In CNC machining, the actual position of the tool is often different from the theoretical position of the tool during programming. This is why we need to modify the program according to the position of the tool. However, as everyone knows, how complicated and error-prone it is to modify the program Therefore, the concept of tool compensation came into being. The so-called tool compensation is a function used to compensate the difference between the actual installation position of the tool and the theoretical programming position. After using the tool compensation function, changing the tool only needs to change the tool position compensation value without modifying the NC program.
In tool compensation, we often use length compensation and radius compensation. Generally, it is difficult for people who are new to the CNC industry to use these two compensations skillfully. Below we will explain these two compensation methods in detail.
picture
1. Tool length compensation
1. The concept of tool length compensation
First of all, we should understand what is the tool length. Tool length is a very important concept. When we program a part, we must first specify the programming center of the part, and then establish the workpiece programming coordinate system, and this coordinate system is only a workpiece coordinate system, and the zero point is generally on the workpiece. The length compensation is only related to the Z coordinate. It is not like the programming zero point in the X and Y planes, because the tool is positioned by the spindle taper hole and does not change. The zero point of the Z coordinate is different. Every knife is a different length.
For example, we want to drill a hole with a depth of 50mm, and then tap a hole with a depth of 45mm, using a drill bit with a length of 250mm and a tap with a length of 350mm. First use the drill bit to drill a hole with a depth of 50 mm. At this time, the machine tool has set the zero point of the workpiece. When the tap is replaced for tapping, if both knives start processing from the set zero point, the tap is longer than the drill bit and the tapping is too long, which will damage the tool. and artifacts. If tool compensation is set at this time, the length of the tap and the drill is compensated. After the zero point of the machine tool is set, even if the length of the tap and the drill is different, due to the existence of compensation, when the tap is called to work, the Z coordinate of the zero point has automatically moved to Z+ (or Z) compensates the length of the tap and ensures the correct machining zero point.
2. Tool length compensation command
Tool length compensation is realized by executing commands containing G43 (G44) and H. At the same time, we give a Z coordinate value, so that the tool moves to a place where the distance from the workpiece surface is Z after compensation. Another command G49 is to cancel the G43 (G44) command. In fact, we don’t need to use this command, because each tool has its own length compensation. When changing the tool, use the G43 (G44) H command to give its own tool length compensation. However, the length compensation of the previous tool is automatically canceled.
G43 means the addition of the compensation amount in the memory to the end point coordinate value of the program instruction, G44 means subtraction, and G49 or H00 can be used to cancel the tool length offset. In the program segment N80G43 Z56 H05, if the value in the memory of 05 is 16, it means that the coordinate value of the end point is 72mm.
3. Two ways of tool length compensation
(1) Use the actual length of the tool as the tool length compensation (this method is recommended). Using the tool length as compensation is to use the tool setting instrument to measure the length of the tool, and then input this value into the tool length compensation register as tool length compensation.
Using the tool length as the tool length compensation can avoid constantly modifying the tool length offset in the processing of different workpieces. In this way, a tool can be used on different workpieces without modifying the tool length offset. In this case, you can file each tool according to certain tool numbering rules, and use a small sign to write the relevant parameters of each tool, including the length and radius of the tool. For those companies with special tool management departments, there is no need to tell the parameters of the tool face to face with the operator. The tool length value on the label is used as tool length compensation without further measurement.
Using the tool length as tool length compensation can also allow the machine tool to measure the length of other tools on the tool setting instrument while the machine tool is running, without taking up the running time of the machine tool because of the tool setting on the machine tool, so that the machining center can be fully utilized. efficiency. In this way, when the spindle moves to the programmed Z coordinate point, it is the spindle coordinate plus (or subtracted) the Z coordinate value after tool length compensation.
(2) Use the distance (positive or negative) between the tool nose and the programmed zero point in the Z direction as the compensation value. This method is suitable for use when the machine tool is operated by only one person and there is not enough time to use the tool setting instrument to measure the length of the tool. In this way, when another workpiece is processed with one tool, the setting of the tool length compensation must be performed again. When using this method for tool length compensation, the compensation value is the tool nose movement distance when the spindle moves from the Z coordinate zero point of the machine tool to the workpiece programming zero point, so this compensation value is always negative and very large.
2. Tool radius compensation
1. The concept of tool radius compensation
During contour machining, the tool center movement trajectory (the movement trajectory of the tool center or wire center) and the actual contour of the machined part must be offset by a certain distance. This offset is called tool radius compensation, also known as tool center offset.
Since the CNC system controls the tool center trajectory, the CNC system needs to calculate the tool center trajectory based on the input part contour size and tool radius compensation value. According to the tool compensation instruction, the CNC machining machine tool can automatically perform tool radius compensation. Especially in manual programming, tool radius compensation is very important. When programming manually, using the tool radius compensation command, you can program according to the contour value of the part, without calculating the tool center trajectory programming, which greatly reduces the amount of calculation and error rate. Although using CAD/CAM automatic programming, the amount of manual calculation is small, and the speed of generating the program is fast, but when the tool has a small amount of wear or the machining contour size deviates slightly from the design size, or in rough milling, semi-finish milling and finish milling. When the step-by-step machining allowance changes, it still needs to be adjusted appropriately. After using the tool radius compensation, there is no need to modify the tool size or modeling size to regenerate the program. It is only necessary to properly modify the tool compensation parameters on the CNC machine tool. . It not only simplifies the programming calculation, but also increases the readability of the program.
Tool radius compensation has two compensation forms: B function (Basic) and C function (Complete). Because the tool radius compensation of the B function only calculates the tool compensation according to this program, it cannot solve the transition problem between program segments, and requires the workpiece contour to be processed into a round corner transition, so the manufacturability of the sharp corner of the workpiece is not good. Moreover, programmers must estimate in advance the discontinuities and intersections that may appear after tool compensation, and manually process them, which obviously increases the difficulty of programming; while the C function tool radius compensation can automatically handle the transfer of tool center paths between two program segments, which can be It is programmed completely according to the contour of the workpiece, so almost all modern CNC machine tools use C function tool radius compensation. At this time, it is required that at least two subsequent blocks of the tool radius compensation block must have a displacement command (G00, G01, G02, G03, etc.) specifying the compensation plane, otherwise the correct tool compensation cannot be established.
2. Tool radius compensation command
According to ISO regulations, when the tool center track is on the right side of the forward direction specified by the program, it is called right tool compensation, which is represented by G42; otherwise, it is called left tool compensation, which is represented by G41.
G41 is the tool left compensation command (left tool compensation), that is, viewed along the tool advancing direction (assuming the workpiece does not move), the tool center track is located on the left side of the workpiece contour, which is called left tool compensation.
G42 is the tool right compensation command (right tool compensation), that is, looking along the tool’s forward direction (assuming the workpiece does not move), the tool center track is located on the right side of the workpiece contour, which is called right tool compensation.
G40 is a command to cancel tool radius compensation. After using this command, the G41 and G42 commands are invalid.
