[jay_dizzle]

hello, we have an Okuma LU3000EX twin turret slant bed lathe with a OSP300 controller, im wondering if it is possible to "sequince restart" to the middle of a program during dual turret machining?

its a real pain in the butt to air cut an entire program just to re-cut the area where an insert failed, or a size was missed. please, any insight is welcome.

[OkumaWiz]

Yes it’s possible. It can be done by entering restart block number on each turret, letting it read to restart blocks and then pressing sequence restart.

Turn on single block please and remember it always starts on previous block to make desired block become effective.

P codes must be minded for restart points.

Best regards,

[jay_dizzle]

thanks for the reply OkumaWiz, i have finally gotten the machine to restart in the middle of a program now, just have to 'mind the p values' ha ha, boy these controllers are fussy when it comes to timing.

any tips on NAT## and P# placement within the program?

[OkumaWiz]

NAT01 and NBT01 can be reduced to NT1 since they are sorted by the G13 and G14 commands. If you have common restart points use something like NPASS for example to restart right before transfer, that way, you can copy and paste the restart point into the dialog every time. (ctrl C and ctrl V work just fine) Then it becomes A-turret, Restart, Paste, B-turret, Restart, Paste, Sequence restart, Cycle start.

Use as few P-codes as is possible. People usually get way carried away thinking they need to have them all over. It's possible to only have a couple of P codes in a program. If the turrets are in separate spindle modes (G140/G141) then none are needed until it comes time to transfer. As a general rule, use the A on the left and the B on the right, make a sub for the transfer that has the needed P codes, and just use a couple of variables in the transfer for cutoff diameter, part length, and Z- gripping distance from front of part and programming becomes EXTREMELY simple. Proveouts get very easy as well since you can use individual A to run the A-Side and call your sub to do the transfer, and then use individual B to run the B-Side. The time gained by "crossing over" is usually lost by increased prove out times, so my rule of thumb is if the cycle on each side is within 30 seconds, don't bother crossing over to "assist cut". Every 15 seconds that comes of 1 turret gets added to the other and most cycles will be more than 15 seconds to complete.

One last tip, skip adding in M01's or G140/G141's as the M01's will need P codes and the G140/G141 can act like them and cause timing errors.

By the way these tips are mostly for the Twin spindles/Sub spindle machines so if pinch turning on a 4 axis, some of the same applies, but pinch turning will require every line in a canned cycle to have P-codes in order to remain in perfect sync.

P-code counters can be reset by putting a - in front of the P-code.
Best regards,

[jay_dizzle]

thanks OkumaWiz, we are up and running, much appreciated!

[deadlykitten]

hy jay_dizzle i saw your post yesterday, and i was going to tell you a few things, but only now i have a bit of free time / time is my enemy

on a "dual cnc", at least 2 similar organs exist : at least 2 turrets, or at least 2 spindles ( 2s+t , 2t+s , 2st )

those similar organs :
... may cut free, independtly : single machining state
... may be linked : dual machining state

for example, if you cut a part, on a 2s+t cnc, 1st spindle + transfer + finish it on 2nd spindle, then :
... during transfer, cnc is in "dual machining state" ( both spindles are synced, thus 2 similar organs are linked )
... otherwise, cnc is in "single machining state" ( because similar organs are no longer linked )

program / code is splitted by checkpoints; if the cnc is :
... simple, thus there are no identical organs, then the checkpoints are the common NAT** addresses, that split the code between consecutive sequences ( turret index, etc )
... dual, thus there are identical organs, then the checkpoints should split the code each time a "dual machining state" is changing ( including turned on or off )

from this perspective, a NAT** adreess should be between "single machining states", and a P code should be between "dual machining states"

"dual machining state" = 2 linked "single machining states", so, put a NAT**/NT**/NN** before a P

some programmers are inserting the P codes using excel, so to view the code side-by-side for each organ

some cnc controllers allow this behaviour, thus they can arrange the code side-by-side, accordingly to the existing "dual machining state" codes; this allows the operator to view&edit the code from a different perspective, thus he can oversee the "dual machining state" arhitecture of the program; i don't know if this is possible on osp

---

okay, so far so good, at least 4 me; i hope that this is useful, or at least there is a bit of sense to it

now, about restart sequences on dual organs : it may be tricky, but the checkpoints have to be created in such a way, that both organs are at clearance position when a restart sequence is performed, otherwise, 1st turret may start approaching, and 2nd turret may crash into the part if there is an id tool ( boring knife, drill, etc )

is easy to create a program for a dual cnc without considering the restart checkpoints

i was told that some programmers, after creating the program, are creating a few copies, and each copy has some custom P codes and NAT**, so to handle a particular failure on a specific tool; it works, but it requires time, and this is a solution for long-term setups, that are not stable ... in other words, those custom programs are about changing the "timing", so to achieve clearance position on both turrets; is kind of a "maintanance" program


if cycle time is short, maybe you can simply trash the part and start all over again

if you enable eco-suite, regardless off "single-block", or "manual-intervention" state, and auto-timer is reduced ( check attached ), you will restart more often in mid-process / kindly

[okuma1984]

does Okuma have a FIND option? like Find a character or G or M code in my program ?eg in Fanuc we can just ask for an "item" [in edit mode] whether it be a coordinate or Feed or G code or M code etc and Arrow down or up

or if i want to copy something i Arrow a BLOCK or a character to select and then copy and paste.. . .. .. how would you do that in Okuma ?

[OkumaWiz]

Yes you have find replace cut copy paste all available. Copy 20 will copy 20 lines of code. Once copied it can remain in the extract buffer until you power off or copy something else into it. Between programs is no problem. No you can’t copy only portions of a line but need to copy full lines until you get to the p100 and newer controls. (Full windows in background )

[okuma1984]

Yes you have find replace cut copy paste all available. Copy 20 will copy 20 lines of code. Once copied it can remain in the extract buffer until you power off or copy something else into it. Between programs is no problem. No you can’t copy only portions of a line but need to copy full lines until you get to the p100 and newer controls. (Full windows in background )

ok so how do you find ?

say FIND "G80" in the program below?


G17 G20 G40 G49 G80 G90
T1 M06
G00 G54 X.5 Y1. S2000 M03
G43 H1 Z1.
G81 Z-.02 R.1 F2.
X1. Y.75
X1.5 Y1.25
G80
G00 Z1.
M05
G91 G28 X0. Y0. Z0.
G90
M30

[Algirdas]

use automatic line numbering feature and you find the line by it's number. When using "find" for restarting you can select the cycle ( in LAP ) number, which is not reflected in the text of part program at all.
Tip: make numbering with step 10 ( or 20, or 30 ) ant then you can easy replace all "0" with zero and space ( "0 " )

[OkumaWiz]

FIND/G80/
REPLACE/G80/G81/

To replace all of them use ;A after the command. You can also use “ marks instead of / so as to be able to find block delete. Ironically your question is actually the answer!

Best regards,

[okuma1984]

FIND/G80/
REPLACE/G80/G81/

To replace all of them use ;A after the command. You can also use “ marks instead of / so as to be able to find block delete. Ironically your question is actually the answer!

Best regards,

no wonder you're a wiz that actually worked. pretty cool

how about indexing the turret counter clockwise ? ?? is that an option ? was this possible 20 years ago so instead of the turret doing a whole revolution from 1 to 12 it would just go to 12 from 1 for example? do you know what i mean?

[OkumaWiz]

Yes is been standard for decades. Newer controls it is on the Turret parameter screen. Older ones it is a bit setting. #4 bit 7 = 1 will auto shortest path index. M86 and 87 will let you choose indexing direction otherwise.