CNC G Code: G0 or G00
Rapid move to a point. (Not necessarily in a straight line!)
G0 (G zero) tells the machine to move as quickly as possible to a given point (absolute or relative, depending on the setting of G90 or 91). This command is modal, so any coordinates that follow will be rapid as well (until a Group 01 code is called). As with all G codes, it specifies only the destination point. HINT: It is usually a good idea to pull the Z up to a safe distance before executing a G0, since the path is not a straight line. Also, never rapid to or from a position too close to the workpiece. Leave some room for lead-ins and lead-outs. Be aware of the decimal point!
Takes the arguments (X, Y, Z, A, B).
Each of these is optional, A and B are for rotary axes. Notice there is no argument for feed rate, it is the machine max.
Assume the machine is currently at X0.0 Y0.0 and G90 is enabled. for the following code:
G0 X3.0 Y1.0 ;
The toolpath will look like this:
Don’t make the mistake of thinking the path looks like the one shown below in red! This is a crash waiting to happen.
The above example assumes milling, for turning, the only difference is the interpretation of the coordinate system.
See also: Haas Manual