Automatically restart of program OSP5020

[vesene]

Hello everybody!
Im new at the forum which I find very interesting. Im from Sweden and therefore maybe all is not grammatically correct, hope you can live whit that.

I have a question about my lathe, a LB15II. How can I make the program to restart after end of program? I have made a barpuller and I dont want to press the start button every time. Im sure there is a easy way but I have not found it altough I have read in the manuals . It would be great to set the partcounter and just collect the parts from the chipcontainer. Greateful for help! Thanks.
/ Samuel

[Superman]

Mills have 2 methods of continuous cycling
I am sure that lathes have the same functionality

Before the M2/M30 insert a "GOTO NSTART" and place a "NSTART" on the 1st line of code would make the program continuous, but a parts count method would need to be added before that GOTO code, say "VC1=VC1+1 ". Parts count is normally advanced when a M2/M30 is executed. The 1 can be replaced with any number like if parting off a number of washers. VC1 is a user variable, most Okumas have 1 to 128 available for program use

NSTART G0 G40 G80 G90
...
VC1=VC1+1
GOTO NSTART
M2 or M30

or use a schedule program .SSB
example .SSB program

( SCHEDULE PROGRAM )
N1 PSELECT <yourprogram1.min> Q99
N2 PSELECT <yourprogram2.min> Q15
N3 PSELECT <yourprogram3.min> Q25
N4 GOTO N1  ( this also makes the program continuous )
N5 END

-This would load the program and then cycle it 99 times
then load #2 program and run it 15 times and so on.

PS. Welcome to the forum

[Goldorak]

Superman is right

but on a lathe you only use V1 instead of VC1

[ssmw]

And if you want 250 pieces you could throw in a

"IF [V16 GT V17] GOTO N0002"

sorry this is a cut and paste from one of my programs...
use any 'V' number you want, and an 'NSTART' instead of an "N0002"
set your V'16' to what ever you want for number of parts and let it run!
( with a 12 foot autoload bar feed - 24 hrs a day!)

[broby]

don't forget that line numbers can only be FOUR (4) alphanumerics long after the "N"
So NSTART will NOT work as a valid line number.
I usually use NSTRT instead.

Isn't it nice to see how the Mills and the Lathe programming teams got together and standardized the coding between the controllers... yep... VC's on the Mills and V's on the Lathes... real consistent guys!

[ssmw]

Yah -
Maybe not real consistent... but they are still fairly amazing controls! I've written a lathe program that has very few hard coded X and Z values in it. Used for parting and chamfering steel tubing for sleeves.. Variables for length, OD, Wall thickness, and amount of chamfer. I needed 1000 of 1 length, and 1000 of another, I just changed a variable in the parameters, and never stopped running!

[broby]

Originally Posted by ssmw Yah - Maybe not real consistent... but they are still fairly amazing controls! I've written a lathe program that has very few hard coded X and Z values in it. Used for parting and chamfering steel tubing for sleeves.. Variables for length, OD, Wall thickness, and amount of chamfer. I needed 1000 of 1 length, and 1000 of another, I just changed a variable in the parameters, and never stopped running!

I so totally agree!
I have written many programs for generic parts that just vary only in size, but have the same profile, on both Lathes and Mills.
The Okuma User Task2 is a very powerfull and relativley straight forward programming method, once you get the idea of how things are done
I must admit, I do love the Okuma controls (and their machines do not break down ery often either... not like our Mazaks... Damn Integrex 400 is out for the count for another 4-6weeks, again).

Cheers
Brian.

[niggle]

How we do this on our lathes is to have a N1 at the start of the program and /GOTO N1 before the M2 at the end. And use the work counters to stop it when a counts up. Having a / infront of the GOTO puts it on block delete, so when the operator wants to stop the program to change a tip or whatever he just puts block delete on and it'll run thru to the M2 and stop.

[vesene]

Thanks for the replies!
I have tried the ways you described but I dont get the program to repeat a certain number of times, it just keeps running. What can I have done wrong?
I didnt figure out how to write a schedule program. And another thing that complicates things is thats my control is in Swedish, not always very accurate translated. Will try more after the weekend, tomorrow we will tranform the workshop to a partyplace, not much beats a Swedish pig-party!

[broby]

at the start of the program is... (Ignore the comments if you like)

NSTRT G0 X800 Z800 (GO HOME)
N0100 G50 S2500 (MAX RPM FOR THIS JOB)
N0102 BLAH BLAH BLAH
.
.
.
YOUR PROGRAM HERE
.
.
.

(END OF PROGRAM CODE HERE)
NEND G0 X800 Z800
N0900 V10=V10+1 (INCREMENT BAR PART COUNTER BY 1)
N0902 V12=V12+1 (INCREMENT TOTAL PARTS MADE COUNTER BY 1)
/GOTO N0908 (TURN OFF BLOCK DELETE TO JUMP THE CONTINUOUS SEQUENCE IF YOU WANT, HAVING BLOCK DELETE ON WILL IGNORE THIS LINE)
N0904 IF [V10 LE V11] NSTRT (JUMP TO LINE STARTING WITH "NSTRT" IF YOU HAVE MADE LESS PARTS THAN ALLOWED FOR THE LENGTH OF THE BAR)
N0906 V10=0 (RESET COUNTER FOR NUMBER OF PARTS PER BAR LENGTH)
N0908 M9
N0910 M5
N0912 M2

Hope this helps
Brian.

[OkumaWiz]

It is NOT a good idea to use a GOTO command to repeat the program. The Okuma keys off of the M02 for many many things. For example:

Alarm C will not ever stop the machine.
Load monitor tool wear can't stop the machine.
Cycle time can not be calculated correctly on graphics page.
MacMan can not count parts or calculate cycle times properly.
Parts counters will not count properly.
Barfeeder interface does not work right since it can't use cycle stop and
Cycle stop switch will be innefective.

I STRONGLY suggest using the Schedule Program. It's easier to write, has an automatic counter and fixes all of the above problems.

See Superman's example - it's as easy as 2 lines of code. Just use SP SELECT instead of PROGRAM SELECT when you call up the program to run and it will give you a list of SDF files to choose from instead of MIN files.

This is the way the machine was designed to be used and it works well and it's simple. Think of it as a master schedule program that is able to call main (MIN) programs.

Good luck.

[broby]

Just goes to show... On the Okuma machines that there is many different ways of skinning the proverbial cat!
The use of a schedule program is certainly the BEST way of doing this process, for all the reasons stated by Okumawiz.
Thanks for pointing those out... has been quite some time since I actually ran a machine and had forgotten about those types of reasons.
Cheers
Brian.