–0.537;
Crest width f=0.366P=2.196
Bottom width W=0.366P-0.536ac=2.196-0.268=1.928
Measure the median diameter with a measuring rod of 3.1 mm, then its measurement size M=d2+4.864dD-1.866P=32.88, determine its tolerance according to the diameter tolerance, then M=32.88–0.118–0.453
2. Write NC program
O0308;
G98 ;
T0202;
M03 S400;
G00 X37.0 Z3.0;
G76 P020530 Q50 R0.08;(Set the finishing twice, the finishing allowance is 0.16mm, the chamfer amount is equal to 0.5 times the pitch, the angle of the tooth is 30°, the minimum depth of cut is 0.05mm.)
G76 X28.75 Z-40.0 P3500 Q600 F6.0;(Set the thread height to 3.5mm and the first knife to cut the depth to 0.6mm.)
G00150.0
M05;
M30
The above procedure adopts the oblique feed approach along the angle of the dental profile in the thread cutting process, as shown in Fig. 2b. In the FANUC-0i system, it is sometimes also possible to use a staggered thread cutting method as shown in Figure 2c. The G76 programming is as follows:
G76 X28.75 Z-40.0 K3500 D600 F6.0 A30.0 P2;
K: thread profile height.
D: The amount of back eating at the first feed.
A: Tooth angle.
P2: Interleaved Thread Cutting
3. Calculate the Z-axis tool offset value
In the actual machining of the trapezoidal thread, since the width of the blade tip is not equal to the width of the groove bottom, the diameter of the thread can not be properly controlled through a single G76 cycle cutting. To solve this problem, the tool can be used after Z-biased and then G76 cycle machining. In order to improve the machining efficiency, it is better to perform only one offset process. Therefore, it is necessary to accurately calculate the offset in the Z direction and the Z-direction offset. The calculation method shown in Figure 5 is calculated as follows:
Let M measure - M theory = 2AO1 = δ, then AO1 = δ/2
As shown in FIG. 5 , the quadrilateral O1O2CE is a parallelogram, then ΔAO1O2≌ΔBCE, AO2=EB. ΔCEF is an isosceles triangle, then EF=2EB=2AO2.
AO2=AO1×tan(∠AO1O2)=tan15°×δ/2
Z direction offset EF=2AO2=δ×tan15°=0.268δ
During actual processing, after one cycle is completed, the measured M value is measured with three pins to calculate the Z offset of the tool, then the Z offset is set in the tool length compensation or wear memory, and G76 is used again for cycle processing. One-time accurate control of the thread diameter and other parameters.
Third, the conclusion
Through the above example analysis we can conclude that in order to easily machine the trapezoidal thread on CNC machine tools, the key is to do the following:
1. Reasonably select the machining instructions of the trapezoidal thread, usually select the G76 command.
2. Accurately set the parameters of the G76 command. These values are usually calculated by analyzing the trapezoidal thread.
3. Based on the initial measured median diameter, the Z-axis tool offset value is accurately calculated to accurately control the trapezoidal thread diameter.
3, The division of processing procedures and analysis of processing range of CNC milling machine
The design of the process route of the CNC milling machine must fully consider various factors, pay attention to the correct division and sequence of the process, and properly arrange the connection between the CNC milling process and the ordinary process. Compared with ordinary milling machine processing, CNC machining is more concentrated.
According to the machining characteristics of CNC milling, there are three forms of the division of the machining process of CNC milling.
1, according to the clamping positioning division process. This method is generally applicable to the processing of small parts of the workpiece, the main part is to divide the processing site into several parts, each process processing part of it. If the shape of the CNC milling, when the internal cavity clamping processing cavity, clamping shape.
2, the rough, fine processing division process. For CNC milling parts that are easily deformed by machining, taking into account the machining accuracy and deformation of the workpiece, the process can be divided according to the principle of rough and fine processing separation, that is, after the first rough finish.