Well Smitty, glad you're getting fixed up with some software.
Yes, as you have found out, there are limitations to the use of canned cycles on lathes.
The G81, G82, G83, G84 are all designed to operate with predetermined motions in the Z direction, since the assumption is made that you will be drilling a hole, with the drill point positioned right at X0 on the lathe's centerline. These cycles cannot be used in the X direction.
However, there is no real magic to these canned cycles, they are simply a shortcut to a common procedure, but you do have to learn about what axis are active for the duration and what they do.
For "peck grooving" which it sounds like what you are doing, a canned cycle would work if you were cutting a groove in the face of a part held in the chuck. But for the direction you are working in which is X, you'll have to write that one out longhand.
Now I don't want to burden you with information overload, but be aware that you can write a small subroutine to accomplish the peck movements in X. It will not be modal, which means you have to call it every time you want to use it. But, once it is written, you can write your main program very quickly, planning your main program moves to each groove location, followed by one run through the subroutine.
By contrast, canned cycles in the G8x series, remain active until cancelled. This is what modality means. This is not all that useful on a lathe, but on a mill, it allows for one rapid move to occur between each execution of a hole drilling cycle.
important Shut off a canned cycle in the G8x series with a G80, which is the shorthand command for cancelling the active cycle. It is a good idea to place certain commands at the beginning of your program, just to make sure that all such things are shut off before the program runs again. Sometimes, you'll abort a program part way through, and if a G8x cycle was still active, it may go yet again after the first positioning move is read even when your program starts over.
For example, the very first lines of your main program should contain things like
G54 (cancel work offsets, applicable to mills)
G40 (cancel tool radius comp)
G80 (cancel any canned cycle)
G90 or G91 (Tell the machine whether the main program is going to be in absolute or incremental coordinate systems.
So if you want to know about writing subroutines, just post a brief answer describing how you would call up one for your controller
BTW, I do not know anything about Turbocnc, so what I have written above is to be understood to be general gcode rules.