G73 Cycle Introduction
In CNC Machining Centers (CNC Milling machines) G73 command (G73 cycle) is used for drilling holes that are deep and that cannot be drilled in one time or that may result in tool breakage, chip jamming. With this cycle, the tool move to the coordinate specified in the program, rapidly approaches the height of Z specified by R, drills with the feed rate specified by F as much as the depth given by Q .. and is move up by the amount of “d” determined parameter setting. In Fanuc systems, this parameter is #5114, but it may vary depending on the controller model. Then it drills the hole with the amount indicated by Q and this process continues until the depth specified with Z.. is reached. If another coordinate is given afterwards, it moves there and the cycle continues to work as described above until the G80 command is issued.
The G83 cycle is also used to also for peck drilling. Although both have very similar cycles, in G83 cycle, the tool moves to the R (safety) distance specified in the cycle each time, while in the G73 cycle, it moves not up to the R distance but by the amount determined parameter setting from the position it is located (For example 1mm.).
As you can imagine, trying to drill deep holes in pne-step using G81 command will result may be tool breakage. For this reason, G73 or G83 cycles should be used according to needs.
|You may be interested also:|
|“CNC Milling | G83 Cycle | Peck Drilling”|
G73 Cycle Format
|G73 X… Y… Z… R… P… Q… F… K(L)… ;|
|G73 : Peck Drilling cycle|
|X : Hole position in X axis|
|Y : Hole position in Y axis|
|Z : Z axis end position = Z depth = Hole depth|
|R : Z axis start position = R level = Clearance|
|P : Dwell time at bottom of hole|
|Q : Depth to increase on each peck|
|F : Feedrate|
|K or L : Number of repeats|
Things to Know
- X and Y coordinates where the hole will be drilled are not usually given in the same line. Instead, the machine is sent to the first hole coordinate in the program, and then drilling with the G73 cycle is started.
- In general, the cycle is not repeated with K.
- 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 G73 cycle is usually used with the G98 command. You can find details about the G98 and G99 command on our website.
- After using the G73 cycle, the cycle must be canceled with the G80 command. If it is not canceled with G80, your machine will drill holes with the conditions specified in the G73 line in every different coordinate included in the program.
- If the command is used with G98, it will use the Z height that it uses to “drill the first hole” when moving between the coordinates to be drilled.
- If the command is used with G99, it will use the R height “when moving between the coordinates to be drilled”.
- If the program is stopped during G73 cycle and some manual movements are made, it must be moved to the point where the program is stopped manually before starting the program again.
- The G73 command is not work 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 G73 command is written.
G73 Cycle Examples
G73 CNC Program Example – 1
T8 M6 ;
M03 S1500 ;
G90 G54 G0 X0 Y0 ;
G43 H8 Z20 M08 ;
G98 G73 X25 Y25 Z-60 R6 Q7 F160 ;
G91 Y30 ;
X35 Y10 ;
X35 Y10 ;