G00: Rapid Move
Overview
- The G00 command instructs a rapid move to a designated coordinate position at a specified feed rate, typically used for fast positioning operations.
Command Format
-
Syntax:
G00 X... Y... Z... E... F...
- Target coordinate positions to move to.
- If an axis is not specified, then no motion will occur for it.
-
Feed Rate:
- The speed at which the movement should occur is set by parameter
NC.Rapid.MaxFeedrate
(see
Parameter Table
)
- If the F argument is used to reduce the feedrate, the commanded feedrate will remain in effect until G00 is no longer active
- The feedrate for standard feeds (eg. G01, G02, G03…) will be stored when G00 becomes active and will be restored once G00 is no longer active
- Subsequent G00 calls will use the default rapid speed unless the F argument is used again
-
Move End Point:
- The end point for the linear movement can be specified in either incremental (G91) or absolute (G90) values.
- In absolute programming (G90), the machine moves to a specific point in the coordinate system.
- In incremental programming (G91), the machine moves a specified distance from its current position.
Examples
N10 G01 X0 Y0 F50
N20 G00 X50 Y25 // moves the tool to coordinates X50, Y25 at the default rapid feedrate
N30 G00 X50 Y25 F100 // performs the same move as above, however the `F` argument sets the feedrate to 100
N40 G00 X60 Y60 // moves at the F100 feedrate since G00 is still active. The modal state of G00 is not affected by repeated G00 commands
N50 X70 // moves at the F100 feedrate as a G00 move since G00 is modal
N60 G01 X10 Y10 // uses the F value that was active prior to the G00 call, F50
N70 G00 X20 Y20 // uses the default rapid feedrate even though the earlier G00 call used F100 because G00 was deactivated by the G01 call
Details
- By default, feed rate override does not affect G00 rapid moves.
- Axes not specified by the G00 command do not move.
See Also: