G00 Code | Rapid Movement

In this article, we describe how to use G00 code for rapid positioning and movement in CNC machines with all details and examples.

0
1210

G00 CNC Code

G00 code is a CNC G code and used in CNC Machines to perform rapid motion. Rapid movement is done in a linear plane with the G00 CNC code. G00 G code is used both in CNC Turning and Milling machines for the same purpose and format.

While a workpiece is machining in CNC machines, there is no always cutting on workpiece. For example, using cutting motion in operations such as moving the machine to the reference, moving the tool to the position where cutting will start, moving the tool to the tool change point causes serious time losses. G00 CNC code is used to move axes as fast as possible for that kind of operations and is one of the most common used CNC G codes.

As you can see in the examples given above, the axes must move fast to shorten the machining times when cutting is not performed. The maximum speed of axes depends on many factors such as the machine manufacturer, the ball screw pitch, the speed of the servo motors used, the parameters and the mechanical construction of the machine.

If G00 CNC code is used anywhere in the program, the machine will move to all coordinates specified in the program by making a linear movement with rapid traverse until one of cutting codes are activated such as G01, G02 or G03.

Absolute and Incremental System

In CNC lathe machines; if U and W are used as axis names G00 G code will perform an incremental movement. If axis names are used as X and Z, the system will move absolute.

In CNC Machining Centers G91 code is used to specify incremental system/motion. Absolute system/motion is activated with the G90 code. In other words, these modes are selected with the help of separate G codes, not by changing the axis names like in CNC lathe.

The table below shows how to switch between absolute and incremental systems on CNC machines.

CNC LatheCNC Milling
CommandG00, G01, G02 etc.G00, G01, G02 etc.
Absolute systemX, Z, C etc.G90
Incremental systemU, W etc.G91
Absolute system exampleG00 X10. Z10. ;G90 G00 X10. Z10. ;
Incremental system exampleG00 U10. W10. ;G91 G00 X10. Z10. ;

When the absolute system is selected, the exact position (coordinate) the tool will go to on the machine is specified. While in the incremental system, how far the tool will travel from its current location is specified.

G00 Code Format

G00 X_(U) Z_(W) (and/or others) ;

Note: X, Z and others refer to the axis to be moved. U (for X axis) and W (for Z axis) are used only in CNC Lathes and refer to the incremental system.

G00 CNC Code Examples

G00 Code Example – 1

G00 code example for CNC Programming
G00 code example for CNC Programming

In the example above, we need to move the CNC cutting tool from its current location (1) to the place where it will start cutting (2). If we assume that the position (2) is 30 on the X axis and 10 on the Z axis on the workpiece and we use the absolute system to move axes;

G00 X30. Z10. ;

G00 Code Example – 2

N21 G00 X24.5 F300 ;
N22 Y12.0 ;
N23 G01 X30.0 ;

In block N21, only the rapid motion will be executed. Feedrate of 300 mm/min will be ignored in this block, but stored for later use. Motion in the block N22 will also be in rapid positioning mode, since G00 G code is a modal command. The last block, N23, is a linear motion (cutting motion), that requires a feedrate. As there is no feedrate assigned to the motion in this block, the last programmed feedrate will be used. That was specified in block N21 and it will become the current feedrate in block N23, as F300 mm/min.

Things To Know

  • In the G00 cnc code, since the axes move at a rapid traverse rate set for the individual axes independently, the tool paths are not always a straight line. Therefore, positioning must be programmed carefully so that a cutting tool will not interfere with a workpiece or fixture during positioning.
  • The block where a T command is specified must contain the G00 command. Designation of the G00 G code¬† is necessary to determine the speed for offset movement which is called by the T command.

Need to More?

Our volunteers have worked together and carefully prepared the articles published here in their native language without using machine translation. You can search the entire site for more information on the subject. You can start a discussion on CNCarea.com forums and join us to get support, ask questions, improve a published article or give your opinion.


Previous articleCNC | Tool Length Offset
Next articleCNC | M Codes | Miscellaneous Functions