For anyone in need of a half decent post for an Okuma lathe.
I've spent the last year not only teaching myself how to "speak Okuma" but also learning how to modify these post processors as well.
The generic LB3000 post didn't play very well with my machine (LB3000MYW800) so I give to you the fruits of my labor. It's not perfect but it's a huge improvement over the generic.
Modifications I've made:
Use Y Axis Retract Feature: Will cancel the tool offset and send the turret "home" in a safe manner if using Y axis offset style toolholders. It can be turned on or off from the post window in Fusion. It is on by default.
M5 Between M3 and M4: If you're using Y axis offset turning you'll most likely have LH and RH tools stacked. This will stop the spindle between operations if the spindle direction changes.
Peck Tapping: Okuma doesn't have a peck tapping canned cycle so this is kind of a hack but works. It calls multiple G77 cycles to get to the desired depth. The key to this working is the M136 on the G77 line. Peck tapping will also work with Live Tools (G178).
Work Plane Call after Activating Y Mode : Once Y mode is activated (G138) the active work plane is cleared so this makes sure to call the plane after the G138.
IPR Feed for Drilling on Center: I prefer ipr feed for drilling.
Expand Cycle Action: Sometimes I like to customize a drill cycle manually so I added this action. Activated by using expandCycle as the action.
Force Retract Action: Forces the machine to home. I'll use this with Pass Through code when running sub programs. Activated by using forceRetract as the action.
Use 3 Pass Action: I use this to sneak up on tight tolerances. It forces the tool to retract to the home position and writes an M0 with the target dimension as a comment in the program. To use it select Manual NC -> Action -> use3Pass:(dimension) The colon is necessary. Place it AFTER the operation you want to check.
Z Home Position Action: I use this to change the turret Z Home Position in the middle of a program. If I'm working between the Main and Sub spindle on my machine I don't want tool changes happening over top of the Sub Spindle. This way I can set the Home Position wherever I need it.
To use it select Manual NC -> Action -> zHome:(homeposition) The colon is necessary here too. Place it BEFORE the operation you want to modify the Home Position of.
Multi-Start Threading: You can now choose a standard G71 threading cycle or simple threading cycles(G33) for Multi-start threads.
Multi-Axis Feedrates: The correct logic is now in place for feedrates when multi-axis milling.
There was an issue when selecting "Alternate Flanking" style threading while using Simple Threading Cycles(G33). Basically, it wasn't working. That's been corrected.
I pulled the CircularData function from the Okuma milling post and added it to this post. This ensures that the output points lie exactly on the circle. This keeps the machine from alarming out.
There are some other minor tweaks here and there but mostly just clean up of the code.
DISCLAIMER: I am not an expert on Okuma nor Javascript. Just someone that needed something done and had to teach myself some new skills. I've seen others on this forum run into similar issues with these Okuma machines as I have so I figured I'd share what I've learned.
-Brandon
