CNC Milling | G86 Cycle | Boring

G86 Cycle Introduction

G86 cycle is used in CNC Machining Centers (CNC Milling machines) to expand the previously drilled holes with the special boring tool and ensure the hole is upright. During the operation with the G86 cycle, the spindle stops at the bottom of the hole and the tool stops and goes up. The reason for this is that the boring tools are single-cutting-edge and if it turns out, it will create scratches on the surface of the hole. As you can see from here, boring is used for precise and vertical machining of sensitive holes. As an example of these processes, we can give the example of machining die centering bush holes and punch slots in cutting dies.

Boring Tool

Boring tools are special tools that have a special tip and the diameter to be machined is adjusted with the help of screw on the tool. In other words, how many diameters you want to drill the hole, you set the diameter on the boring tool and run the cycle. This cycle works basically the same as G81 drilling, not pecking. The only difference is that the tool stops at the bottom of the hole and goes up while the tool is standing.

With this cycle, the boring tool goes to the coordinate specified in the program, quickly approaches the height of Z specified by R, boring the workpiece depth given by Z .. with the feedrate indicated by F, spindle stop at the bottom of hole 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.

G86 Cycle Format

G86 X… Y… Z… R… K… F…


G86 : Boring 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
K : Number of cycle repetitions
F : Feedrate

Things to Know

  • X and Y coordinates where the hole will be boring are not usually given in the same line. Instead, the machine is sent to the first hole coordinate in the program, and then boring with the G86 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 G86 cycle is usually used with the G98 command. You can find details about the G98 and G99 command on our website.
  • After using the G86 cycle, the cycle must be canceled with the G80 command. If it is not canceled with G80, your machine will boring holes with the conditions specified in the G86 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 “boring the first hole” when moving between the coordinates to be boring.
  • If the command is used with G99, it will use the R height “when moving between the coordinates to be boring”.
  • If the program is stopped during G86 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 G86 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 G86 command is written.

G86 Cycle Examples

G86 CNC Program Example – 1

G86 Cycle Program Example

G28 G91 Z0;
T4 M06;
M03 S800;
G90 G54 G0 X30 Y25 ;
G43 H4 Z25 M08;
G98 G86 Z-25 R5 F100;
Y65 ;
G28 G91 Z0;