Complete set of CNC system instructions during the operation of CNC milling and punching machines

Complete set of CNC system instructions during the operation of CNC milling and punching machines

1. Pause instruction

G04X (U)_/ P_ It refers to the tool pause time (feed stops, spindle does not stop), and the value after address P or X is the pause time. The value after X must have a decimal point, otherwise it is calculated as one thousandth of this value in seconds (s). The value after P cannot have a decimal point (i.e. an integer) and is measured in milliseconds (ms).

For example, G04X2.0; Or G04X2000; Pause for 2 seconds

G04P2000;

However, in some hole system processing instructions (such as G82, G88, and G89), in order to ensure the roughness of the hole bottom, there needs to be a pause time when the tool is processed to the hole bottom. At this time, it can only be represented by address P. If address X is used, the control system considers X to be the X-axis coordinate value for execution.

For example, G82X100.0Y100.0Z-20.0R5.0F200P2000; Drill (100.0100.0) to the bottom of the hole and pause for 2 seconds

G82X100.0Y100.0Z-20.0R5.0F200X2.0; Drilling (2.0100.0) to the bottom of the hole will not pause.

2. Differences and connections between M00, M01, M02, and M30

M00 is an unconditional pause instruction for the program. The program execution stops at this feeding point and the spindle stops rotating. To restart the program, you must first return to the JOG state, press CW (spindle forward rotation) to start the spindle, and then return to the AUTO state, press the START key to start the program.

M01 is a program selective pause instruction. Before the program can be executed, the OPSTOP button on the control panel must be opened. The effect after execution is the same as M00, and the program needs to be restarted as above.

M00 and M01 are often used for inspection or chip removal of workpiece dimensions during machining.

M02 main program end instruction. Execute this command, the feed stops, the spindle stops, and the coolant is turned off. But the program cursor stops at the end of the program.

M30 main program end instruction. The function is the same as M02, but the difference is that the cursor returns to the program header position, regardless of whether there are other program segments after M30.

3. The meanings of addresses D and H are the same

The tool compensation parameters D and H have the same function and can be interchanged freely. They all represent the address name of the compensation register in the CNC system, but the specific compensation value is determined by the compensation number address after them. However, in the machining center, in order to prevent errors, it is generally artificially specified that H is the tool length compensation address, the compensation number is from 1 to 20, D is the tool radius compensation address, and the compensation number starts from 21 (the tool library for 20 tools).

For example, G00G43H1Z100.0;

G01G41D21X20.0Y35.0F200;

4. Mirror command

Mirror machining instructions M21, M22, and M23. When only mirroring the X-axis or Y-axis, the cutting sequence (clockwise and counterclockwise milling), tool compensation direction, and arc interpolation direction during cutting will be opposite to the actual program, as shown in Figure 1. When simultaneously applying