Programming instructions

4-46
Motion Blocks NC Programming 17VRS
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
•
In the power-on state, G96 always applies to the first spindle (S/S1). If
G96 is to be applied to a different spindle, the desired spindle must be
selected prior to the G96 NC-block by using the SPF <spindle number>
command.
•
Depending on the settings in the process parameter Bxx.041 (Spindle
Speed Programming Default), G96 may be the power-on default. G96
constant surface speed (CSS) remains modally active until it is can-
celed by G97.
•
After the controller is turned on, after an NC-program is loaded, after a
BST, M02, M30, RET or control reset, G96 is set automatically de-
pending on the setting in the process parameter Bxx.041, and the
spindle speed values (S values) are reset.
•
If the S value is changed when G96 is active, this S value change
must be programmed together with G96.
•
When G96 is active, the maximum spindle speed can be limited by the
command G92 S <spindle speed>.
•
The spindle override is limited to 100% when G96 is active. Reducing
the spindle override to less than 100% results in a reduction of the
surface speed.
•
If G96 is canceled by G97, the most recently active spindle speed is
taken over as the new spindle speed command value.
Example NC program - face turning with G96
20
40
60
80
100
20 40 60 80 100 120 140
Z
X
[P1]
[P4]
[P2][P5]
[P3][P6]
Fig. 4-46: Face turning
G00 G54 G90 G06 G08 X72.5 Z100 [P1]
Starting conditions
S1 2500 M103
Spindle ON
G00 Z78 [P2]
Infeed for first cut
G96 X27.5 S1 400 [P3]
1st face turning operation
G00 Z100 [P4]
Withdraw Z axis
X72.5 [P1]
Starting point
G00 Z76.5 [P5]
Infeed for second cut
G96 X27.5 S1 400 [P6]
2nd face turning operation
G00 Z100 [P4]
Withdraw Z axis
M105
Spindle OFF
RET Return to program beginning
NC-program