[stude8]

I'm not sure where to post this question so I'll post it here since I'm most familiar with Okuma Lathes. I've been sequence restarting Okumas for 30 years so that's not my problem.
Recently I bought a Dainichi with a Fanuc 6T and I use G71 for lap programming and G70 for the finishing cycle. My question is how do I pick up the finishing pass for a rerun? Thanks.

[tea hole]

You sell it, buy an Okuma, reprogram the part for OSP, then run it in there.

But seriously, it has to do with you running in dry run and turning it off when you're ready to continue I believe. But you'd be better off looking on a different forum. Even a mori or clausing forum maybe.

[stude8]

That's what I ended up doing. Ran in dry run mode to the finish pass. Thought there might be a different way.

BTW I do have about a dozen Okuma lathes including 3 LC-40"s. But this Dainichi has a 21 inch Kitagawa chuck, 60 inch between centers and does bigger work. Even dry running it takes a very long time to get to the finish pass.
Thanks for your response.

[fordav11]

nar that's the wrong way to do it.

put single block on. In MEMORY run the program to where the tool is positioned before the G71 line, switch to EDIT and cursor to the G70 line. Put back to MEMORY, single block off and press start. that works on every Fanuc control I've ever seen from 6T to latest 32i

[stude8]

Thanks guys. I tried it this morning and all is good. I had looked through all the manuals but could not find anything.

[fordav11]

its not in the manual. it's a secret ;-)
actually they would never tell you that because it requires knowledge of the program and what it does and since every program is different they can not cover all bases. if someone were to carelessly skip over program lines without knowledge of what they are doing it would present a crash situation.

[Tancuda]

You can try this program format also,

and when you want to finish only, you push the "block delete" button.
I don't have my program in front of me, but it should look like this:

0010
Header.......
Tool, rpm, coolant
G0 X Z (approch)
\G71 P100 Q200 etc......
P100 shape.......
shape ..............
shape ..............
Q200 shape end
\G70 P100 Q200 etc....
go home
M02

[stude8]

Thanks Tancuda. Looks like that would work. Am I correct in saying that in line P100 I would put the finishing speed and feed? But what if I want to use a DNMG instead of a CNMG for finishing?

[fordav11]

that example is for 1 tool. yes you can add a finishing speed to the first P100 line.
if you want a different tool for finishing add another process and just give it the G70
like this.....

N1 G50 S1000
G0 T0101
G96 S.... M3
G0 X.... Z....
G71 P100 Q200 etc......
P100 shape.......
shape ..............
shape ..............
Q200 shape end
go home
T0100
M01

N2 G50 S1000
G0 T0202
G96 S.... M3
G0 X.... Z......
G70 P100 Q200 etc....
go home
T0200 M5
M02


if you want to run the finish cut go to edit, cursor to N2, switch to memory and press start.

[Tancuda]

Sorry for the delay Stude8,
fordav11 is correct, my program are for a large vertical lathe with one big part at a time, so I don't mind
changing the tool number, and cycle start every time, but for small machine with lot's of parts, fordav11's method is good.

[stude8]

Thanks all! I understand and now will save lots of air cutting time.