G02, G03, G05 -Circular Interpolation - GSK GSK928TEa User Manual

4.3 G02, G03, G05
【Command format】
G02 Z(W)_ X(U)_ I_ K_ F_ ; circle center coordinates programming, CCW arc
G02 Z(W)_ X(U)_ R_ F_
G03 Z(W)_ X(U)_ I_ K_ F_ ; circle center coordinates programming, CW arc
G03 Z(W)_ X(U)_ R_ F_
G05 Z(W)_ X(U)_ I_ K_ F_ ; arbitrary point(I, K) on arc programming
The tool traverses from the current point X(U), Z(W) to the specified arc in G02, G03, G05 at the set
speed, the arc radius is R or the distance vector from the circle center to starting point is I, K(G02, G03),
or arbitrary point I, K(G05) on the arc.
【Field 】
X, Z ：absolute coordinates of end point;
U, W ：relative movement from starting point to end point;
F：cutting feedrate;
R：arc radius;
K：it is Z different value between circle center and starting point of arc in G02/G03;
It is Z coordinate value of arbitrary point and starting point of arc in G05;
I：it is X different value between circle center and starting point of arc in G02/G03;
It is X coordinate value of arbitrary point and starting point of arc in G05.
【Field range】
X, Z, U, W：-9999.999 mm～9999.999mm
I, K： -1000000.000 mm～1000000.000mm in G02/G03; -9999.999 mm～9999.999mm in G05
F：0.001 mm/min～15000mm/min
R：0＜R≤1000000.000mm
【Explanation】
Z/X programming in G02, G03, G05; the traverse speed is set by F and controlled by the
feedrate override.
F value is modal, and can be omitted when it is not changed. At the same time, it is controlled
by the feedrate override.
Actual feedrate=Fx feedrate override
G02, G03, G05 are modal, and can be omitted when there are the same in the next block. G02 can be
written to G2 and they are equivalent; G03 can be written to G3 and they are equivalent; G05 can be
written to G5 and they are equivalent. The fields are explained as follows:
172
GSK928TEa Turning CNC System
—Circular interpolation
; arc radius program, CCW arc
; arc radius program, CW arc
User Manual