Page
Chapter: 6
Section:
PROGRAMMING
25
6.7.3 THE FEEDRATE F IS NOT AFFECTED BY "P18" (G61, G62)
When operating with feedrates slower than 1 mm/min. or 1 inch/min. machine parameter
"P18" must be set to a value other than "0".
The CNC divides the programmed feedrate by the P18 value and applies the result as
axis feedrate.
It is possible to program whether this "P18" is to be considered or ignored by means
of functions G61 and G62.
G61 The value of P18 is ignored. The CNC applies the programmed F value.
G62 The value of P18 is not ignored. The programmed feedrate F value is affected
by this value as described above.
Example: Machine parameter "P18 = 100"
N0
F1
Programmed F 1 mm/min.
N1
G62.1 X20
Movement at 0.01 mm/min.
N2
X-100
Movement at 0.01 mm/min.
N3
G61
F not affected by P18
N4
X0
Movement at 1 mm/min.
N5
G62
F affected by P18
N6
X30
Movement at 0.01 mm/min.
N7
M30
Attention:
G61 and G62 are modal and incompatible with each other.
On power-up, after executing an M30, after an Emergency or a Reset, the
CNC assumes G62.
6.7.4 ACCELERATION RAMP MODIFICATION (G93)
When the axes operate in Closed Loop, machine parameters "P16, P17", "P91" and
"P92" set the acceleration and deceleration times for each axis.
In certain situations it may be interesting to apply other acc./dec. times.
With this function, it is possible to program the desired acc./dec. time.
Its programming format is:
G93 X Y
Parameters X Y indicate in seconds, with millisecond accuracy, the acceleration time
required for setting for each one of the axes. Maximum value 6 seconds.
Example: G93 X1.500 Y0.700 fixes an acceleration and deceleration ramp of 1.5 seconds
for axis X and another one of 700 milliseconds for axis Y.
On power-up, after executing an M30, after an Emergency or a Reset, the CNC assumes
the settings of machine parameters "P16, P17", "P91" and "P92".
SPECIAL FUNCTIONS
