P920 is 920 microns thread depth (according to the help in VR Turning)
TIP - In the editor, highlight the gcode you want to know about, and press CTRL + F1 at the same time and hey presto - you'll get.....
The G76 command contains, within two blocks, all the information required to generate a standard thread form and pitch.
A G76 uses one edge cutting to reduce the load on the tool tip.
Click here to show G76 Canned Cycle General Diagram.
A G76 command is written in the following format:
G76 P (A) / (B) / (C) Q (Min) R ;
G76 X(U) Z(W) P (DEP) Q (1st) F ;
where,
P (A) is the number of thread finishing passes (1 to 99).
P (B) is the chamfer amount. This is the angle at which the tool leaves the billet, at the end of the thread cutting cycle.
P (C) is the angle of the tool tip (8Ø°, 6Ø°, 55°, 3Ø°, 29° and Ø°). Note - (A), (B) and (C) are all specified at the same time by the address P, eg, PØ36Ø6Ø = number of cuts is Ø3, chamfer amount of 6Ø and tool angle of 6Ø°.
Q (Min) is the minimum cutting depth (in microns). When the depth of the cut calculated by the CNC control becomes less than this limit, the cutting depth is clamped at this minimum value.
R is the finishing allowance. This is the final, or finishing, cuts applied to the thread. The number of stages to complete this finishing allowance is determined by the value of P(A), ie, the value of R divided by the P(A) number of finishing passes equals the value of each finishing allowance stage.
X(U) is the end position of the thread in the X axis (the core diameter).
Z(W) is the end position of the thread in the Z axis.
P (DEP) is the depth of the thread as a radius value (in microns).
Q (1st) is the depth of the first pass as a radius value (in microns).
F is the size of the thread pitch.
Click here to show the G76 General Notes Page.
Click here to show a G76 Multiple Thread Cutting Cycle Example.
Click here to show a G76 Internal Thread Cutting Cycle Example.
(for example)
