Deep hole boring has always been a difficult problem in mechanical and mold processing. A classmate encountered a 48×215mm deep hole processing on a rubber hose mold before. I hope to write down the pit he waded through and provide it to you. Some help and reference.
1. Parts diagram analysis and process planning
Part Drawing Analysis
Figure 1 shows the rubber hose mold part, there are 4 holes with a diameter of 48×215mm deep to be machined. The overall size is 420×270×250mm, there are 4 grooves on the top, bottom, left, and right sides, there are steps on the hole surface, and slopes on both sides are row matching surfaces.
Figure 1 Hose mold parts
The size of the part is shown in the figure. The process requirements of this part are that the conicity of the hole should not exceed 0.1mm, the surface roughness value should be Ra3.2μm, the tolerance of the hole distance should not exceed 0.03mm, and the verticality should be 0.03mm. The product of this mold It is a glass rubber hose, its wall thickness is only 0.8mm, and the customer requires that the thickness exceeds 0.8mm will not be accepted. It can be said that the thinner the better, it is to save costs.
At that time, I really had no idea about such a difficult part. Although our unit was only responsible for processing deep cavity borings, customers could cooperate with other processing. After many attempts, a simple and reasonable processing scheme was developed.
Process Planning
Simple Machining Sequence Before Part Boring
After the fine material comes back, the milling machine first processes the grooves on both sides. As shown in Figure 1, the positions B and E are first rough and then refined, and the number is processed.
The steps on the front of the machine are roughened, leaving a margin of 0.5mm on one side, as shown in Figure 1 at A and F.
The step of the processed bottom surface is roughened, and a margin of 0.5mm is left on one side, as shown in C and D in Figure 1.
Then re-clamp and adjust the meter, divide the four sides, and center the center for drilling and positioning. It is processed step by step by drills with a diameter of 10mm, 24mm and 35mm, and finally drilled through with a drill with a diameter of 44mm.
After the completion, go to the large water mill to process the surface and bottom, as shown in Figure 2, and grind to the number to ensure that the parallelism is 0.03mm.
As shown in Figure 1, a 0.3mm finishing allowance is reserved for side grinding of B and E.
Clamping and positioning datum of parts
The workpiece is directly clamped on the CNC workbench, and the 4 mold feet are respectively tightened, and the calibration is divided into centers, and the error is controlled within 0.03mm.
2. CNC machining of parts
Part Drawing Analysis
Self-made boring tool: first make a boring tool holder as shown in Figure 3, the material is 837H, rough turning first, reserve 0.5mm margin, and process it with an external cylindrical grinder after heat treatment, the focus is to ensure the coaxiality. The small knife holder with the insert blade is purchased as a standard piece of 10×10mm, which is convenient for replacing the blade and guarantees the size.
The inclination angle of the built-in small knife holder is 20°, wire cutting processing, slightly tight fit. The boring tool holder is equipped with M6mm inner hexagon screws, and the small tool holder is locked with the inner hexagon screws. Carbide inserts are installed in the standard small tool holder, the main deflection angle is 30°, the clearance angle of the flank face is 15°, and the sharp corner of the insert has an angle of R0.3~R0.4mm to minimize the contact surface to prevent vibration.
picture
picture
Figure 2 Dimensions of parts
The processing plan is determined
Hole processing scheme 1
Fast-feeding wire cutting is the most direct and simple method without roughing, but because the size is too deep to 215mm, it is difficult to solve the problem of cooling and flushing during processing, and it is easy to break the wire, and the surface roughness value cannot meet the requirements.
Hole processing scheme 2
With slow wire cutting, the wire is easy to break due to the depth of the hole, but the processing fee for each hole is about 1,945 yuan, and the total cost of wire cutting for the mold is nearly 7,700 yuan, which is far beyond the customer's cost calculation.
Hole processing scheme 3
CNC shape milling process, use extended handle to install round or diamond-shaped alloy knife grains, deep layered processing, due to the large contact area, the sound is very loud and harsh every time the tool enters and exits, and the processed surface roughness The value and dimensional accuracy are very poor, and there are undercut grooves in the middle from time to time. Only the roughness cannot be controlled, which is far from the standard.
Hole processing scheme 4
For CNC boring processing, the model used is Model 850B, which can be used for general machine tools. The Z-axis height of this model is 500mm, which can meet the processing requirements of boring tool holder 230 and workpiece hole depth of 250mm, and the total processing time per hole It only takes 2 hours, the machining accuracy is high, and the surface roughness value and dimensional accuracy all meet the drawing requirements. Through the comparison of cost, processing accuracy and processing difficulty, the hole processing plan of plan 4 is selected.
CNC boring process
Clamping and alignment
Put the workpiece on the machine tool, tighten the position of the four corners, and level the parallel position and levelness of the workpiece. If it exceeds 0.03mm, the upper and lower sides of the workpiece must be reground, otherwise it is difficult to ensure the verticality of the hole. The calibration tolerance is controlled within 0.02mm. Among the 4 surfaces, the second step surface is used as the 0 surface of the Z-axis for processing, and there is enough space for lifting the tool as much as possible.
Boring tool holder
For the first rough machining, measure the dimension of the boring blade higher than the large tool holder with a table card, and reserve about 0.5mm on one side for rough machining, which is convenient for semi-finishing machining. The main deflection angle of the boring insert is 30°, the clearance angle of the flank is 15°, and the radius of the tool tip is R0.3~R0.4mm, so as to minimize the contact surface and force to prevent undercutting caused by vibration. The surface of the boring tool against the workpiece is 0.
Boring program
Command format G76X_Y_Z_R_Q_P_F_;, G76 is fine boring command, X/Y/Z hole coordinate position, P is pause at the bottom of the hole, Q means pause offset after tool processing, to prevent scratching the machined side when lifting the tool.
Rough machining parameter setting
The speed S is 120 rpm, the feed F is 80 mm/min, the cutting amount is 1.0 mm, the cutting oil is the cooling liquid, the fluidity of the oil needs to be good, and the cooling is in place.
Semi-finishing parameter setting
After the rough machining is completed, the card number and inspection are carried out. The size of the deep inner hole can be measured by the inner hole gauge, which usually has a certain taper. The speed S is 110 rpm, the feed F is 70mm/min, and the cutting amount is 0.6mm. The cutting oil is the cooling liquid, the fluidity of the oil needs to be good, and the cooling is in place to ensure the roughness of the finishing.
Finishing parameter settings
Each hole is processed with a new blade, the speed S is 100 rpm, and the feed is 60mm/min. The position of the blade is measured with a micrometer card, and the small tool holder is locked for processing. Test hole processing first, because there is a 15mm step on the top surface of the workpiece, until the size meets the drawing requirements.
3. Programming
picture
Note: For rough machining, intermediate machining and finishing machining, only change the value of F and S in the program content.
This set of processing plan has undergone several on-site improvements. It starts from the shape milling processing plan. In the middle, the knife needs to be lifted and changed several times. The processing time of each hole is about 4 hours. The roughness value processed makes the customer very happy. The headache caused it to take a day to polish a hole with the machine in the second process, and the roundness of the polished hole was not up to standard.
picture
Figure 3 boring tool holder
Boring machining mainly involves the setting of the two parameters of feed and speed. The feed speed is normally calculated as Vc=πDN/1,000. After many times of on-site processing and continuous improvement, it is finally concluded that the finishing speed S is 100 rpm. Feed F is 60mm/min. Although the result is simple and requires a lot of effort, it can be concluded that intermediate processing/semi-finishing and finishing can be completed in one time. The total processing time of each hole is within 2h. Cylindricity and roughness The values are all up to the standard, which reduces the customer's secondary processing time, really improves the production efficiency, and has won praise from customers.
Although this set of final boring processing plan is simple, the process is really not easy. If any detail is missing, the processing effect may be different. The most worrying thing about deep hole boring is that vibration will occur during processing, and excessive force will cause Undercut, the workpiece will be scrapped. Therefore, in the aspects of blade selection, precautions and other processing parameters, I hope it can play a role in reference and prevention.
