The G76 cycle is a threading cycle that allows the program to go through any single thread in either a single or a double block of program code. myCNC uses the 10/11/15T and the 0T/16T/18T style parameters.
G76 X.. Z.. I.. K.. D.. F.. A.. P..
G-code example of a single line thread cycle:
G76 X2.89 Z-1.6 I0 K0.051 D0140 A60 P4 F0.0833
The two-line thread cycle consists of a command in the following style:
G76 P(11)(22)(33), Q, R G76 X, Z, R, P, Q, F
NOTE: The R/P/Q addresses of the first and the second line are not the same and have their own meaning within each block only.
Due to different CAM software packages using different units (for example, mm in Fusion 360 versus 1/1000th of a mm in SolidCAM), a toggle in Settings > Config > G-codes settings > G76 Fusion Syntax is necessary:
The above toggle allows the user to switch between the two units systems.
G-code examples of a double line G76 cutting command:
G76 P009900 Q40 R100 G76 X16.18 Z-6.3 P560 Q40 F1
N27 G76 P001000 Q0.147 R0 N28 G76 X11.39 Z-10. P0.88 Q0.147 F1.337
The P- and A-parameters allow to control for the thread cutting type and thread insert angle respectively. The A parameter table is available below:
|A29||ACME thread type|
|A30||Metric trapezoidal thread type|
|A55||Whitworth 55 degree thread type|
|A60||Standard 60 degree V thread type|
|A80||German PG thread type|
The radial infeed is programmed with the A0 parameter, while non-zero A parameter represents compound infeed. Additionally, the P parameter can also be selected for a one-edge or a two-edge cutting mode which either has a constant amount or a constant depth for the infeed:
If the P-parameter is omitted in the G76 command, then the P1 mode is used by default.