G76 Многозаходный цикл нарезания резьбы
G76 P- Z- I- J- R- K- Q- H- E- L-
Это ошибка, если:
- Активная рабочая плоскость не ZX (не G18).
- Указаны другие координаты X- или Y-.
- Значение R- меньше чем 1.0.
- Не указаны все необходимые параметры.
- P-, J-, K- или H- отрицательные.
- E- больше чем половина длинны привода.
Изображение: G76 Нарезание резьбы
Линия прохода Линия проходящая через начальное положение по X параллельно оси Z.
P- Шаг резьбы в расстоянии за 1 оборот.
Z- Положение конца резьбы. В конце цикла инструмент останется в положении Z-.
I- "Вершина резьбы" отступ от линии прохода. Отрицательное значение I используется для внешних резьб, а положительное для внутренних резьб. Обычно материал стачивает до этого размера перед циклом G76.
J- Положительное значение обозначающее "глубину начального прохода". Первый проход будет на расстояние J- за вершиной резьбы.
K-
Положительное число задающее "полную глубину резьбы". Конечный проход будет за вершиной резьбы на величину К-.
Опциональные параметры:
[... Будет допереведено ...]
R-
The "depth degression". R1.0 selects constant depth on successive threading passes. R2.0 selects constant area. Values between 1.0 and 2.0 select decreasing depth but increasing area. Values above 2.0 select decreasing area. Beware that unnecessarily high degression values will cause a large number of passes to be used. (degression = a descent by stages or steps.)
Q-
The "compound slide angle" is the angle (in degrees) describing to what extent successive passes should be offset along the drive line. This is used to cause one side of the tool to remove more material than the other. A positive Q value causes the leading edge of the tool to cut more heavily. Typical values are 29, 29.5 or 30.
H-
The number of "spring passes". Spring passes are additional passes at full thread depth. If no additional passes are desired, program H0.
Tapered entry and exit moves can be programmed using E- and L-.
E-
Specifies the distance along the drive line used for the taper. The angle of the taper will be so the last pass tapers to the thread crest over the distance specified with E. E0.2 will give a taper for the first/last 0.2 length units along the thread. For a 45 degree taper program E the same as K
L-
Specifies which ends of the thread get the taper. Program L0 for no taper (the default), L1 for entry taper, L2 for exit taper, or L3 for both entry and exit tapers. Entry tapers will pause at the drive line to synchronize with the index pulse then feed in to the beginning of the taper. No entry taper and the tool will rapid to the cut depth then synchronize and begin the cut.
The tool is moved to the initial X and Z positions prior to issuing the G76. The X position is the "drive line" and the Z position is the start of the threads.
The tool will pause briefly for synchronization before each threading pass, so a relief groove will be required at the entry unless the beginning of the thread is past the end of the material or an entry taper is used.
Unless using an exit taper, the exit move (traverse to original X) is not synchronized to the spindle speed. With a slow spindle, the exit move might take only a small fraction of a revolution. If the spindle speed is increased after several passes are complete, subsequent exit moves will require a larger portion of a revolution, resulting in a very heavy cut during the exit move. This can be avoided by providing a relief groove at the exit, or by not changing the spindle speed while threading.
The final position of the tool will be at the end of the "drive line". A safe Z move will be needed with an internal thread to remove the tool from the hole.
The sample program g76.ngc shows the use of the G76 canned cycle, and can be previewed and executed on any machine using the sim/lathe.ini configuration.
The following example shows the result of running this G-Code:
G0 Z-.5 X .2
G76 P0.05 Z-1 I-.075 J0.008 K0.045 Q29.5 L2 E0.045
The tool is in the final position after the G76 cycle is completed. You can see the entry path on the right from the Q29.5 and the exit path on the left from the L2 E0.045. The white lines are the cutting moves.
Figure: Threading Example
.