Low-speed turning triangular thread The turning tool of low-speed turning triangular thread is generally high-speed steel. If separate roughing and finishing cars are processed separately, better surface roughness and accuracy can be obtained. Rough turning tool teeth angle often take 5 8.5 ~ 5 9 °, than the fine turning tool teeth angle is smaller 1 ~ 1.5 °, with a roughing knife to the tooth depth (ie external thread diameter), and then use the fine car The light thread on the side of the knife car can protect the cutting edge and save time. When grinding rough thread cutters, do not deliberately sharpen the sharp corners of the knife, as long as the rake angle is properly increased in the rake angle of the driving knife, so that both the purpose of smooth chip removal and the reduction of the profile angle can be achieved. However, when the rake angle is increased and the wedge angle is reduced, the strength of the turning tool is reduced, so the back angle should be reduced appropriately, so that the lack of strength of the turning tool can be compensated. There are two kinds of feeding methods for triangular threads: Straight and oblique. 1 1 straight-in straight-in method Turning the triangular thread, the two edges of the turning tool are cut at the same time, the turning tool is subjected to great force, the heat dissipation is difficult, the wear is fast, and the chip removal is difficult. The cutting depth of each feed cannot be too large. However, the processed thread profile is more accurate. Because the cutting edge of the turning tool participates in the cutting, it is easy to produce the phenomenon of "knife" and picks up the tooth surface, even causing the cutting edge to break due to large cutting force, which may damage the turning tool and cause vibration. Therefore, it is only suitable for the finishing of threads with thread pitch P < 2mm and high precision threads. Nowadays, CNC lathes all have thread cutting functions. Most CNC beds have single-threaded thread cutting functions, and high-end CNC lathes have thread-based composite fixed-cycle cutting functions. When cutting the thread, the thread feed must be performed several times according to the size of the thread pitch, the depth of the thread profile, the material of the turning tool, the material of the workpiece, and the feed rate of the lathe, etc., and the cutting method is used for cutting. The amount of knife for each feed is distributed according to the law of diminishing. For example, to turn an M5 0×4 ordinary cylindrical thread, the calculated programming thread diameter is 4 9.72mm, the programmed thread diameter is 4 6 .5 2mm, the infeed section is taken 3mm, the withdrawal section is taken 2mm, and the single lead is G32. The thread writing instruction program is as follows: O1111;...N10G0 0X4 9.72; N11G32Z - 32.0F4; N12G0 0X5 0 .N13Z3.0; N14X4 8.72; Z - 32.0N15G32Z - 32.0F4; N16G0 0X5 0 .0; N17Z3 .0 ;N18X4 8.12 ;N19G32Z - 32 .0F4 ;...N33G0 0X4 6 .5 2 ;N34G32Z - 32 .0F4 ;...N5 0M30 ;Because the G32 is only a thread machining instruction, the turning of the turning tool, cutting out and returning are all required. Into the program, the program looks longer, such as the use of thread cycle processing instructions G92, G76, etc. to write programs, the program is shorter. For example, for a general cylindrical external thread M30 × 2 - 6g, the external diameter of M30 × 2 - 6g found in GB197-81 is 30 -0 .0 3 8-0 .3 18mm, and the programmed external diameter is 2 9.7mm. Let the bottom of the tooth be composed of a single circular arc R, take R = 0.2mm, calculate the bottom diameter of the thread as 27.244.6mm, and take the programmed bottom diameter as 27.3mm. Prepare to arrange 6 cutters to finish, adopt the straight knife method, set the first to sixth cutter thread cutting depth (diameter value) is 0. 8mm, 0. 5mm, 0. 4mm, 0. 4mm, 0 .2mm, 0.1mm. The origin is programmed in the Z direction on the right side of the workpiece. The program is programmed with the thread single cycle cutting command G92, and the program is as follows: O2 2 2 2 ;...N10G0 0X33.0Z3.0 ; N11G92X2 8.9Z - 40 .0F2 .0 ; N12X2 8 .4 ; N13X2 8.0 ; N14X2 7.6 ; N15X2 7.4 ;N16X2 7.3;...N4 0M30 ;The program of turning M2 4×3 ordinary triangular external thread with FANUC6T system G76 thread compound cycle cutting instruction is as follows (The Z axis programming origin with the thread far away from the chuck is adopted. Into the feed, set the thread finishing allowance to zero). O3333;...N10G0 0X30 .0Z8.0 ;N11G76X2 0 .75 2Z - 40 .0I0K1.6 2 4D0 .6 14F3.0A0 ;...N15M0 2 ; Here, X2 0 .75 2 is the thread bottom diameter, Z - 40 .0 Is the end of the thread coordinates, I0 means that the thread radius is zero, which is a cylindrical thread, K1.6 2 4 is the tooth height, A0 means straight forward method feed, the half angle is 30 °, D0 .6 14 is The first knife knife depth, F3.0 shows that the pitch is 3mm. 1 2 Oblique oblique method When the triangular thread is turned, the turning tool advances obliquely along one side of the thread profile, and only one side of the edge of the turning tool is used for cutting. After several passes, machining is completed. When using this method to machine triangular threads, the cutting conditions of the tool are good, the cutting depth can be increased, and the production efficiency is high. However, the machined surface has a large roughness and is only suitable for rough machining. When finishing the thread, in order to make the surface smooth on both sides of the thread, the last one or two feeds should adopt the straight feed method to ensure the thread profile is accurate. The oblique method can be used either for the left or right edge cutting, and for the left single edge blade for the example, to rewrite the program based on the above procedure. M30 has a profile angle α = 6 0° and its half angle is 30°. You can let each knife go down at the same time as the distance h from the knife, and also take a length L to the left, so that this length is equal to the distance to the knife and multiplied by the tangent of the half angle, that is L = htan α2. The processing procedure is as follows: O4 444 ;...N10G0 0X33.0Z3.0 ;N11G92X2 8.9Z - 40 .0F2 .0 ;N12G0 0Z2 .85 6 ;N13G92X2 8.4Z - 40 .0F2 .0 ;N14G0 0Z2 .74 1;N15G92X2 8.0Z - 40 .0F2 .0 ;N16G0 0Z2 .6 2 6 ;N17G92X2 7.6Z - 40 .0F2 .0 ;N18G0 0Z2 .5 6 8 ;N19G92X2 7.4Z - 40 .0F2 .0 ;N2 0X2 7.3 ;...N5 0M30 ; Compared with O2222, the program has only four segments: N12, N14, N16, and N18. This is a four-stage program that changes the double-edged cutting edge of the thread to a single edge blade. However, the first knife and the last knife are straight-forward and double-sided cutting, which ensures the accuracy of the angle. Thread processing compound thread G76 command processing thread, some of the feed methods are skew method, the distribution of cutting depth of each tool is automatically assigned by the numerical control system according to the law of decrement, the purpose is to make each cutting area is nearly equal. Shown in Figure 1 is the method of feeding the thread compound cycle processing. Fig. 1 Thread-composite cycle machining feed Fig.1 Feedwayofcompoundloopcuttingthread For example, the external thread of a cylindrical triangle of M30×3: Thread diameter Dd=Dg- 0 .1×Pitch = 30 - 0 .1× 3=2 9.7 Thread Dx =Dg-1.3×Pitch=30 - 1.3×3=2 6.1 The tooth depth is 2 9.7- 2 6 .1=1.8mm. The program written by GSK CNC GSK980T lathe CNC system is as follows: O5 5 5 5 ;...N2 0G0X4 0Z4 7;N30G76P0 2 0 5 6 0Q5 0R0 .0 8;N4 0G76X2 6 .1Z0R0P180 0Q5 0 0F3;...N80M30 ; Here, P0 2 0 5 6 0 means that the number of finishing operations is two, and the thread chamfer width is 5× 1 10×pitch=1.5mm, profile angle is 60°; Q50 indicates the minimum cutting amount is 0. 0 5mm; R0. 0 8 indicates the finishing allowance is 0.08mm; X26.1 is the thread bottom Diameter, Z0 is the coordinates of the end point of the thread, R0 is a straight thread with a thread radius difference of zero, P180 0 means the tooth height is 1.8mm, Q50 0 means the first cutting amount is 0.5mm, and F3 means the thread pitch. Use the FANUC6T system G76 thread compound cycle cutting instruction to program the turning M2 4×3 ordinary triangular external thread as follows (the Z-direction programming origin of the thread far from the chuck): O6 6 6 6 ;...N10G0 0X30 .0Z8. 0 ;N11G76X2 0 .75 2Z - 40 .0I0K1.6 2 4D0 .6 14F3.0A30 ;...N15M0 2 ; Here, X2 0 .75 2 is the thread bottom diameter, Z - 40 .0 is the thread end coordinate, I0 is the thread The radius difference is zero, which is a cylindrical thread, K1.6 2 4 is the tooth height, A30 is the single-edged blade eating method, the dental half angle is 30°, D0 .6 14 is the depth of the first knife, F3. 0 means that the pitch is 3mm. Another example is the use of FANUC0 system G76 threaded composite cutting instructions for the preparation of turning M2 4 × 3 ordinary triangular external thread program is as follows: O7777; ... N10G0 0X30 .0Z8.0; N11G76P0 110 6 0Q10 0R10 0; N12G76X2 0 .75 2Z-40. 0R0P16 2 4Q6 14F3.0 ;...N15M0 2 ; Here, P0 110 6 0 means that the number of finishing operations is 1, and the oblique retraction amount is 10, which is a pitch, and the angle of the tooth profile is 6 0°. Q10 0 means the minimum depth of cut is 0 .1mm , R10 0 means that the finishing allowance is 0.1mm, X2 0.75 2 means the thread path, Z - 40 .0 means the coordinates of the thread end, and R0 means that the thread radius difference is zero and it is a cylindrical thread, P16 2 4 The tooth height is 1.62 4mm, Q6 14 is the depth of the first knife, 0 6 14mm, F3.0 is the pitch of 3mm, and the feed method is the oblique edge method. 2 The cutting speed of high-speed cutting triangular thread on high-speed turning threads on CNC lathes can be taken as v = 4 0 ~ 10 0m min. When the cutting can only be fed straight forward, so that the chip discharge into the ball or the two cutting edge chip discharge evenly discharged from the front, can not be out of the band crumbs, straight out of the chip is not safe, we must strictly control the chip shape. It is not possible to use the oblique feed method, which will destroy the surface quality of the workpiece and damage the tool. To use hard alloy thread turning tools, the tool must have good hardness and impact toughness. The choice of YT15 carbide turning tool is more appropriate. When turning a large pitch (P > 2mm), or when the workpiece material is hard, the cutting edges on both sides of the turning tool should be ground with a width of 0.2 - 0.4 mm and a negative chamfer of -5°. Due to the high-speed cutting, the workpiece material is squeezed more severely, and the angle of the tooth profile is enlarged. Therefore, the angle of the tool tip should be smaller than the angle of the tooth profile by 0.5°;