Okuma roughing canned cycle HELP

I’m looking for a canned cycle g code to rough in a groove on a lathe to feed back and forth in z when taking a new rough cut instead of g85 and only feeding from right (tailstock) to left (spindle), I can be more specific if needed, any help is greatly appreciated!
I want it to rough back and forth vs roughing 1 direction as I’m using a button insert with cutter comp set and p8
I program with igf and it doesn’t give me the option to change tool paths when roughing
This is programmed in igf rough mid od if that helps
Thanks again!

If you are looking to do a zigzag grooving cycle you are out of luck in Okuma IGF. It only has plunge grooving cycles using G73/G74.

You may be able to do a finish mid OD cycle with a zigzag path to accomplish what you want but do not try with cutter comp or it will freak out and give you unexpected moves as it tries to calculate the path reversal.

hy jl :) roughing cycles are feeding uni-directional, and this is not only for okuma machines

if you wish for a 2nd direction, then you have to replace cycles with g-code

if you still wish to use igf, consider a more stable approach:
... rough it assimetrical, with a 'd' or 'v' insert, then finish it with the button insert, most likely using p3 + editing the toolpath start & end, by adding virtual segments, in order to avoid a little crash during comp-in and comp-out movements :)
... depending on groove shape, it may be required to add an intermediate operation, with the button insert, like a small grooving right in the middle of your groove, in order to reduce tool stress during the finish operation, so to avoid having the button insert arch contact > 180 degrees

if you wish for a real approach sugestion, please share groove drawing and button insert radius :)

---

just a few notes; maybe they don't resonate now with you, but, for now, just know that they are here :
... a button insert can be declared in p3 p4 and p8, and still deliver same operation; futher more, a bit tricky, but it can be declared actully in whatever p you wish, including p0, and still make it deliver the toolpath ( for example, a button insert measured in p8 can deliver a chamfer in p1; more precise, the chamfer is represented by a segment, who's position, on the toolpath, would theoretically require a p1 tool )
... with p3, is possible to cut an imaginary closed shape, like a full circle, or rectangle, etc ( this trick is used to shorten machining comp toolpaths arround sharp vertexes, or to achieve higher accuracy by managing backlash position; 'ding' for more infos; also pls check attached )
... when it comes to p quadrants, those don't represent your real tool, but the imaginary tool nose quadrant; is not a must to have the real tool nose quadrant identical with the imaginary tool nose quadrant, but is a must to have the real and the imaginary co-radial ( something like when eating pizza, each one has it's own slice, but they all were coradial inside the box, when delivered; well, some cook their own pizza, but, hmm )
... in other words : as long as there are no interferences, or, more precise, as long as the interferences are accepted, toolpath design is not restricted by tool-nose-p

all above represents particularities related to compensation; igf can handle some of them / kindly :)

not so smart advice, as deadlykitten provides, but maybe effective in some approach.
1. You don't need to stick to grooving cycle. Look at thread cut cycle.
2. You can split the shape to simple (vulgar) parts.
3. Sometimes is easier to update G-code manually.