Tool setting is the main operation and important skill in CNC machining. Under certain conditions, the accuracy of tool setting can determine the machining accuracy of parts. At the same time, the efficiency of tool setting also directly affects the efficiency of CNC machining. It is not enough to just know the tool setting method. You must also know the various tool setting settings of the CNC system and the calling methods of these methods in the machining program. At the same time, you must know the advantages and disadvantages of various tool setting methods, as well as the conditions for use.
1. Tool setting principle The purpose of tool setting is to establish the workpiece coordinate system. Intuitively speaking, tool setting is to establish the position of the workpiece on the machine tool workbench, which is actually to find the coordinates of the tool setting point in the machine tool coordinate system. For CNC lathes, the tool setting point must be selected before machining. The tool setting point refers to the starting point of the tool movement relative to the workpiece when the workpiece is machined by a CNC machine tool. The tool setting point can be set on the workpiece (such as the design datum or positioning datum on the workpiece), or on the fixture or machine tool. If it is set at a certain point on the fixture or machine tool, the point must maintain a certain precision dimensional relationship with the positioning datum of the workpiece. When setting the tool, the tool position point should be coincident with the tool setting point. The so-called tool position point refers to the positioning reference point of the tool. For the turning tool, its tool position point is the tool tip. The purpose of tool setting is to determine the absolute coordinate value of the tool setting point (or the workpiece origin) in the machine tool coordinate system and measure the tool position deviation value of the tool. The accuracy of tool point alignment directly affects the processing accuracy. When actually processing the workpiece, using one tool generally cannot meet the processing requirements of the workpiece, and usually multiple tools are used for processing. When using multiple turning tools for processing, the geometric position of the tool tip point will be different after the tool change without changing the tool position. This requires that different tools can ensure the normal operation of the program when starting processing at different starting positions. In order to solve this problem, the machine tool CNC system is equipped with the function of tool geometry position compensation. Using the tool geometry position compensation function, as long as the position deviation of each tool relative to a pre-selected reference tool is measured in advance, it is input into the specified group number of the tool parameter correction column of the CNC system, and the T instruction is used in the processing program to automatically compensate the tool position deviation in the tool trajectory. The measurement of tool position deviation also needs to be achieved through tool setting operation. 2. Tool setting method In CNC machining, the basic tool setting methods include trial cutting method, tool setting instrument tool setting and automatic tool setting. This article takes CNC milling machine as an example to introduce several commonly used tool setting methods. 1. Trial cutting tool setting method This method is simple and convenient, but it will leave cutting marks on the workpiece surface, and the tool setting accuracy is low. As shown in Figure 1, the double-sided tool setting method is adopted with the tool setting point (here it coincides with the origin of the workpiece coordinate system) at the center of the workpiece surface as an example. (1) Tool setting in x and y directions. ① Mount the workpiece on the workbench through the fixture. When clamping, the four sides of the workpiece should leave space for tool setting. ② Start the spindle to rotate at medium speed, move the workbench and spindle quickly, let the tool move quickly to a position close to the left side of the workpiece with a certain safety distance, and then reduce the speed to move close to the left side of the workpiece. ③ When approaching the workpiece, use fine adjustment (usually 0.01mm) to approach, let the tool slowly approach the left side of the workpiece, so that the tool just touches the left surface of the workpiece (observe, listen to the cutting sound, see the cutting mark, see the chips, as long as any one of these conditions occurs, it means that the tool touches the workpiece), and then retreat 0.01mm. Note the coordinate value displayed in the machine tool coordinate system at this time, such as -240.500. ④ Retract the tool along the positive z direction to above the workpiece surface, and use the same method to approach the right side of the workpiece, and note the coordinate value displayed in the machine tool coordinate system at this time, such as -340.500. ⑤ Based on this, the coordinate value of the origin of the workpiece coordinate system in the machine tool coordinate system is
{-240.500+(-340.500)}/2=-290.500. ⑥ Similarly, the coordinate value of the origin of the workpiece coordinate system in the machine tool coordinate system can be measured. (2) Z-axis tool setting. ① Move the tool quickly above the workpiece. ② Start the spindle to rotate at medium speed, move the worktable and spindle quickly, and move the tool quickly to a position close to the upper surface of the workpiece with a certain safe distance, then reduce the speed to allow the tool end face to approach the upper surface of the workpiece. ③ When approaching the workpiece, use fine adjustment operation (generally 0.01mm) to approach, and let the tool end face slowly approach the workpiece surface (note that it is best to cut at the edge of the workpiece when the tool, especially the end mill, contacts the workpiece surface with an area less than a semicircle, and try not to let the center hole of the end mill cut on the workpiece surface), so that the tool end face just touches the upper surface of the workpiece, and then raise the axis again, and record the z value in the machine tool coordinate system at this time, -140.400, then the coordinate value of the workpiece coordinate system origin W in the machine tool coordinate system is -140.400. (3) Input the measured x, y, and z values into the machine tool workpiece coordinate system storage address G5* (generally use G54~G59 codes to store tool parameters). (4) Enter the panel input mode (MDI), enter "G5*", press the start key (in automatic mode), and run G5* to make it effective. (5) Check whether the tool setting is correct. 2. Tool setting with feeler gauge, standard mandrel, and block gauge This method is similar to the tool setting method with trial cutting, except that the spindle does not rotate during tool setting. A feeler gauge (or standard mandrel, block gauge) is added between the tool and the workpiece. The thickness of the feeler gauge should be subtracted when calculating the coordinates. Because the spindle does not need to rotate for cutting, this method will not leave marks on the workpiece surface, but the tool setting accuracy is not high enough. 3. Tool setting with edge finders, eccentric rods, and axis setters The operation steps are similar to the tool setting method with trial cutting, except that the tool is replaced with an edge finder or eccentric rod. This is the most commonly used method. It is efficient and can ensure tool setting accuracy. Be careful when using an edge finder to allow its steel ball to slightly contact the workpiece. At the same time, the workpiece to be processed must be a good conductor and the positioning reference surface must have a good surface roughness. The z-axis setter is generally used for transfer (indirect) tool setting.
