Programming instructions

NC Programming 17VRS Motion Blocks
4-37
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Input Feedrate as Inverse Time Value 'G93'
The machining time for a programmed workpiece can be defined by the
function G93 input feedrate as inverse time value. The machining time is
determined via the F-word. With the specified machining time, the con-
troller calculates the required path velocity depending on the limit values.
G93 F<time in seconds>
G93 is active on a NC-block-by-block basis and must be programmed in
combination with an F-word.
•
In the programmed NC-block, G93 overlays G94 or G95.
•
The F-value which is programmed with G93 does not affect the F-values
which were programmed with G94 or G95.
•
The F-value programmed together with G93 can be programmed with
five places to the left of the decimal point and two places to the right.
Example NC-program using G93
20
40
60
80
100
20 40 60 80 100
X
Y
[P4]
[P3]
[P2]
[P1]
20
40
60
80
100
X
Z
-10010
[P1]
[P4]
Fig. 4-41: Linear interpolation, G01 with 2 axes and input feedrate as inverse
time value
G00 G90 G54 G06 G08 Motion commands, interpolation
conditions
X0 Y0 Z10 S3000 M03 Starting position, spindle ON
G93 G01 X26.26 Y18 Z5 F0.97 [P1] starting position, input feedrate as
inverse time value
G93 Z-5 F0.3 Infeed Z axis
G93 Y80 F1.86 [P2] linear interpolation, 1 axis
G93 X41 Y93.5 F0.6 [P3] linear interpolation, 2 axes
G93 X111 F2.1 [P4] linear interpolation, 1 axis
G00 Z10 M05 Z axis to safety distance
RET Return to program beginning
Syntax