What is G02 g code?

G02 instructs the CNC machine to move along a Circular Arc from its current position to a new coordinate. The movement is performed with a controlled federate. The new coordinate can be absolute or relative, depending on the effective mode (G90 or G91). This type of movement is called Circular interpolation.


What is the difference between G CODE G02 and G03?

With both commands, the machine will move from its current position to the same target coordinate. In G02, the movement will be in a clockwise (CW) direction. in G03 the movement will ve in counter-clockwise (CCW).

Syntax:

Version 1 – “R” Syntax:

G02/G03 X12.5 Y14.7 R2.0 F0.2;
  • X, Y – The target coordinates at the end of the movement.
  • R – The arc’s radius.
  • F – The feedrate (Speed) at which the machine will move from the current position to the target position.

What is Ijk in CNC programming?

G02/G03 X12.5 Y14.7 I1.0 J2.0 F0.2;
  • X, Y – The target coordinates at the end of the movement.
  • I, J – The arc’s center point relative to X, Y.
  • F – The feedrate (Speed) at which the machine will move from the current position to the target position.
  • The radius will be calculated.


What does G02 Gcode do?

The machine will move from its current position to the target position at a controlled federate. The endpoint position is calculated depending on the “mode” of the program. Absolute or Relative coordinate mode (GCODE G90 or G91) – The default depends on your controller. The actual path will be determined by the direction (G02 or G03) and the syntax format (IJK or R).

The movement is always done on a plane!

In a lathe machine, it will typically be the XZ plane (I,K with the IJK syntax). On a milling machine, it can be XY, YZ, or XZ depending on the selected working plane (G17, G18, or G19).
G17 (XY Plane) – Use X, Y, I, and J.
G18 (XZ Plane) – Use X, Z, I, and K.
G19 (YZ Plane) – Use Y, Z, J, and K.
For more information on working plane selection and G17 / G18 / G19, read here.

Use Examples of G02

Gcode G02 and G03 Explnation

Example #1CW movement along the Blue Arc in Absolute Mode – “R” Syntax.

N10 G90 (Setting Absolute mode);
N20 G01 X4.0 Y0.0 F0.1 ;
N30 Y2.0 (Position the machine at [P2]);
N40 G02 X10.5 Y9.5 R5.0 F0.5; (CW cirullar move to [P3] at a federate of 0.5);

Example #2CCW movement along the Orange Arc in Absolute Mode – “IJK” Syntax.

N10 G90 (Setting Absolute mode);
N20 G01 X4.0 Y0.0 F0.1 ;
N30 Y2.0 (Position the machine at [P2]);
N40 G03 X10.5 I3.0 J4.0 F0.5; (CCW cirullar move to [P3] at a federate of 0.5);

Example #3CW movement along the Blue Arc in Incremental Mode – “R” Syntax.

N10 G91 (Setting Incremental mode);
N20 G01 X4.0 F0.1 ;
N30 Y2.0 (Position the machine at [P2]);
N40 G02 X6.5 Y7.5 R5.0 F0.5; (CW cirullar move to [P3] at a federate of 0.5);

Example #4 – Full 360° circle. A full circle can be programmed only in “IJK” Syntax!

N10 G90 (Setting Absolute mode);
N20 G01 X4.0 Y0.0 F0.1 ;
N30 Y2.0 (Position the machine at [P2]);
N40 G02 I3.0 J4.0 F0.5(CW Full Circle starts and end on [P2]);
Scroll to Top