The R value in the first line of the O series format sets the Return amount between pecks and is a modal value. This value can also be set in parameter #722 in the O series and remains until changed by specifying another value with G75 R in the program. Accordingly, if you wanted the two machines to have a similar one line format, and you're happy to have a constant retract amount across all G75 applications used with the O series machine, the value can be set in the parameter and the first G75 line in the cycle omitted. However, the series O and 10 control use a different syntax in the main G75 block. Therfore, the programs aren't transportable between the two controls.
The syntax for the G75 cycle for the 10 series machine is as follows:
G75 X(U).... Z(W).... I.... K.... F.... D.... Where:
X = Finish point in X
Z = Finish point in Z
U = Incremental value of X
W = Incremental value of Z
I = Step across movement in Z direction
K = Depth of cut in the X direction
F = Feed rate
D = Relief amount for the tool at the end of the cut in Z.
In the above format, Z,I and D are used if the cycle is to be used to machine a groove wider than the width of the grooving tool, or for a series of holes where the pitch of the holes will be described by I and the last hole coordinate by Z.
1. When used for any drilling operation, parameter D is omitted.
2. When used to drill a single hole Z,I and D are omitted. When omitted, the D parameter is assumes to have a value of zero, and Z and I are ignored in software.
The Return amount set by R in the first G75 line of the O series control format, is set in parameter #6217 of the 10 series control. Unlike the O series, this is the only way the Return amount can be set on a 10 series machine.