Constant cutting speed (G96/G97/G196)
Syntax: | ||
G96 | Selecting constant cutting speed | modal |
G97 | Deselecting constant cutting speed, selecting spindle speed | modal, initial state |
G196 | Maximum spindle speed for G96 | G196 non modal |
|
| max. speed modal |
Using the G functions G96, G97 and G196, it is possible to optionally change the interpretation of the S word:
G96 | S in [m/min or ft/min *] (cutting speed) |
G97 | S in [rpm] (spindle speed ) |
G196 | S in [rpm] (max. spindle speed during G96) |
* [as of Build V2.11.2032.08 with G70 and P-CHAN-00360 = 1]
When selected with G96, the starting rpm of the spindle is calculated from the programmed cutting speed and the distance of the tool tip to the turning centre point. This distance results from the last (not in the current NC block) programmed position and the reference point offset of the face turning axis. Exactly one face turning axis must be present in the current machining plane (G17, G18, G19).
A cutting speed programmed for G96 using the S word is only valid until it is deselected by G97. With G96, constant cutting speed is only activated when the S word is programmed.
Specifying a maximum spindle speed with G196 in conjunction with the S word is optional and only active during G96. Spindle speed limiting must be programmed before G96 is selected.
 | Extended G function G196 As of Build V3.1.3057.04 |
Alternatively, the maximum spindle speed can be programmed as an additional value in [rpm] in conjunction with G196. It is modal.
This syntax permits the programming of G196 and G96 in the same NC block. A separate specific NC block is not required.
Syntax: | |
G196 = <Max_spindle_speed>
| G196 non modal, max. speed modal |
Close to the turning centre point, the programmed maximum spindle speed (G196) or the maximum spindle speed specified in the assigned axis parameters P-AXIS-00212 defines the limits of the constant cutting speed.
When deselected with G97, the last spindle speed set is retained.
Motion blocks of the face turning axis in rapid traverse (G00) lead to an interruption of G96 to prevent undesired speed value changes when the tool is positioned. The next motion block with G01, G02 or G03 cancels suppression of G96.
Programming Example
Constant cutting speed (G96/G97/G196)