Okuma LB3000 Post Inside

[BrandonTBFBF]

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

[KrupalVala]

Hi @BrandonTBFBF ,

Thank you for sharing your feedback and Modified post with us. I really appreciate the time and effort you put into the Post modification.

We will look into it.

Thanks,

[will_1]

Hi @BrandonTBFBF ,

I am actually working on updating our Okuma post processor and have already fixed most of the things you mentioned. Thanks for the feedback.

-Will

[BrandonTBFBF]

Hi @will_1,

Be sure to take a look at the getCommonCycle function in my post. The "I" or "K" value must be a positive number on the canned cycle line.

I used Math.abs() to get there. Not sure if this is the correct method but it got me what I needed.

Thanks,

Brandon

[will_1]

Will do!

Thank you @BrandonTBFBF !

[BrandonTBFBF]

I've made some updates to this. 

There was an erroneous second clearance plane call on with the live tool tapping cycle.

When tapping multiple holes on the same plane with live tools the old version would try to use High Feed between them. This would cause the machine to to sit still since the spindle was not turning. It now uses G0.

If you were milling with the C axis locked and went to drill axial holes with a live tool (XZC Mode) it wouldn't unlock the spindle brake. This is now fixed.

I added two more Actions: useM136 and useSSV. 

   useSSV turns Spindle Speed Variation on with an M695

  useM136 adds an M136 to a drilling or tapping cycle. This retracts the tool to the clearance point rather than the first cycle point.

[BrandonTBFBF]

I found a small issue with the post I shared above. It was missing a G0 after the G137(Polar Interpolation) call.

This version fixes that.

[will_1]

Hi @BrandonTBFBF ,

Thanks for the feedback, we will make sure it gets into the library post processor.

Thanks,

Will

[BrandonTBFBF]

Update.

This version uses the CircularData function from the Okuma milling post. This prevents issues when using I,J,K rather than radius arcs (L).

I also added the following:

The onManualNC/executeManualNC functions posted on this forum by @bob.schultz . I use a lot of subprogram calls so now the Pass Through feature posts the code in between two sections properly.

A user defined property Max Spindle Speed Sub. The sub spindle on my machine has a max speed of 6000 rpm while the main can only do 4200 rpm. This will post the correct G50 based one which spindle you're working on.

A "Remove Long Tool" feature. If I select "Manual Tool Change" for a tool I'm milling with, chances are it's too long to clear the sheet metal or will hit the chuck/part. So this post will write an M0 after sending the turret home to allow you to remove that tool. 

This post is finally to the point where I can just "post and go". 

The only issue that still exists is the occasional "C360." in a canned cycle line rather than "C0." I have yet to figure out a solution for that.

-Brandon 

[scarwars13]

Thank you VERY MUCH Brandon!  This post has saved me and likely countless others alot of unpleasant headaches and mishaps!  Please continue to share your updates as this has allowed our machine to do radial drilling for the first time!  Never had a cnc lathe before so the lathe guys will laugh but its really exciting and opens up alot of potential for our projects.  Once again much appreciated!  F360 community is the best!

[scarwars13]

One thing I wish is that there was some way to control Polar Mode without using a different post.  Not sure if this is possible but our LB3k is a 450 so the sub can interfere with the turret in some circumstances when heli milling using x and y.  I edited a standard LB3K post to force polar mode so that the c,x rotates instead of x,y action but need to use different posts to control that feature.

[BrandonTBFBF]

My post will force PolarMode using Manual NC - Action - usePolarMode.

If you open the post itself you'll see a list of supported Action commands at the top.

[scarwars13]

One other question, when threading using your post get an error unless i check the box use cycle.  This fix does not use thread orientation so re running threading cycles to tune in thread sizing crossthreads every time. Its either one shot or scrap the part.  Any ideas?

[BrandonTBFBF]

I've always used G33 with this lathe so I never got around to coding the canned cycle. 

I'm able to re run threads as long as the spindle speed is the same. The spindle speed override knob not being at 100 can cause issues with cross threading if you're not careful.

EDIT: I looked through the programming manual this morning and I don't see anything about thread orientation for either the G71 threading cycle or G31/G33 threading. All I see is phase offset for multi-start threads. It also looks like the G71 cycle is already set up in the post. 

Do you have an example of what you'd like to use?

[bradfordmachineshop]

Where are you adding the polar interpolation at?

How do I make a toolpath output with G137 polar interpolation?    

Im proving your post out in our new Okuma Genos L3000MY.

Thanks again for all these tips so far!!

[BrandonTBFBF]

add a Manual NC - Action - usePolarMode before the operation you want to use polar interpolation.

[BrandonTBFBF]

Report back with any issues you find.

[scarwars13]

Ok thanks for looking into this for me!

Im also a new to lathing so that may have something to do with it.  I was trying to cut an M12 thread and my spindle speed was at 100 for sure but thats a good thing to watch for in the future.  I will post the error code i get when i cut a thread again without using the canned cycle.

[BrandonTBFBF]

Id you don't want to use a canned cycle select Use Simple Thread from the user properties box when you go to post. That outputs G33s and it works splendidly. 

If you don't have Use Cycle checked it will pull from the Expand Cycle Point function and won't work properly. I might get around to fixing that one day.

[M.M.M.G.]

good night.

I have a okuma L3000e with Y axis, live tooling. i´m using the last post on the web and works almost fine. but i can not work with my angular live tools. 

I put the tools on the correct plane and it work on fusion, but can not generate the code.