[hoganj]

Hi all,
I am a high school machine shop instructor and we recently acquired a 1993 LNC 8 turning center with OSP 5020L. Slowly figuring things out but have some questions.

1. It has an rs-232 port but would like to know for sure if it is capable of sending and recieving cnc programs through it?
2. Is there a way to enter in my own programming with out using the IGF function? I have tried editing the IGF program but when the cycle reaches my custom programming it just stops at that line of code but it is not giving me any kind of error message.

3. When I am using the IGF feature I keep getting a message that my bubble memory is near full, what can I do about that?

4. I am wanting to make 1.2 thick by 2.5 OD aluminum blanks. I have a royal product combo cutoff and bar puller but I am struggling to get that to work. So far I am able to face off, cut the OD, and part off but beyond that I am stuck to get the automation going. Any suggestions here?


5.Anyone near central Colorado experienced with this vintage willing to come train for compensation?

Thanks
Jake

[zooloader]

A search through the okuma forum will give you the info for setting up the RS-232 ie. Comm software and wiring your cable to the plugs.
Post your hybrid programming so we can see what's going on. Plenty of eyes here to help.

[Algirdas]

I am a high school machine shop instructor

congratulations

rs-232 port but would like to know for sure if it is capable of sending and recieving cnc programs

sure, yes. Be aware - You can't call part program from RS232 for execution if control specification doesn't contains DNC ("drip feed")

Is there a way to enter in my own programming with out using the IGF function?

sure, yes. Edit or RS232 transfer or ...

it just stops at that line of code but it is not giving me any kind of error message

more details, please, if You want this issue with IGF to be solved

my bubble memory is near full, what can I do about that?

delete IGF files - they are hudge. Check, what else is occupying Your user space. Maybe "A.MIN"; "A1.MIN", "B.MIN" and so on? Delete it

face off, cut the OD, and part off

the part is done, cool

I am stuck to get the automation going

You mean the bar feeder? What interface is between OSP and bar feeder? Is bar feeder linked to OSP by key?

[hoganj]

A search through the okuma forum will give you the info for setting up the RS-232 ie. Comm software and wiring your cable to the plugs.
Post your hybrid programming so we can see what's going on. Plenty of eyes here to help.

My hybrid programming for the bar pulling I want to do is:
following the IGF line of code of N306 M05 M09
with the spindle stopped I need T0606 (a bar puller) to cross feed in,
so I have a - G01 X-.825 F10.0
Than I need the chuck to unclamp - M84
Than I need a long feed out to - G01 Z1.250 F10.
Than I need to clamp chuck - M83
Than I need to Cross feed out to G01 X2.8 F10.
and than retract turret and end and reset program.

Thinking there might be some G and M codes that I am not aware of that I need to have in there

[hoganj]

How can I find out if my control contains drip feed?

I did find the IGF parmeter for enabling the bar puller but I haven't figured out where in IGF to program it so I was just triing to enter in my own code for it.

[underthetire]

Your LNC8 will not have drip feed (DNC-B). That was a special order very custom install on a LNC8.
You will need to switch to feed per minute mode to pull stock, otherwise the spindle must be rotating.
Your memory is full, delete unused programs. Very small memory capacity on the 5020L controller.
Send me a PM with your contact info. I have classroom manuals.

[redwolfhollow]

Are you commanding G98 (Feed per Minute) before the pull?
If that works don't forget to G99 afterward or it will appear to "stall" when you call up your next feedrate.

Side note: My Okuma would move in this (G99) situation when the chuck was hand spun!

Oh, I don't miss the bubble. Sometimes getting the program to fit was the only holdup. Here are some helps for that.
Get rid of all your "N" words except any that you link to. Make those numbers single digit.
Change modals from M08,G01 etc to M8,G1 etc.
If you are in G1 don't call it again. Or any other modal.
F70 is the same as F.007 and takes two less digits. F5 is F.0005, saves four.


N306 M05 M09
T0606
G01 X-.825 F10.0
M84
G01 Z1.250 F10.
M83
G01 X2.8 F10.

Becomes:

N3 M5 M9
T606
G1 X-.825 F10.
M84
Z1.25
M83
X2.8

Barry

[Algirdas]

No reason to use IGF at all for that kind of part program. It's easier to make such a part program directly in MG codes. Is Your IGF "one touch" IGF? It isn't right? So, You need to correct IGF made part programs manually. I would use "NC input" for bar puller if IGF is absolutely necessary (for training purpose, for instance)