0 votes
108 views
in cnc programming by (9.4k points)

In this article, we describe how to use G84 tapping cycle in CNC milling (CNC Machining Centre) machines with all details and examples.

G84 Cycle Introduction

In CNC Machining Centers (CNC Milling machines) G84 command (G84 cycle) is used for tapping (threading in the hole) operations. 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 G84 command (G84 cycle) to prevent jamming of the chip and discharge the chip out of the piece during the relevant 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.

G84 Cycle Format

G84 X… Y… Z… R… Q… F…

Parameters

G84: Stepped or direct tapping (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 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 G84 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 G84 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 G84 cycle. If it is not canceled with G80, your machine will try to tapping each different coordinate in the program with the conditions specified in the G84 line.
  • If the command is used with G98, it will use the Z height that it uses when going “first 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 G84 cycle. In this case, the thread extraction process will be impaired since the pitches will not be same with the starting position.
  • The G84 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 G84 command is written.
  • While the G84 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.

G84 Cycle Examples

G84 CNC Program Example – 1

G84 Cycle CNC Program Example

O1234;
N10 T2 M06;
N20 G90 G54 G00 X30 Y25;
N30 S300 M03;
N40 G43 H02 Z10 M08;
N50 G84 Z-20 R5 F1.25;
N60 X80 Y50;
N70 G80 G00 Z50 M09;
N80 M30;

G84 CNC Program Example – 2

CNC Milling – G84 Rigid Tapping Program Example

N395 O0084;
N400 G54 G90;
N460 T02 M6; ( Guide Drill )
N465 G94 F400 S2000 M03;
N475 G43 G00 Z10 H2 M08;
N480 G99 G90 G81 X30. Y50. Z–5.;
R3. K1 F500; noktası X30, Y50,;
N485 X60 Y30;
N490 X90 Y50;
N495 X60 Y70;
N500 G80;
N510 G00 Z200;
N520 M05 M09;
N525 T03 M6; ( ø8,5 Drill )
N465 G94 F600 S2000 M03;
N475 G43 G00 Z10 H3 M08;
N480 G99 G90 G81 X30. Y50. Z–35. R3. K1 F500;
N485 X60 Y30;
N490 X90 Y50;
N495 X60 Y70;
N500 G80;
N510 G00 Z200;
N520 M05 M09;
N525 T04 M6; ( M10 Tapping Tool )
N465 M03;
N475 G43 G00 Z10 H4 M08;
N480 G99 G90 G84 X30. Y50. Z–35. R3. K1 F300; ( S200 x Pitch(1,5) = 300 )
N485 X60 Y30;
N490 X90 Y50;
N495 X60 Y70;
N500 G80;
N530 G00 Z200;
N535 M05 M09;
N540 M30;


Need to more?

In this article, we described How to use G84 tapping cycle 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.
...