0 votes
115 views
in cnc programming by (9.1k points)

In this article, we describe how to use G81 cycle for drilling in CNC milling (CNC Machining Centre) machines with all details and examples.

G81 Cycle Introduction

In CNC Machining Centers (CNC Milling machines) G81 cycle is used to drill holes that are not deep and can be drilled in one step. 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, 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 G83 cycle should be used when drilling deep holes because the G81 cycle drills the hole to be drilled in one step without any rebound movement.

G81 Cycle Format

G81 X… Y… Z… R… K… F…

Parameters

G81 : Drilling cycle – One step
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

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 G81 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 G81 cycle is usually used with the G98 command. You can find details about the G98 and G99 command on our website.
  • After using the G81 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 G81 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 G81 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 G81 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 G81 command is written.

G81 Cycle Examples

G81 CNC Program Example – 1

G81 Cycle Program Example

O0001;
T2 M6 ;
M03 S1500 ;
G43 H2 Z30 M08 ;
G90 G00 G54 X30 Y15 ;
G98 G81 Z-18 R5 F200 ;
Y40 ;
X80 ;
Y15 ;
G80 ;
G28 G91 G00 Z0 ;
M30 ;


Need to more?

In this article, we described How to use G81 cycle for drilling in CNC milling (CNC Machining Centre) machines with all details and examples. For more details;

For your comments, suggestions and questions, you can write to us from the “Comments Section” below without registration and please consider to share this post!

Your answer

Your name to display (optional):
Privacy: Your email address will only be used for sending these notifications.
Anti-spam verification:
To avoid this verification in future, please log in or register.
...