An individual boss has an annual output value of more than RMB 6 million, but the annual tool consumption accounts for more than 8% of the output value, which means that the annual tool consumption reaches 500,000.
Now that the market is not good, processing costs are getting lower and lower. He wants to save tool expenses and asked me if I have any good ideas?
I suggested that he start from the following two aspects:
1. Reasonable configuration of tools
Let him save money through the reasonable allocation of limited resources, which can be quantified from the following three aspects.
1. Reduce the number of tools in stock
2. Reduce tool purchase costs
3. Improve efficiency and steadily increase output value
In particular, his company's parts are produced in small batches and in many varieties, involving many types of tools. Not to mention abnormal consumption, it is easy to cost hundreds of thousands of idle and wasted tools.
The implementation steps of the above three points to optimize tool configuration from the aspect of information management are not within the scope of sharing today. Friends are welcome to leave a message and contribute your wisdom.
2. Specific applications of cutting tools
In the process of metal cutting, various cutting tools will continue to be consumed. The cutting tools have normal wear and abnormal wear.
Abnormal wear, the tool industry has done a lot of verification, and summarized 9 types of wear that often occur.
For each wear situation, I once gave specific solutions and countermeasures in my micro-course on tool application. Friends who learned it shouted that it was too valuable and saved the factory at least 100,000+ tool costs!
Haha, today, I will share 3 G code applications that everyone is familiar with from the perspective of CNC programming, allowing you to save tool costs.
These three G codes that everyone is familiar with are:
1. G97 command that specifies the spindle speed.
2. G96 command specifying constant linear speed.
3. G50 command specifying the maximum speed
Before sharing the G code application, let's take a look at the cutting parameters of a set of tools:
picture
There are three reference parameters Vc, Ap and Fn marked on the blade box;
1. Feed rate Fn
2. Linear speed Vc
3. Cutting depth Ap
Tool manufacturers have done a lot of verification to determine the impact of these three cutting parameters on tool life.
These three cutting parameters: speed, feed and depth of cut, all have an impact on tool life.
Among them, the cutting depth (Ap) has the smallest impact, and the feed rate (Fn) has a greater impact than the cutting depth. The cutting linear speed (Vc) has the greatest impact on the life of the insert.
For optimal tool life:
1. Maximize Ap- to reduce the number of tool passes
2. Maximize Fn- to shorten cutting time
3. Lower Vc- for optimal tool life
If the tool wears out too quickly...
The purpose is to reduce the linear speed Vc so as to obtain the best tool life.
How to do it specifically?
This involves the combined use of three G codes in CNC programming.
1. Command G97 specifying spindle speed
This command refers to the number of revolutions per minute that the machine tool spindle and workpiece rotate. The unit is r/min (revolution/minute).
Writing G97 S1000 into the program tells the machine tool that the spindle will rotate 1,000 revolutions per minute.
Yes, most people will specify the spindle speed in this way when programming.
The above conclusion drawn from a large number of practical verifications in the tool industry is that the parameter that has the greatest impact on the life of the insert is: cutting linear speed (Vc) rather than rotation speed n
So what is the relationship between the rotation speed n and the linear speed Vc?
2. Command G96 specifying constant linear speed
This command refers to the surface speed of a certain point on the workpiece. The unit is m/min (meters per minute).
It can be understood that when cutting a workpiece, the speed of any point on the outer circle or surface of the workpiece is the distance that this point on the surface of the workpiece moves per unit time (1 minute). (speed=distance/time).
For example, G96S100 means that a certain point rotates and moves 100 meters per minute.
picture
Linear speed Vc formula (speed = distance/time):
picture
Remark:
D: represents the diameter of the workpiece (if milling, D represents the diameter of the tool)
n: represents the rotation speed
The rotational speed n can be calculated:
picture
This is the relationship between the rotation speed n and the linear speed Vc.
If the tool wears out too quickly...
The purpose is to reduce the linear speed Vc so as to obtain the best tool life.
When programming, most people will use G97 to specify the spindle speed instead of the linear speed. What will happen?
For example: finishing outer circle (D1-D2)
picture
If you specify G97S1500 in the program
Diameter D1=50mm
Diameter D2=80mm
Through the formula:
picture
It can be calculated:
Linear speed Vc at diameter D1=235.5 m/min
Linear speed Vc at diameter D2=376.8 m/min
If G97 is used in the program, the linear speed will change as the diameter of the part changes.
Let me say the important things again:
1). Use G97 to specify the rotation speed in the program. As the diameter of the part changes, the linear speed will change.
2). The cutting linear speed (Vc) has the greatest impact on the life of the blade.
For example, in the above example, you can just write the result calculated by G97S1500 in the program:
Linear speed Vc at diameter D1=235.5m/min
Linear speed Vc at diameter D2=376.8 m/min
picture
Among them, the linear speed Vc=376.8 m/min has exceeded the maximum Vc range of the blade (the blade Vc range in the picture above: 140~320), so the wear of the blade becomes very fast!
3. Command to specify the maximum spindle speed (G50)
The meaning of this command is to control the maximum speed of the spindle;
For example, writing G50 S3000 in the program means that the spindle rotation speed does not exceed 3000 rpm.
Some friends may ask: Why should we use this command?
1). The G96 method is used in the program to specify the linear speed. As the diameter of the part becomes smaller, the spindle speed will increase. It can even be theoretically infinitely larger.
picture
2). The machine tool has a maximum speed. If the spindle speed increases (for example, the end surface of the lathe can theoretically increase infinitely) exceeding the maximum speed of the machine tool, it will cause a safety accident. Therefore, it is necessary to control the maximum spindle speed command G50.
For example: (finishing the outer circle and end face is as shown below)
Part material: steel (P)
Blade: CCMT 120404…
1. In terms of parts
This part requires turning the outer circle and the end face. If the program uses G97, due to the change in diameter, the linear speed will also change. In this way, the texture of the processed parts will be uneven, which will affect the surface finish of the parts. Therefore, it is recommended to use G96 and G50 to write programs.
2. In terms of cutting tools
Blade linear speed Vc: 140-320 (This reference data can be found in the blade box or tool sample for almost all blades)
Among the three elements of cutting (rotation speed, depth of cut, and linear speed), linear speed has the greatest impact on tool wear.
Therefore, when processing and debugging, Vc should be as low as possible, starting from a lower value, such as Vc=140.
The procedure is as follows:
(INSERT: CCMT120404)
T0101
N1(TURNING FACE)
G97S500M3
G0Z0
X52.M8
G50S3000 (set maximum speed)
G96S140 (setting line speed)
G99G1X0.0F0.2
G0Z0.5
…..
When turning the end face, the diameter D50 is turned to the center of the part 0, always at a constant linear speed of Vc=140; that is, the spindle speed gradually increases from S892 to S3000;
