Positioning (G00)

Preparation Function

The G00 command moves a tool to the position in the workpiece system specified with an absolute or an incremental command at a rapid traverse rate. In the absolute command, coordinate value of the end point is programmed. In the incremental command the distance the tool moves is programmed.

Rapid Type:
- Interpolated
- Non-Interpolated (Dog-leg)
- XY Interpolated, Z First/Last

Command format:

(G90) G00 X___ Y___ Z___ ; (Absolute programming)

(G91) G00 X___ Y___ Z___ ; (Incremental programming)


Sample program:

Absolute programming:


1) Non-Interpolated (Dog-leg):
G90 G00 X90. Y50. ; (Absolute programming)

2) Interpolated:
G90 G00 X90. Y50. ; (Absolute programming)



Incremental programming:


1) Non-Interpolated (Dog-leg):
G91 G00 X70. Y30. ; (Incremental programming)

2) Interpolated:
G91 G00 X70. Y30. ; (Incremental programming)

Explanations:

Either of the following tool paths can be selected according to bit of parameter (e.g. Fanuc 15i-Model A, Parameter No. 1400 #4 LRP, See page 74).

- Nonlinear interpolation positioning (Dog-leg)
The tool is positioned with the rapid traverse rate for each axis separately. The tool path is normally straight.

- Linear interpolation positioning
The tool path is the same as in linear interpolation (G01). The tool is positioned within the shortest possible time at a speed that is not more than the rapid traverse rate for each axis.

The rapid traverse rate in the G00 command is set for each axis independently by the machine tool builder (e.g. Fanuc 15i-Model A, Parameter No. 1420, See page 82). Accordingly, the rapid traverse rate cannot be specified in the address F.

E.g. FULLTEK CNC Machines CENTEK Series (Syntec Controller) - System Settings
461 : X axis max. rapid travel feedrate (mm/min)
462 : Y axis max. rapid travel feedrate (mm/min)
463 : Z axis max. rapid travel feedrate (mm/min)
464 : 4th axis max. rapid travel feedrate (mm/min)



In the positioning mode actuated by G00, the tool is accelerated to a predetermined speed at the start of a block and is decelerated at the end of a block. Execution proceeds to the next block after confirming the in-position.

"In-position" means that the feed motor is within the specified range. This range is determined by the machine tool builder by setting to parameter (e.g. Fanuc 15i-Model A, Parameter No. 1827, See page 123)

G00, G90 and G91 are modal G codes.
Once they are specified, they remain effective until the next associated G code is specified.

G00 in programming:
G-code Manufacturer Series Modality Group Function
G00 FANUC Series 16/18/160/180 – Model C for Machining Center modal 01 Positioning
G00 FANUC Series 0i Mate-MC modal 01 Positioning
G00 FANUC Series 0i Mate-MB modal 01 Positioning
G00 FANUC Series 0i-MB modal 01 Positioning
G00 FANUC Series 15i-MB, Series 150i-MB modal 01 Positioning