Wang Xiaoling from Guangdong University of Technology detailed the manual recovery and reprocessing technology for CNC machining interruptions, which allows the machine tool to resume processing from the point of interruption, saving processing time and improving production efficiency. She also cited an application example of toy mold machining interruption. 1 Introduction In CNC machining production, we often encounter situations where the CNC machining of a mold, which has lasted for several hours or more than ten hours, is about to be completed, but due to certain reasons (such as power outage, tool breakage, alarm, etc.), the machining has to be interrupted. After the interruption event is dealt with, when the CNC machine tool wants to restart the machining, it often has to start from the beginning of the program, resulting in a large amount of idle running of the machine tool and reducing the machining efficiency. In order to save machining time and improve production efficiency, the best way is to resume the original machining from the point of interruption. Currently, there are three methods to achieve such reprocessing: (1) Reprocessing by manually recovering the interrupted program; (2) Reprocessing by using the machine tool's built-in breakpoint recovery function; (3) Automatic recovery of machining by using specially developed "program restart" software. However, the latter two are limited by machine tools or software, and their actual operation is quite passive and inflexible. In fact, it is not difficult to manually recover from the interruption of CNC machining. As long as you master the key points of the method and have certain manual programming knowledge, you can easily achieve it. 2 Manual recovery and reprocessing method for CNC machining interruption The operation of CNC machine tools is controlled by the programmed program. Therefore, how to obtain the interruption point of the program and its reprocessing status so that it can be reprocessed correctly and safely becomes the key to this method. The author divides the manual recovery and reprocessing method for CNC machining interruption into the following four points. 2.1 Obtaining the breakpoint information when the machine tool interrupts machining (1) If a broken tool or alarm occurs during CNC machining, causing the machining to be unable to continue, the program should be interrupted. You can press the "feed hold key" or "emergency stop switch" on the machine tool panel. (Generally, the "reset" key should not be pressed, because the reset key of some CNC machine tools (such as the SYNTEC 900M system) will cause the loss of machining information - the current absolute coordinate value and line number, resulting in the breakpoint information when the machining is interrupted being lost due to the system reset.) (2) Copy down the breakpoint information on the controller panel when the machine is interrupted: the current line number, absolute coordinate value and tool number. 2.2 Search the NC program according to the breakpoint information to determine the breakpoint position of the NC program and calculate the remachining position of the NC program. When resuming machining, the tool can be directly cut to the breakpoint to continue machining. However, it is difficult to determine the accurate coordinates of the breakpoint. Even if the coordinates of the breakpoint are accurately obtained, such remachining will leave obvious tool marks at the breakpoint, resulting in discontinuity of the machining surface at the breakpoint, thus affecting the machining accuracy. In order to achieve a smooth transition of the breakpoint, when resuming machining, the NC program should be rolled back several lines from the breakpoint, and then the end position of the last complete program segment before that position should be determined. This position is the "remachining position". [IMG=Figure 1 Height Parameters]/uploadpic/THESIS/2007/11/2007111411104278647J.jpg[/IMG] [align=center]Figure 1 Height Parameters[/align] [IMG=Figure 2 Mickey Mouse Punch]/uploadpic/THESIS/2007/11/2007111411105753340E.jpg[/IMG] Figure 2 Mickey Mouse Punch When the machine tool restarts, the tool starts machining directly from the re-machining position. Since the surface between the re-machining position and the interruption point has already been machined, executing the corresponding NC program again will not cut to the workpiece surface, but will smoothly transition to the re-machining position while closely adhering to the workpiece surface before starting actual machining, thus ensuring good machining accuracy. The difference between CNC milling machines and machining centers in determining the reprocessing location is as follows: CNC milling machines do not have automatic tool changing functionality. Their programs are written according to predefined machining operations and are divided based on the tool—one tool per program. Therefore, the search for interrupted programs can start directly from the program beginning. Machining centers, on the other hand, have automatic tool changing functionality, and their entire machining process is contained within a single program. Therefore, to save search time and effort, the search should begin from the part of the program where the interrupted tool was located. It is important to note that the breakpoint location should not be determined solely by the program's interrupt line number. In larger NC programs, there may be several program segments with the same line number; for example, in the following program, there are as many as 24 program segments with line number N3110. Therefore, the absolute coordinates at the time of the interruption must be considered to confirm the breakpoint location. ┇ N31lOX4.351Y-29.075Z-12.387 ┇ N3110X-6.742Y-30.214Z-15.543 ┇ N3110X-2.097Y-23.792Z-10.789 ┇ N31lOXl.51Y-18.523Z-9.425 ┇ N3110X-9.01Y-21.826Z-10.652 ┇ N3110X-6.87Y-17.958Z-10.52 ┇ N8952250． N8954M5 N8956X0.Y0.M9 N8960M30 % 2.3 Determine the machining state at the remachining position The machining state at the remachining position is the initial machining state value when the program resumes machining, including preparation function words, auxiliary function words, process parameters, etc. A complete CNC program consists of several program segments. Different CNC systems often have different program segment formats. Modern CNC machine tools widely adopt the variable program segment format. The characteristics of this format are: there is no strict requirement for the order of code words, and unnecessary code words and modal instructions that are the same as the previous segment can be omitted. Therefore, it is difficult to determine the state information related to the remachining position from only one program segment. Therefore, the specific way to determine the machining state at the remachining position is: search the program back from the remachining position to find useful machining state parameters. (1) Find the C, T, H, F, S codes and record their values. The G code, tool number and its compensation method, feed rate, spindle speed, etc. are the basic state information of a certain point in the machining process. (2) Determination of height parameters (as shown in Figure 1) ① Determination of safety height. For milling, the starting point and retraction point must be a safe height away from the upper surface of the workpiece to ensure that the tool does not collide with the workpiece or fixture when it is stopped. The plane where the tool center (or tool tip) is located at the safety height position is also called the safety plane. ② Determination of feed depth. In CNC machining, in order to save time, the tool uses rapid traverse (i.e., GOO speed) when idling. However, the re-machining position is usually inside or on the workpiece. If the tool directly descends to the re-machining position at GOO speed and uses a vertical descent method, it is easy to cause inertial overcut or collision with the workpiece. To avoid this situation, the tool should be moved rapidly from the safety plane to the machining position (i.e., the X and Y coordinate values ​​of the re-machining position) at GOO speed, then quickly descend to the specified height, and then switch to feed depth to the machining surface (i.e., the Z coordinate value of the re-machining position). This specified height is called the feed advance height, which is the starting point for the tool to switch from rapid traverse to feed when it enters the machine. This feed advance height value should be 2-5mm greater than (i.e., higher than) the Z-coordinate value of the remachining position. 2.4 Based on the determined remachining position and its status information, the original program is appropriately modified to obtain a new remachining program. To enable the machine tool to continue the original machining from the point of interruption, the original program needs to be appropriately modified or deleted. An NC program generally consists of three parts: program header, program body, and program tail. Therefore, the new remachining program should also include these three parts. The program header of the new program is used to restore the machining state set during machining. Therefore, the modification or deletion of the original program mainly targets the program segment between the remachining position and the program header: a new program is generated based on the obtained remachining position and its status parameters and the original program header format. 3 Application Example The Mickey Mouse punch shown in Figure 2 was machined on a CNC milling machine with a KND-200 CNC system and an MV-5F machine tool model. The tool broke during the machining, so the program execution was interrupted. The relevant information on the controller panel at the time of the interruption was copied down: the current machining line number is N3110, and the absolute coordinates are (X-17.243, r-1.406, Z-13.159). The original program was opened with Notepad or other opening methods and the following modifications were made: (1) The CNC milling machine does not have an automatic tool change function, so the program can be searched directly from the program header of the interrupted program. (2) Combining the copied interrupted machining line number and absolute coordinate value, the program breakpoint was searched using the search function. After searching, the program segment with the 7th line number N3110 was the breakpoint location, which is the bold part of the program shown below. % N102GOGl7G40CA9G80G90 N106GOG90X34.88Y-35.S1500M3 N110Z-12.951M8 N112GlZ-15.951F300． N114X35.Y-34.931F600． ┇ N3110) (4.351Y-29.075Z-12.387 ┇ N3110X-6.742Y-30.214Z-15.543 ┇ N3110X-2.097Y-23.792Z-10.789 ┇ N31lOXl.51Y-18.523Z-9.425 ┇ N3110X-9.01Y-21.826Z-10.652 ┇ N3110X-6.87Y-17.958Z-10.52 ┇ N3108X17.163Y-1.451Z-13.029 N3110X17.241Y-1.406Z-13.159；Breakpoint N3112X17.319Y-1.361Z-13.293 ┇ N8950GOZ-12.951 N8952250． N8954M5 N8956X0.Y0.M9 N8960M30 % (3) Determine the reprocessing position. Roughly estimate the time elapsed from the tool break to the interruption of processing, and determine that the reprocessing position is the program segment N3000, which is backtracked from the breakpoint position determined in the previous step — (X11.821, Y-4.535, Z-9.601), as shown in the bold part of the program below: ┇ N3110X-6.87Y-17.958Z-10.52 ┇ N2998X11.714Y-4.597Z-9.598 N3000X11.821Y-4.535Z-9.601；Reprocessing position N3002X11.928Y-4.473Z-9.606 ┇ N3108X17.163Y-1.451Z-13.029 N3110X17.241Y-1.406Z-13.159；Breakpoint┇ (4) Determine the processing status of the reprocessing position. Search backwards from the program segment where the reprocessing position is located to determine the C code, F speed, etc. of the program segment. In this example, the processing status at the reprocessing position is: C code is C01, Z feed rate is 300, XY feed rate is 600. ┇ N110Z-12.951M8 N112G1Z-15.951F300． N114X35.Y-34.931F600． (5) Delete the processed program segment. Delete the program segment from the reprocessing position back to the XY tool entry position. % N102GOGl7C,40G49C～0G90 N106GOG90X34.88Y-35.S1500M3; The scribing part is the XY tool entry position N3000X11.821Y-4.535Z-9.601; Reprocessing position┇ (6) Modify the program header: ① Replace the XY tool entry coordinates (X34.88, Y-35.) in the program header with the X and Y coordinates (X11.821, Y-4.535) of the reprocessing position. % N102GOGl7C,40C～9G80G90 N106GOG90X11.821Y-4.535S1500M3; Tool entry position N3000X11.821Y-4.535Z-9.601; Re-machining position ┇ ② Add the feed entry height value to the next line of the program segment. The Z coordinate of the re-machining position is -9.601, so the feed entry height value is set to 6. N106GOG90X11;821Y-4.535S1500M3 N108Z-6.M8; Feed entry height N3000X11.821Y-4.535Z-9.601 ┇ ③ Add the correct feed entry program segment: ┇ N108Z-6.M8; Feed depth N110G1Z-9.601F300.; Added G code, depth of cut (i.e., coordinate 2-9.601 of the re-machining position) and feed speed N3000X11.821Y-4.535Z-9.601 ┇ ④ Add the correct C code and XY feed speed in the program segment of the re-machining position (in this example, the G code instruction in the N3000 line program segment is the modal instruction C1, which is the same as the previous line, so it can also be omitted). N110GlZ-9.601F300． N3000G1X11.821Y-4.535Z-9.601F600． ; Added G code and XY feed speed ┇ （7） Save the modified program with a different name. 4 Conclusion This article primarily introduces methods for NC programs using absolute coordinates. For NC programs that alternate between absolute and relative coordinates, this method is more cumbersome, and without a thorough understanding of manual programming, errors and accidents are easily caused. Therefore, the author does not recommend manual methods for NC programs that alternate between absolute and relative coordinates. The author has used the methods described in this article to help company technicians solve the problem of having to start machining from scratch due to CNC interruptions on numerous occasions. (Proceedings of the 2nd Servo and Motion Control Forum; Proceedings of the 3rd Servo and Motion Control Forum)