G74 Cycle Introduction
In CNC Machining Centers (CNC Milling machines) G74 command (G74 cycle) is used for left hand rigid tapping (threading in the hole) operations.
How it Works?
With this cycle, the tool goes to the coordinate specified in the program, quickly approaches the height of Z specified by R, machine will be threading in accordance with the line marked with F in the command line, and goes back to the distance R with rapid movement.
Pitch amount can be given directly or by calculating according to the model of the control unit. In some control units, the F value may be a direct pitch (For example: F1.5) and in some controls it may be calculated (For example: Revolution 400, the desired pitch is 1.5 = F = 600). If the relevant threading process is completed and another coordinate is given afterwards, the machine moves there and the cycle continues to work as described above until the G80 command is given.
Q parameter should be used together with the G74 command (G74 cycle) to prevent jamming of the chip and discharge the chip out of the piece during the relevant left-hand tapping process for deep hole. If the machine is supported by the Q variable to be added to the relevant thread cutting line, the system will move related axis ( Most of time Z ) given in the Q variable and goes up to the distance R and descends to remove the chip.
|You may be interested also:|
|“CNC Milling | G84 Cycle | Rigid Tapping”|
G74 Cycle Format
|G74 X… Y… Z… R… Q… F…|
|G74: Stepped or direct left hand rigid tapping (left-hand thread cutting) cycle|
|X: X coordinate of the hole to be tapped|
|Y: Y coordinate of the hole to be tapped|
|Z: Tapping depth|
|R: Point to start tapping (Threading) (Approach distance)|
|Q: The amount of pass to be taken each time (Optional / If control unit supports)|
|F: Pitch value (It should be entered directly or by calculation as mentioned above.)|
Things to Know
- The X and Y coordinates to which the left hand tapping are usually not given on the same line. Instead, the machine is sent to the first hole coordinate in the program, and then tapping starts with the G74 cycle.
- In general, the cycle is not repeated with K. (Therefore, it is not shown when describing the format above.)
- What is written in the first two items describes the methods generally used by the users in the market. The command format has been written technically appropriate. The command I want you to know can be written and applied as described here, although the first two items are frequently encountered in the market due to the ease of control of the program and the ease of writing.
- The G74 cycle is usually used with the G98 command. You can find details about the G98 and G99 command on our site.
- The cycle must be canceled with the G80 command after using the G74 cycle. If it is not canceled with G80, your machine will try to left hand tapping each different coordinate in the program with the conditions specified in the G74 line.
- If the command is used with G98, it will use the Z height that it uses when going “first left hand tapping” when moving between the coordinates to be pulled.
- If the command is used with G99, it will use the R height “when moving between the coordinates to be pulled”.
- The program should not be stopped and restarted during the G74 cycle. In this case, the thread extraction process will be impaired since the pitches will not be same with the starting position.
- The G74 command is not run under MDI mode. Although it is technically related to machine type, control unit type and parameters, not running cycles under MDI mode is more suitable for work safety and correct machining of the workpiece.
- M98 and M99 commands are not used in lines where G74 command is written.
- While the G74 command is running, the system does not allow to check or change tapping feedrate generally for the correct pitch. Even if there is no such restriction in the system, cutting progress should be left at 100% and should never be changed during thread cutting.
G74 Cycle Examples
G74 CNC Program Example – 1
G43 H1 Z50 M03 S600;
G90 G54 G00 X27 Y21;
G98 G74 Z-21 R10 F1200;