1. G Function Description
Description:
1. use G00 to move to specified (X,Y) when performance start
2. use G00 to reach specified R point.
3. use G01 to interpolate a distance Q at the present depth
4. use G00 to return a distance d (CNC parameter 4002)
5. repeat drilling hole until reach the Z point
6. use G00 to return initial point(G98) or programmable R
point(G99)
Notes:
1. d distance is defined in CNC parameter No.4002.
2. before using G73, please use M Code let the drill start to turn.
3. if M Code and G73 are specified in the same block ,this M Code
only executes in the first time of positioning in that block, when K
is used to specify numbers of times, this M Code is executed for
the first only, for the second hole and subsequent holes, the M
Code is not executed.
4. G73 is module G Code , when use G73 once ,it is effectively
always ,we only give the (X,Y) in the next line of program ,then
controller will start to drill of (X,Y).
5. this module G code ,use G80 to cancel ,or G00 ,G01,G02,G03 or
other cycle this G code will be canceled automatically.
Condition:
1. Before drilling axis be changed, Canned Cycle must be canceled
first.
2. If a Block is not included movement command of any axes (X, Y,
Z), then drilling can not be executed.
3. The data that Q and R specified, only be set in the block we
execute drilling, it can not be set in the block we do not execute
drilling.
4. G Code group 01 and G73 can not be specified in the same block,
or G73 Canned Cycle will be cancel.
5. In Canned Cycle, tool length compensation (G41/G42/G40)will be
ignored.
Program example:
85
    "