4.9.5 G94/G95: Feed rate control per minute/per revolution
Format:
G94 F_
G95 F_
The G95 command setting F_ is the feed speed per revolution. The tool cuts the surface of the workpiece in accordance with the speed at which the spindle moves F_ each time. The G94 command cancels the feed rate control per revolution (ie, G95 mode) and restores the feed rate per minute with F_.
Feed Rate in Millimeters (Inches) per Revolution
Note: |
In the G94 and G95 instructions, the F_ values are defined differently as follows: |
1. |
If the F_ value in G94 is not given to the decimal point, it will be treated as having a decimal point after the mantissa. If the value given is a decimal, the decimal is still valid; therefore, F300 will be treated as F300.0, while F300.05, F300.6 and other decimals are still valid. |
2. |
If the F_ value in G95 is not given a decimal point, it will be converted to an integer multiple of the minimum unit of the system. If the value given is a decimal, the decimal is still valid; therefore when the minimum unit of the system is 0.001, F300 will be treated as if it is F0.300, and the fractions such as F300.05 and F300.6 are still valid. |
3. |
From the above definition, the range of F_ values can be sorted out: |
G21 (Metric unit input) |
G20 (Inch unit input) |
|
G94 mode feed per minute |
F0.001~F60000 (0.001~60000 mm/min) |
F0.0001~F2362 (0.0001~2362 inch/min) |
Feed per revolution in G95 mode |
F0.001~F999.999 (0.001~999.999 mm/rev) |
F0.0001~F39.3700 (0.0001~39.3700 mm/rev) |