Programming manual
CNC 8055
CNC 8055i
ISO CODE PROGRAMMING
5.
·M· & ·EN· MODELS
SOFT: V02.2X
·75·
Spindle selection (G28, G29)
5.4 Spindle selection (G28, G29)
This CNC can govern two spindles: the main one and the second one. They both can be operative
simultaneously, but only one can be controlled at a time.
This selection is made using functions G28 and G29.
G28: Second spindle selection.
G29: Main spindle selection.
Once the desired spindle has been selected, it can be acted upon from the keyboard or by means
of the following functions:
M3, M4, M5, M19
S****
G33, G34, G94, G95, G96, G97
Both spindles can work in open and closed loop.
Functions G28 and G29 are modal and incompatible with each other.
Function G28 and G29 must be programmed alone in the block.
No more information can be programmed in that block. On power-up, after executing an M02, M30
or after an EMERGENCY or RESET, the CNC assumes function G29 (selects the main spindle).
Operating example for when 2 spindles are used.
On power-up, the CNC assumes function G29 selecting the main spindle.
All the keyboard actions and by spindle related functions affect the main spindle.
Example: S1000 M3
Main spindle clockwise at 1000 rpm.
To select the second spindle, execute function G28.
From then on, All the keyboard actions and spindle related functions affect the second spindle.
The main spindle remains in its previous status.
Example: S1500 M4
Second spindle turns counterclockwise at 1500 rpm.
The main spindle keeps turning at 1000 rpm.
To select the main spindle again, execute function G29.
From then on, all the keyboard actions and spindle related functions affect the main spindle.
The second spindle stays in its previous status.
Example: S2000
The main spindle keeps turning clockwise but at 2000 rpm.
The second spindle keeps turning at 1500 rpm.
To Next Page
Loading...
