Salut,
J'ai fait quelques expérimentations pour voir le Gcode que ça sort, et j'ai reporté les noms des paramètres sur l'écran filetage.
Tu trouveras les explications des paramètres sur la doc tournage de Mach4 page 29
J'en déduis que le Xi doit être le Ø extérieur du filetage.
c'est le X de la ligne G0 = Position Xi + 2* Xc (clearance = dégagement)
Zi c'est le pt de départ en Z, c'est le Z de la ligne G0 = Position Zi + Zc (Zc = dégagement en Z)
A: angle pour un filetage conique.
Pitch (F) pas du filetage
Tip (deg) angle de filet (60° pour du ISO, 55° pour du Wihtworth, 30° pour du trap) (3ieme valeur du paramètre P de la 1ière ligne du G76 = P0202
30)
Thread Depth: profondeur du filet (au rayon) ; à la louche il me semble qu'en ISO 60°, c'est 0.62 fois le pas (au rayon)
Retract (rev): Rétraction entre passes
Min depth: prof de passe mini
Start depth: prof de passe de la 1ière passe.
K: mode de filetage (volume constant, passe constante, flanc alterné ou non) ...
Sur la doc
G76 – Multiple Thread Cutting Cycle:
The multiple thread cutting cycle simplifies the cutting of threads.
This cycle is specified in two blocks and will rough and finish threads with or without lead outs and with different infeed options. By comparison, using G32 would require at least 3 blocks of code per pass.
Format: G76 P_ _ _ _ _ _ Q__ R__ K__
G76 X__ Z__ R__ P__ Q__ F__
First line:
P: 6 digit number specifying the number of finish passes, length of lead out, and the angle of the threading tool. Each parameter is two digits. The number of finish passes can be specified from 01 to 99. The lead out is specified in the number of leads from 0.0 to 9.9 (00 to 99). Then the tool angle. For example: P053060 = 05 finish passes, 3.0 leads to lead out, and a 60 degree tool.
Q: Specifies the minimum cutting depth. If the calculated depth of cut becomes less than this value, then the specified minimum is used.
R: Finish allowance.
K: Infeed type. There are 4 possible infeed selections, 0 to 3. The 4 options are combinations of two infeed types and two depth of cut types. The two infeed types are flank and alternate flank, see figure 76-1. In the flank infeed mode each depth of cut moves down at the angle for the thread, following the trailing flank of the tool. Alternate flank changes from leading to trailing flank for each pass. The two depth of cut types are constant volume and constant depth. In constant volume the depth of cut will get smaller (down to the minimum specified by Q) for each pass to maintain a constant volume of material being removed. This is usually better for tool life and thread quality. Constant depth is just that. Each depth of cut is the same down to the finish allowance.
o 0 constant volume flank infeed
o 1 constant volume alternate flank infeed
o 2 constant depth flank infeed
o 3 constant depth alternate flank infeed.
Second line:
X, Z: Coordinates of the end point of the thread. Can also be specified as U and W for incremental distance and direction from the current position.
R: Taper amount in the X axis, specified in radius. If omitted or 0 is specified a straigt thread will be cut.
P: Height of the thread in radius.
Q: 1st depth of cut in radius.
F: Lead of thread.
++
David