# GCODE – G00 – Rapid traverse

## What is G00?

The G00 command instructs the machine to move at its maximum possible speed in a straight line from its current position to a new coordinate. The new coordinate can be absolute or relative, depending on the effective mode (G90 or G91).

## Syntax:

``G00 X8.3 Y9.7 Z12.0;``
• X, Y, Z – The target coordinate at the end of the movement.

## What it does:

The machine will move from its current position to the target position at the maximum possible speed. The speed is usually pre-defined by the machine builder and cannot be changed. The command is typically used for:

• Positioning the cutting tool before the cut.
• Changing a tool from the magazine/turret.

Because of the fast movement, special care must be taken to ensure that the way between the start and end positions is free from any disturbances! A disturbance could be the clamping device or the blank being machined.

## Examples:

### Example #1 – Move Directly from P1 to P2 along the Blue Line.

``````N10 G90 (Setting Absolute mode);
N20 G00 X1.0 Y1.0 (Position the machine at [P1]);
N30 G00 X9.0 Y7.0 F0.5; (Move Directly to position [P2] in Rapid Traverese);
``````

This will result in a crash between the cutting tool and the clamping fixture!

### Example #2 – Move Indirectly from P1 to P2 along the Red Lines.

``````N10 G90 (Setting Absolute mode);
N20 G00 X1.0 Y1.0 (Position the machine at P1);
N30 G00 X9.0; (Move to Coordinate [9,1] in Rapid Traverse);
N40 Y7.0 (Continue moving rapidly from [9,1] to [P2])
``````

The cutting tool will arrive at the desired destination safely!

Important! We can keep adding as many coordinate points as we want. The machine will continue to move to the next coordinate until the next Modal Command is encountered.

``````N10 G00 X9.0 Y7.0 F0.5;
N20 Y12.0 (Move to the next point in Y direction (X & Z stay the same);
N30 X5.0, Y3.0 (Move to the next point in both X and Y, Z stays the same);
N40 Z100.0; (Move to the next point in Z direction, X & Y stay the same);
``````

Remark: The command can be executed also in G91 incremental mode.

Scroll to Top