G82 Cycle Introduction
In CNC Machining Centers (CNC Milling machines) it may be necessary to hold the cutter drill at the end of the hole to obtain smooth surfaces at the bottom of the hole in blind holes. The G82 cycle is used for drilling operations that should be wait at the bottom of the hole.
With this cycle, the drilling tool goes to the coordinate specified in the program, quickly approaches the height of Z specified by R, drill the workpiece depth given by Z .. with the feedrate indicated by F, wait at the bottom of hole indicated by P and goes back to the distance R with rapid movement. If another coordinate is given afterwards, it moves there and the cycle continues until G80 is commanded.
The operating logic of G81 and G82 commands are the same. The only difference between the two is that when the tool reaches the bottom of the hole in the G81 cycle, it immediately returns with G0 speed, while in the G82 cycle, the tool waits for the time given by P and then back with the G0 speed.
|You may be interested also:|
|“CNC Milling | G83 Cycle | Peck Drilling”|
G82 Cycle Format
|G82 X… Y… Z… R… P… K… F…|
|G82 : Drilling cycle – With dwell at the bottom of hole|
|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|
|K : Number of cycle repetitions|
|F : Feedrate|
|P : Dwell time at the bottom of hole (Unit in seconds or milliseconds according to the parametric setting)|
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 G82 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 G82 cycle is usually used with the G98 command. You can find details about the G98 and G99 command on our website.
- The G82 cycle is used to dwell the cutting tool at the bottom of the hole for the desired time to obtain a smooth surface at the bottom of the hole.
- After using the G82 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 G82 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 G82 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 G82 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 G82 command is written.
G82 Cycle Examples
G82 CNC Program Example – 1
G90 G54 G0 X0 Y0;
G43 H2 Z50 M08;
G98 G82 X30 Y18 Z-15 R5 P2000 F160;
G91 X40 Y16;
G90 G00 Z100 ;