Programming instructions

4-20
Motion Blocks NC Programming 17VRS
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
Example of Programming Using Absolute Dimension Input (G90)
G00 G90 G54 G06 G08 Motion commands, interpolation conditions
M03 S2000 Spindle ON
X34.5 Z136.5 [P1] Starting position
G01 X40 Z128.5 F500 [P2] linear interpolation
Z100 [P3] circle starting point
G02 X80 Z60 I80 K100 [P4] quarter circle in clockwise direction
G01 Z10 [P5] machining end point
G00 X100 X axis to safety distance
M05 Spindle OFF
RET Return to program beginning
Example of Programming Using Incremental Dimension Input (G91)
G00 G90 G54 G06 G08 Motion commands, interpolation conditions
M03 S2000 Spindle ON
X34.5 Z136.5 [P1] Starting position
G01 G91 X5.5 Z-8 F500 [P2] linear interpolation
Z-28.5 [P3] circle starting point
G02 X40 Z-40 I40 K0 [P4] quarter circle in clockwise direction
G01 Z-50 [P5] machining end point
G90 G00 X100 X axis to safety distance
M05 Spindle OFF
RET Return to program beginning
Circle Radius Programming
In order to allow dimensions to be taken directly off workpiece drawings,
an option is provided for circular paths to be declared directly in the NC-
program by stating the radius.
A distinct circular path is only produced within a semicircle (180°) when
G02 or G03 programming is used (
see Fig. 4-27).
For this reason, it is
important to indicate whether the traversing angle will be greater or less
than 180°. For arcs whose angle exceeds 180°, the radius must be en-
tered preceded by a minus sign.
G02
R+ ... with a traverse angle to 180°
G03
R- ... with a traverse angle > 180°
Example Defining the arc
20
40
60
80
100
20 40 60 80 100 120 140
Z
Ø X
[E]
R= +30
R= -30
[S]
Fig. 4-27: Circle radius programming, determining the sign to be used for the
radius
G01 X... Z...
G02 X... Z... R±30
Syntax for circle radius
programming in the G17 plane
X ... Y ...