Check your parameter manual for 5101 bit #2

[admin]

I just noticed that you said you had a 0i Mate (different animal from the 0T). Check your parameter manual for 5101 bit #2 (the third bit from the right). The function is the same as for the 0T. A setting of "1" should make your Z axis retract all the way.

[admin]

G74 is a Face Grooving, or Peck Drilling cycle, depending on the omission or value of certain arguments. The 0 Series control uses what is now referred to an Standard Series 16 format, wherein the cycle is a two block arrangement. On later controls, Series 15 format can be selected via parameters.

Following is the complete format including the arguments required for machining a Face Groove

G74 R...
G74 X(U)... Z(W)... P... Q... R... F...

Where:
R in the first G74 block = Return amount
This designation is modal and is not changed until another value is designated. This first block can be omitted and the value specified by the parameter #5139. This parameter is changed by the program command.
X = Finish absolute component of face groove
U = Incremental amount in X from Start to Finish diameters of face groove
Z = Absolute depth component of face groove, or drilled hole
W = Increment amount from Start to Finish in Z
P = Movement amount in X direction (without sign), for face groove
Q = Peck depth of cut in Z direction (without sign), for face groove, or drilled hole
R in second G74 block = Relief amount of the tool at the cutting bottom. The sign of R is always plus. However, if address X(U) and P are omitted, the relief direction can be specified by the desired sign.
F = Feed rate

Following is an example to Peck Drill a hole 50mm deep, 5mm pecks, feed rate of 0.150mm/rev, and a Relief amount of 0.25mm specified via the program.

G74 R0.250
G74 Z-50.000 Q5.000 F0.150