4.7.1 G98/G99: Can cycle command returns original starting height/reference height R point


Format:

G98: Can cycle instruction to return to the original starting height

G99: Can cycle command returns the reference height R point


Canned cycles refer to instructions that can be executed cyclically, such as drilling, boring, or tapping. The actions of these instructions are similar. The figure 1 below shows that the tool returns to the original starting height after machining in the G98 command; and in the G99 command, when the action is completed, the tool is returned to the preset reference height R point, as shown in Figure 2 below.


G98: Retract to Star Height


G99: Retract to Reference Position (R point)


When using the can cycle instruction group, it is only necessary to give a cycle machining instruction in the first machining hole position. After that, each repetition machining hole position can be repeatedly processed only by giving its plane position value. Executing G80 cancels the can cycle command; if the Group 01 G code (G00/G01/G02/G03/G33) is also canceled, the can cycle command will be canceled.


Reference position in the can cycle program command. In G90 absolute coordinate mode, R_ value represents the value of reference position; in G91 relative incremental coordinate mode, R_ value is always positive, representing the original starting height to the reference position. R distance. The machining depth Z value can be defined by G90/G91 respectively: in G90 absolute coordinate mode, Z_ value represents the depth position value; in G91 relative incremental coordinate mode, Z_ value represents the relative position from the reference position R point to the processing depth bottom line Distance, this can be positive or negative. The definitions of the machining cycle instructions in G90/G91 are shown in Figure 1 and Figure 2 below.


G90: Absolute Position Mode


G91: Incremental Value Mode


In addition, in the G91 relative incremental coordinate mode, K_ value can be set for all cycle machining instructions, indicating that the cycle command will be repeated along the straight line or oblique line K_ times (for example: repeat drilling), such as "G91 Gxx Xdx Ydy" Z_ R_ F_ Kk;" indicates that the Gxx (G73~G89) cycle machining instruction is repeated for k times, and the distance between the adjacent two holes on the X and Y axes is dx and dy, respectively.


K_ value=4 in G91 Incremental Value Mode


Note 1:

If the G90 absolute coordinate mode is used, the K_ value will have no effect. The K_ cycle will only be repeated in the same place (X, Y).

Note 2:

Some cyclic instructions such as G74, G76, G82, G84, G87, G88 and G89 can give P_ value, so that there may be P_ seconds dwell time at the machining depth Z to increase the accuracy of machining depth or The spindle can have a reversed buffer time at the depth Z (as shown below).


Dwell P_ Seconds