Based on many years of on-site practical debugging experience, starting from the principles of metal tool cutting, combined with factors such as tool material, cutting parameters, wiper edge, leading angle, processing method and composite tool, six optimization methods are introduced to reduce cutting costs. The purpose of improving production efficiency.
01
Preface
The rapid development of my country's manufacturing industry has created huge economic benefits for our country and even the world. As market competition becomes increasingly fierce, cost reduction and efficiency improvement have become issues that every enterprise must face. In order to effectively reduce costs and increase efficiency, it is necessary to analyze the composition of production costs. Production cost consists of three parts: direct materials, direct labor and manufacturing overhead. Direct materials refer to labor objects in the production process, which are processed into semi-finished products or finished products, and their use value subsequently becomes another use value. Direct labor refers to the human resources consumed in the production process, which can be calculated by wages, welfare expenses, etc. Manufacturing expenses refer to facilities such as factories, machines, vehicles and equipment, materials and auxiliary materials used in the production process. Part of their consumption is included in the cost through depreciation, and the other part is through maintenance, fixed expenses, machine material consumption and auxiliary material consumption are included in the cost. This article optimizes several tool usage methods to reduce tool consumption costs and improve processing efficiency, thereby achieving the effect of saving machine tool usage costs.
02
Change tool material to improve processing efficiency
Commonly used tool materials include the following: high-speed steel, carbide, ceramics, CBN and PCD. CBN and PCD have higher hardness, highest wear resistance, and their materials are relatively brittle. High-speed steel has the best toughness, but its hardness is very low and its wear resistance is poor.
High-speed steel is a high-carbon alloy steel. The main alloy elements are tungsten, chromium, molybdenum, cobalt, vanadium and aluminum, etc., and contains a large amount of carbides. High-speed steel cutting tools have high toughness and relatively low hardness. The advantages are that they are cheap, have high plasticity, and can process almost all materials. They were the main materials used in early cutting tools. The disadvantages are that they require higher requirements on operators and require manual labor. Sharpening, and the cutting speed that high-speed steel materials can withstand is very low. For example, the workpiece material is 45 steel, the hardness is 250HBW, the cutting speed is 30~60m/min, and the cutting efficiency is low.
At present, the most commonly used tool material is coated carbide. The hardness and heat resistance of coated carbide tools are better than those of high-speed steel tools. It can withstand higher cutting speeds, with cutting speeds ranging from 100 to 300m/min[1].
Taking the outer circle of turning steel parts as an example, if carbide turning tools are used to replace high-speed steel turning tools, the cutting speed can be increased from 50m/min to 180m/min, and the efficiency is increased by more than 3 times, and carbide tools also have higher cutting tools. life. Carbide turning tools with replaceable blades do not need to be sharpened, just replace the blade, and the operator does not need to have sharpening skills.
In addition to high-speed steel and carbide cutting tools, there are also ceramics, CBN and PCD. These three materials have higher cutting speeds - more than 1000m/min, but their application range is limited. Ceramics and CBN are usually used to process cast iron workpieces and steel workpieces with high hardness above 50HRC. PCD is usually used to process aluminum, plastic, wood and carbide, but cannot process cast iron parts [2].
Taking aluminum alloy milling cutters as an example, the cutting speed of high-speed steel milling cutters is 120~300m/min. The recommended cutting speed of Mapal brand carbide milling cutters HP615 material is 700m/min, while milling cutters made of PCD material can be used. The cutting speed is 1500~2000m/min.
03
Effect of cutting parameters on tool life and production efficiency
In order to improve machining efficiency and tool life, it is necessary to determine whether the cutting parameters are reasonable and analyze the impact of each cutting parameter on tool life and efficiency. Cutting parameters include cutting speed (linear speed), feed speed and back cutting amount, also known as the three cutting elements.
3.1 Cutting speed vc
The relationship between cutting speed vc and spindle speed is vc=πDn/1000, where D is the effective diameter of the tool/workpiece (unit: mm), and n is the machine tool speed (unit: r/min). When the cutting speed is too high, flank wear will increase and the surface quality of the workpiece will deteriorate. When the cutting speed is extremely high, the insert will also undergo plastic deformation. The influence curve of cutting speed on tool life is shown in Figure 1.
picture
Figure 1 Effect curve of cutting speed on tool life
3.2 Feed speed vf
The calculation formula of feed speed is vf=fZZnn, fZ is the tool feed (unit is mm/z), Zn is the number of effective cutting edges (unit is units), n is the machine tool speed (unit is r/min). If the feed speed is too high, the chips will be uncontrolled, and the quality of the machined surface will deteriorate. The cutting power is high, and the chips will impact the tool or the machined surface. The influence curve of feed speed on tool life is shown in Figure 2.
picture
Figure 2 Effect curve of feed speed on tool life
3.3 The amount of back knife ap
The back cutting amount refers to the difference between the uncut surface and the cut surface. The influence curve of the back cutting amount on the tool life is shown in Figure 3.
picture
Figure 3 The influence curve of back cutting amount on tool life
Among the three cutting factors, cutting speed, feed speed and back engagement amount all have an impact on tool life. The impact of the back cutting amount is the smallest, the feed speed has a greater impact than the back cutting amount, and the cutting speed has the greatest impact on the life of the blade.
In order to obtain the highest tool life, the direction of the optimization parameters is: maximize the back engagement to reduce the number of tool passes; maximize the feed rate to shorten the cutting time; reduce the cutting speed to obtain the best tool life.
To improve roughing efficiency, you can start by optimizing the amount of back cutting. If there are many tool paths, increase the amount of back cutting and reduce the tool path, or increase the amount of back cutting, reduce the cutting speed, and improve tool life. , increase the feed speed and ensure processing efficiency.
3.4 Application examples
The flange produced by an automobile parts processing factory is shown in Figure 4. The existing processing solution is inefficient, and various cutting parameters need to be optimized to improve tool life and production efficiency.
picture
Figure 4 Flange
Optimize the processing plan by increasing the amount of back cutting, reducing tool paths, and reducing cutting speed. Before optimization, the tool paths were many and chaotic, but after optimization, the tool paths were clear, as shown in Figures 5 and 6. The parameters before and after optimization are shown in Table 1. After optimization, the tool life has been increased from 15 parts to 31 parts.
picture
Figure 5 Optimizing the front tool path
picture
Figure 6 Optimized tool path
Table 1 Parameters before and after optimization
picture
The factor that measures the cutting performance of the blade is the cutting speed. The CNC system reads the spindle speed. Many programmers only consider the speed when designing programs and ignore the diameter factor. However, in actual machining, the diameter factor also has a greater impact. Taking turning as an example, when the workpiece diameter D is 50mm and the machine tool speed n is 1000r/min, the linear speed vc=157m/min. When the workpiece diameter D is 100mm and the machine tool speed n is 1000r/min, the linear speed vc=314m/min.
According to the tool sample, the cutting speed of 314m/min is very high, close to the limit that the carbide blade can withstand. High cutting speed can accelerate the wear process of the tool and reduce the service life of the tool.
It can be seen from this that for the same machine tool speed, different workpiece diameters, and tool cutting speeds, when the tool life is too low, you can check whether it is caused by the cutting speed being too high.
04
The influence of wiper edge on cutting efficiency
The wiper blade has a tip angle composed of 3 to 9 arcs with different radii, and the arc radius can reach more than 900mm. The relationship between tool tip fillet, feed amount and surface quality is
Rmax＝fn²/8r(1)
Rmax (wiping edge) = Rmax/² (2)
In the formula, fn is the feed amount (mm/r); r is the tool tip fillet radius (mm); Rmax is the height difference between the peak and trough of the cutting surface (mm).
This method is suitable for finishing turning or boring. The wiper tool itself does not have a fast feed function. However, according to the previous formula, it can be inferred that the characteristics of the wiper tool are: when the processing parameters are the same, the surface quality of the wiper tool can be increased by 1 times; when the surface quality is the same, the feed speed of the wiper tool can be increased by 1 time. .
When the same surface quality is required, higher feed speeds can be used when using wiper tools.
Taking the processing of the end face of the output shell as an example of efficiency improvement, the workpiece material is QT500 and the surface roughness value Ra≤1.6μm is required. In order to improve the cycle time, a wiper blade was used. On the premise of meeting the same surface roughness requirements, the feed speed was increased from 0.36mm/r to 0.5mm/r. The measured surface roughness value Ra=1.33μm, and the blade life was the same. The various processing parameters using ordinary turning inserts and wiper inserts are shown in Table 2. The end face of the output shell after optimization is shown in Figure 7.
Table 2 Various processing parameters of ordinary turning inserts and wiper inserts
picture
picture
Figure 7 Optimized output shell end face
05
Effect of main deflection angle on cutting efficiency
The feed per tooth was mentioned in the previous brief introduction to the concept of feed speed. Some brands of tool samples recommend the maximum chip thickness hex as the cutting parameter instead of the feed per tooth. Because what determines the feed amount is the maximum chip thickness hex and the leading angle Kr of the tool. The conversion formula is hex=fzsinKr.
When the main deflection angle is 90°, fz=hex, the maximum chip thickness of the tool is the same as the feed per tooth. As the main deflection angle decreases, the feed speed can be increased.
Taking the square shoulder milling cutter (see Figure 8) as an example, the number of teeth ZN of the 90° square shoulder milling cutter is 5 flutes, n=1000r/min, hex=0.2mm, fz=0.2mm/z, machine tool feed speed vf =0.2×5×1000=1000 (mm/min).
picture
a) Square shoulder milling cutter structure diagram
picture
b) Physical objects
Figure 8 90° square shoulder milling cutter
45° leading angle face milling cutter (see Figure 9) ZN has 5 flutes, n=1000r/min, hex=0.2mm, fz=hex /sin45°=0.282mm/z, then the machine tool feed speed vf=0.282× 5×1000=1410 (mm/min).
picture
a) Structure diagram of face milling cutter
picture
b) Physical objects
Figure 9 45° square shoulder milling cutter
10° leading angle face milling cutter (see Figure 10) ZN has 5 edges, n=1000r/min, hex=0.2mm, fz= hex/sin10°=1.156mm/z, then the machine tool feed speed vf=1.156× 5×1000=5780 (mm/min).
picture
a) Signal
picture
b) Physical objects
Figure 10 10° square shoulder milling cutter
To sum up, at the same rotation speed of the same type of blade, the smaller the main deflection angle, the higher the feed speed that can be used. It is worth noting that the 90° square shoulder milling cutter mainly bears radial force, and the axial force approaches zero. As the main deflection angle decreases, taking the 10° main deflection angle milling cutter as an example, it mainly bears axial force. The radial force is very small. The smaller the main deflection angle, the greater the vibration tendency and the higher the power consumed.
06
The influence of processing methods on cutting efficiency
The cutting tool path also has a great impact on machining efficiency. For example, a recently popular dynamic milling method is an efficient trochoidal milling method with a large back cutting volume and a small cutting width. The difference from conventional trochoidal milling is that the dynamic milling process strictly adheres to the constant chip thickness hex. Has high metal removal rate. Since dynamic milling can ensure constant cutting force during tool cutting, the processing speed is fast and stable.
Taking milling of the outer contour of the valve body as an example to illustrate the impact of processing methods on cutting efficiency. The workpiece is made of stainless steel. The difficulty is that the tool length-to-diameter ratio reaches 4 times the diameter, which causes vibration during processing. The original plan used replaceable insert square shoulder milling cutters, which resulted in large cutting vibration due to the large aspect ratio. Unable to process normally. Optimized to use carbide end mills, large back cutting capacity, small cutting width, and dynamic milling method. The dynamic milling tool path simulation is shown in Figure 11, and the comparison parameters are shown in Table 3.
picture
Figure 11 Dynamic milling tool path simulation
Table 3 Parameter comparison
picture
07
Improve machining efficiency with composite tools
For high-volume products, composite tools are usually used to improve production efficiency, such as chamfer drills, composite boring tools (see Figure 12), etc.
picture
Figure 12 Compound boring tool
Composite tools use one tool to process multiple work steps, which improves processing efficiency and saves the tool change time of multiple tools. Composite cutting tools also have many shortcomings. The biggest drawback is that they are not universal. The cutting tools are only designed for a certain workpiece and cannot be used universally with other workpieces [3].
08
Conclusion
This article provides six ways to optimize cutting tools, which can provide guidance for improving production efficiency and reducing costs. The tool optimization method should be flexible and needs to be done on a practical basis. Before optimization, it is necessary to analyze the bottleneck process, optimize the tool in a targeted manner, and grasp the key points to solve the problem according to the specific production conditions.
