How to start program from defined place

[=aike=]

Hi!
I need to start program not from begining but from some defined place in program.
For example not from 1st string but from 20th.
How can I do it? I tried to find it in my manual, but unfortunatly.
OSP5000, Lathe LC20.

[fordav11]

use RESTART.
select A turret, softkey RESTART, type Nxxx press WRITE
select B turret, softkey RESTART, type Nxxx press WRITE
Press SEQUENCE RESTART button
Press START

[=aike=]

use RESTART.
select A turret, softkey RESTART, type Nxxx press WRITE
select B turret, softkey RESTART, type Nxxx press WRITE
Press SEQUENCE RESTART button
Press START

Nxxx - is it the sequenced number of string (1,2,3,....100) or it is the LABLE
(N11, N12, N100)?

[Thawk53]

Nxxx - is it the sequenced number of string (1,2,3,....100) or it is the LABLE
(N11, N12, N100)?

You need to have a sequence number at the start of each tool or machining process. N1, N2, N3 etc. These are the numbers you use for the restart procedure fordave11 explained. Be sure to use restart, not number search.

[littlerob]

You need to have a sequence number at the start of each tool or machining process. N1, N2, N3 etc. These are the numbers you use for the restart procedure fordave11 explained. Be sure to use restart, not number search.

No you don't. The sequence numbers appear in the top right side of the screen. For each motion the machine goes through there is a number designated to it. You can restart on any of those numbers, just be cautious.

Robert

[fordav11]

but you have to have pre-recorded those sequence numbers while the machine was running in auto because they don't relate to actual program line N numbers.
Its far simpler and practical to put N numbers at the start of each tool and restart from there.

[Ashish B]

I think that a great way to use a macro program.


Suppose you are at X200.0 Z-130.0 in the previous cycle.

You should place a code in the NC Program ( this is the position at which you want to start the program in the next cycle )
#101=#5021
#102=#5023

One more modification should be done at the start of the program. It would be -
01234
G90G54G80
G00X#101Z#103
M03 S2000
------
------
------
M30

The codes written in the BLUE colour will locate the tool to the desired position..



P.S - I have used common variables to store the machine position & then commanded G00X_Z_ at those variable values.

Thanks
Ashish

[fordav11]

eh? that may work on Fanuc but definitely not on Okuma. And since this is an Okuma question and it was solved at post#2.......

[littlerob]

but you have to have pre-recorded those sequence numbers while the machine was running in auto because they don't relate to actual program line N numbers.
Its far simpler and practical to put N numbers at the start of each tool and restart from there.

I agree it is simpler, but disagree with practicalitiy. I don't want the machine to run through an entire cycle to make a single cut. You can get the appropriate number by locking the machine and seeing the sequnce # during dry run, or since you already ran it you should have recorded the #, it doesn't make any sense to restart if you haven't run it all ready. But if you want to cut air for half an hour, that's cool.

[fordav11]

it depends on the job and the operator. some people have trouble just keeping track of insert wear
across 2 turrets loaded to capacity with tooling
Personally I'd just run it again from the start of that tool. My programs are hell-optimized and take 5-10
minutes so it's no big loss to lose 1 minute. I could always dry run it too if I wanted to.
I'd rather waste 2 minutes waiting than waste 1-2 hours fixing the machine after an operator
crashed it because of an incorrect restart pick-up point.