Programming instructions

ADT-CNC4620 Programming Manual
- 32 -
3.5.1. Axial cutting cycle G90
Format: G90 X/U Z/W R_ F_ ;
X/U: cutting end X axis coordinates;
Z/W: cutting end Z axis coordinates;
F: cutting speed
R: cone slope; radial coordinate difference (radius) between cutting start and cutting
end; if R and U do not have same sign, |R| ≤ |U/2| (diameter programming) or |R| ≤
|U/2|(radius programming) is required. If R isn’t specified, the cylinder processing
is shown in the figure below:
Cutting Fast feeding
Z axis X axis Start point
Execution process:
1) X axis locates (G0) to cutting start quickly from cycle start;
2) Interpolate (G1) to cutting end from cutting start in linear;
3) X axis radially back to radial coordinate position of cycle start in line interpolation
(G1) mode;
4) Z axis quickly locates (G0) and returns to the start point, and cycle ends.
Note:
1) G90 is modal instruction.
2) In single block operation, the system stops at the end position of every block, and pause
and resetting operation are valid in the motion process.