Share a G code application written many years ago, which is still of great value now...
Solution: Save tool costs from a programming perspective.......
Suitable for the following groups of people:
❶Business owner, technical backbone
❷ Workshop technicians, programmers
❸Tool Application Engineer
❹What you want to improve
The text is as follows:
I have a student who is an individual boss. The annual output value of the enterprise is more than 6 million, but the annual tool consumption accounts for more than 8% of the output value, that is, the annual tool consumption reaches 500,000.
Now the market is not good, and the processing cost is getting lower and lower. He wants to save tool expenses, and ask me what is the best way?
I suggest that he start from the following two aspects:
First, the reasonable configuration of the tool
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 the purchase cost of tools
3. Efficiency improvement to steadily increase output value
In particular, his company has small batches of parts and many varieties, which involve many types of tools. Not to mention abnormal consumption, it is easy to realize that the cost of idle and wasted tools exceeds hundreds of thousands.
The above three points to optimize the implementation steps of tool configuration from the aspect of information management are not in the scope of today’s sharing. Friends are welcome to leave a message to contribute your wisdom.
Second, the specific application of the tool
In the process of metal cutting, various tools will be continuously consumed, and the tools have normal wear and abnormal wear.
For abnormal wear, the cutting 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 tool application micro-class.....
Today, from the perspective of CNC programming, I will share 3 G code applications that everyone is familiar with, so that you can save tool costs.
These three G-codes that everyone is familiar with are:
1. G97 command specifying the spindle speed.
2. Specify the G96 command of constant linear speed.
3. G50 instruction specifying the maximum speed
Before sharing the G code application, let's look at the cutting parameters of a set of tools:
picture
There are three reference parameters Vc, Ap, Fn marked on the blade box;
1. Feed rate Fn
2. Line speed Vc
3. Cutting depth Ap
Tool manufacturers have done a lot of verification to get 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 depth of cut (Ap) has the least influence, and the influence of feed rate (Fn) is greater than the depth of cut. The cutting line speed (Vc) has the greatest impact on the life of the insert.
For optimum tool life:
1. Maximize Ap- to reduce the number of tool passes
2. Maximize Fn- to shorten cutting time
3. Reduce Vc- to get the best tool life
If the tool wears out too quickly.....
It is to reduce the line speed Vc, so as to obtain the best tool life.
How to do it?
This involves the coordinated use of three G codes in NC programming.
1. Command G97 for specifying the 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 (rev/minute).
Writing G97 S1000 in the program is to tell the machine tool spindle to rotate 1000 revolutions per minute.
Yes, most people will specify the spindle speed in this way when programming.
According to the conclusion obtained from a large number of practical verifications in the tool industry above, the parameter that has the greatest impact on the life of the blade is: cutting line speed (Vc) rather than rotational speed n
So what is the relationship between the rotational speed n and the linear velocity Vc?
2. Command G96 for specifying constant linear speed
This command refers to the surface speed of a certain point of the workpiece. The unit is m/min (meter/minute).
It can be understood that when the workpiece is cut, the speed of any point on the outer circle of the workpiece or on the surface is the distance moved by this point on the surface of the workpiece 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 velocity 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 rotational speed
The rotational speed n can be calculated:
picture
This is the relationship between the rotational speed n and the linear velocity Vc.
If the tool wears out too quickly.....
It is to reduce the line speed Vc, so as to obtain the best tool life.
When programming, most people will use the G97 method 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
By formula:
picture
It can be calculated that:
Linear velocity Vc at diameter D1=235.5 m/min
Linear velocity Vc at diameter D2=376.8 m/min
If G97 is used in the program, the line speed will change as the diameter of the part changes.
Important things to say again:
1). Use G97 to specify the speed in the program, and the linear speed will change as the diameter of the part changes
2). The cutting line speed (Vc) has the greatest impact on the life of the blade.
For example, in the above example, you just write the calculation of G97S1500 in the program:
Linear velocity Vc at diameter D1=235.5m/min
Linear velocity Vc at diameter D2=376.8 m/min
picture
Among them, the linear velocity Vc=376.8 m/min has exceeded the tolerance range of the maximum Vc of the blade (the blade Vc range in the above picture: 140~320), so the wear of the blade will become very fast!
3. Command to specify the maximum spindle speed (G50)
The meaning of this command is the command to control the maximum speed of the spindle;
For example, writing G50 S3000 in the program means that the rotation speed of the spindle does not exceed 3000 revolutions per minute.
Some friends may ask: Why use this command?
1). The program uses G96 to specify the linear speed. As the diameter of the part becomes smaller, the spindle speed will increase. It can even theoretically become infinitely larger.
picture
2). The machine tool has a maximum speed. If the spindle speed increases (such as the end face of the car, it can be infinitely increased in theory), exceeding the maximum speed of the machine tool 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 as shown in the figure 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, the line speed will also change due to the change of the diameter. In this way, the texture of the processed part will be uneven, which will affect the surface finish of the part. Therefore, it is recommended to use G96 and G50 to write the program.
2. In terms of tools
Blade linear speed Vc: 140-320 (almost all blades can be queried on the blade box or tool sample for this reference data)
Among the three elements of cutting (speed, depth of cut, and line speed), the line speed has the greatest influence on tool wear.
Therefore, when processing and debugging, try to get the bottom point of Vc, and start with 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 (set line speed)
G99G1X0.0F0.2
G0Z0.5
…
When turning the end face, the diameter D50 is turned to the center of the part 0, and the linear speed is always constant at Vc=140; that is, the spindle speed is gradually increased from S892 to S3000;
