Circular Interpolation

Circular moves are programmed with the codes G02 and G03.

G02 = circular interpolation clockwise.
G03 = circular interpolation anticlockwise.

In the following examples, there are five conditions that must be met before a G02 and a G03 can be programmed.

1st Condition

The tool must be at the precise start position.

2nd Condition

The next block control will control the direction the circular move will take G02/G03

3rd Condition

The block must also have the precise end position of the circular move X,Z

4th Condition

The block must establish the arc centre of the circular move. In an incremental coordinate system the circle centre is taken from the start position. The X centre is designated (I) and the Z axis centre is designated (K). The I and K values must have the precise figures of the circle centre coordinates programmed in this block.

5th Condition

After completing the circular move the G02/G03 must be cancelled if the next movement is linear with a G01 or G00

Programming example with G02/G03 and I/K Incremental Circle Centre

N50 G00 X0 Z5
N60 G01 G42 Z0
N70 G01 X40 (P1)
N80 G03 X50 Z-5 I0 K-5 (P2)
N90 G01 Z-36 (P3)
N100 G02 X58 Z-40 I4 K0 (P4)
N110 G01 X74 (P5)
N120 G03 X80 Z-43 I0 K-3 (P6)
N140 G01 Z-80
N150 G01 G40 X82
N160 G00 X500 Z800
N170 M02