[kawman]

Hi, i was wondering if someone with okuma dual turret machines can give me an example of the G code they run, i walked into this position where i have about 15 lathes mostly osp 7000l's but a few are the osp 5000, and the old programmer up and quit, so now i have to figure all this out with no help, im trying to get some cam software working, i would just like to see how other people are coding for these machines, so if anyone could give me just some examples of putting the turrets in to hold mode and tool changes, it would be greatly appreciated. here is code that the previous programmer wrote. thank you for all your help.



G13
DEF WORK
PS LC,[-46,0],[47,12]
PS LC,[-46,0],[47,05],0
END
DRAW
N1500 G13
N1505 VCHKL=1.150
N1510 VCHKD=.1 (CHUCK BARRIER)
N1515 VCHKZ=-4.5660 (Z-3.4160)
N1520 VCHKX=.1 (ACTUAL POSITION CHECK)
N05 G13
N10 M25
N15 G50 S3800
N20 DIA1 = .864 (O.D. FINISH SIZE)
N25 DIA6 = 1.01 (FLG. O.D. SIZE)
N30 DIA5 = .550 (ROUGH BORE SIZE)
N35 ZZ01 = -3.166 (FINISH LENGTH)
N40 ZZ02 = -2.283 (BODY LENGTH)
N45 FSID = .6090 (FINISH BORE SIZE)
N70 ZZ07 = -2.387 (OVERALL LENGTH MINUS SHORT BODY LENGTH)
N75 G00 X10.0 Z1.0 T0101 M09 M42 M05 P05
/N80 M01 M05 M09 P10 (O.D. HOLD)
N100 G14
N105 M25
N110 DIA7 = -.5900 (ROUGH BORE SIZE)
N115 DIA3 = -.6090 (I.D. FINISH SIZE)
N120 ZZ03 = -3.166 (FINISH LENGTH)
N125 G00 X10.0 Z15.0 T0707 M09 M42 M05 P05
N130 X0.
N135 Z15.
N140 IF VTOPC NTOP (BAR FEED)
N145 M77
N150 M84 (FEED OUT BAR END)
N155 M93
N160 M83
N165 M76 (BAR END DROP)
N170 M92
N175 M84
N180 G00 Z1.0
N185 M93
N186 G04 F.5
N190 G01 Z.050 F200. G94 (POSITION FOR NEW BAR)
N195 G95 M83
N200 G00 Z1.0
N205 M101
N210 X10.0 Z3.0 M92
N215 GOTO N380
NTOP
N225 Z= ZZ03 - .050 M84 (BAR STOP POSTIONING)
N230 M93
N231 G04 F.1
N235 G94 G01 Z.030 F200. (POSTION FOR NEXT PC)
N240 G95 M83
N245 G00 Z1.0
N250 M101
N255 X10.0 Z3.0 M92
/N260 M01 M05 M09 P10
N275 G13
N280 X10.0 Z1.0 S3200 T0101 M08 M42 M03 P15
N285 X=DIA6 + .325 Z.01
N290 G01 X=DIA5 - .200 F.009 (ROUGH FACE)
N295 G00 X=DIA1 + .020 Z.050 P20
N300 G01 Z=ZZ02 + .003 F.009 P25 (ROUGH O.D. BODY)
N335 X=DIA6 + .020
N340 G01 Z=ZZ01 - .175 F.010 (ROUGH FLG. O.D.)
N345 G00 X10.0 Z1.0
N350 M00 M05 M09 P30
N375 G14
N380 G00 X10.0 Z6.0 S3200 T0404 M08 M42 M03 P15
N385 X-.6480 Z3.0
N390 Z.050 P20
N391 G01 Z-.194 F.006 P25 (ROUGH CBORE)
N392 X=DIA7
N395 G01 Z=ZZ03 - .150 F.007 (ROUGH BORE)
N400 G00 X=DIA7 + .015 Z1.0
N405 X10.0 Z6.0
N410 M00 M05 M09 P30
N425 G13
N440 G00 X10.0 Z1.0 S2500 T0505 M08 M42 M03 P35
N445 X=DIA6 + .075 Z=ZZ02
N450 G01 X.813 F.003 (RELIEF GROOVE NEXT TO FLG.)
N455 X.803 F.001
N460 X=DIA1 -.015 F.005
N465 G02 X=DIA1 + .002 Z=ZZ02 + .0085 K.0085
N530 G00 X4.0
N535 X10.0 Z1.0

[budgieW]

The program looks OK, basically it is a "smart" parametric program that uses variables

G13 is top turret
G14 is the bottom turret.

Both turrets have the same coordinate axis so there fore can run the same Gcode. You can run normal Gcode if you wish

[underthetire]

And p codes are timing codes. The only other thing you need to worry about is G110 and G111, those are for constant surface footage, a and b turret respectively.

Sent from my G-Tab Quantum using Tapatalk

[MCR-B II]

My opinion is to try writing a simple program.

G13
G50 S1000
.use P codes
.
.
G14 (B Turret doing nothing)
M02

.Then same program for B turret but A is doing nothing.

You can learn with alarms.
But If IGF available then everything easy.

[kawman]

Thanks for all the advise guys, MCR-B II, what is IGF? i have been working out the bugs with my post processor, we are running bobcam, i believe i finally have a good program, i will know tomorrow for sure, 1 other thing i wanted to ask about, is are you guys familiar with using a taper bank? basically he was using the common variables, the operators would input the amount of taper into the common variables page, and then he would call that up with a diameter variable ex dia4 = dia3 + AA04, AA04 is the common variable the operator puts in, not sure how to incorporate that in to cam, just wondered if anyone has used it this way, i never have

[Algirdas]

IGF is an interactive dialog style Okuma software for part program creation. Complicated Okuma machinetools are equipped with IGF by default. What happens if you push the IGF button on OSP?

[underthetire]

By the time the 7000 came out, it was 1 touch IGF and pretty sure it was a pricy option on almost all the machines.

Sent from my G-Tab Quantum using Tapatalk

[kawman]

it must have been an option because none of our machines have it, it would be awesome if they did! for some reason i keep getting a plus axis over variable alarm on the XA, i will post some code maybe you guys can help me out, cause it doesn't make any sense to me and all the tools are touched off,


Ok here is code i generated from bobcad, on the id groove rough op i get a over plus variable on line 5016, even though it runs the top part of the code fine, and i put all the finishes together and it ran through with no problems, maybe there is something i am not seeing. any advise is much appreciated


$05274.MIN%
( PROGRAM NUMBER: 00100)
( PROGRAM START - TURNING CYCLES )
( PROGRAM NAME: 05274.MIN)
( POST: OKUMA OSP7000L )
( DATE: MON. 05/12/2014)
( TIME: 09:52AM)
( )
N01 G18 G20 G80 G90 G99
G14
N02 G00 X15. Z5.0 S500 T0101 M03 P05
/N03 M01 M05 M09 P15 (ID HOLD)

(Machine Setup - 1 Face Rough )
(TOOL #2 )
G13
N06 G00 X15. Z5.0 S500 T0202 M03 P05
N11 G50 S1000
N16 G97 S500 M08
N21 G00 X12.5 Z1.0
N26 Z0.
N31 G01 X10.5 F.006
N36 G00 Z5.0
N37 G00 X15.0 Z10.0
N41 M01 M05 M09 P15

(Machine Setup - 1 OD Rough )
(TOOL #2 )
G13
N55 G00 X15. Z10. S300 T0202 M03 P20
N60 G50 S1000
N65 G97 S300 M08
N70 G00 X12.7625 Z.05
N75 X12.5625
N80 G42 G01 X12.4625 Z0. F.008
N85 Z-5.315 F.008
N90 X12.5625 Z-5.265 F.008
N95 G00 Z.05
N100 X12.4625
N105 G01 X12.3625 Z0. F.008
N110 Z-4.915 F.008
N115 X12.456 F.008
N120 Z-5.315 F.008
N125 X12.556 Z-5.265 F.008
N130 G00 Z.05
N135 X12.3625
N140 G01 X12.2625 Z0. F.008
N145 Z-4.915 F.008
N150 X12.3625 F.008
N155 X12.4625 Z-4.865 F.008
N160 G00 Z.05
N165 X12.2625
N170 G01 X12.1625 Z0. F.008
N175 Z-.1476 F.008
N180 X12.21 Z-.2362 F.008
N185 Z-4.915 F.008
N190 X12.2625 F.008
N195 X12.3625 Z-4.865 F.008
N200 G00 Z.05
N205 X12.1834
N210 G01 X12.0834 Z0. F.008
N215 X12.1625 Z-.1476 F.008
N220 X12.2625 Z-.0976 F.008
N225 G00 X12.756
N230 Z-5.1863
N235 G01 X12.556 F.008
N240 G01 X12.356 Z-5.2863 F.008
N245 Z-5.315 F.008
N250 X12.456 Z-5.265 F.008
N255 G00 Z-5.2363
N260 G01 X12.2985 Z-5.315 F.008
N265 X12.3985 Z-5.265 F.008
N270 G00 X15.
N275 Z10.
N280
N285 M01 M05 M09 P30

(Machine Setup - 1 ID Rough )
(TOOL #2 )
G14
N295 G00 X15. Z10. S300 T0202 M03 P20
N300 G50 S1000
N305 G97 S300 M08
N310 G00 X10.64 Z.1
N315 Z.05
N320 G41 G01 X10.74 Z0. F.008
N325 Z-5.315 F.008
N330 X10.64 Z-5.265 F.008
N335 G00 Z.05
N340 X10.68
N345 G01 X10.78 Z0. F.008
N350 Z-5.315 F.008
N355 X10.68 Z-5.265 F.008
N360 G00 Z.05
N365 X10.712
N370 G01 X10.812 Z0. F.008
N375 Z-5.315 F.008
N380 X10.712 Z-5.265 F.008
N385 G00 X10.598
N390 Z10.
N395 X15.
N400
N606 M01 M05 M09 P30

(OD GROOVE ROUGH TOOL #6)

G13
N616 G00 X15. Z10. S300 T0606 M03 P40
N621 G50 S1000
N626 G97 S300 M08
N631 G00 X12.7625 Z-2.3429
N636 X12.5225
N641 G01 Z-3.6415 F.006
N646 X12.6225 Z-3.5915 F.006
N651 G00 Z-2.3429
N656 X12.4825
N661 G01 Z-3.6415 F.006
N666 X12.5825 Z-3.5915 F.006
N671 G00 Z-2.3429
N676 X12.4425
N681 G01 Z-3.6415 F.006
N686 X12.5425 Z-3.5915 F.006
N691 G00 Z-2.3429
N696 X12.4025
N701 G01 Z-3.6415 F.006
N706 X12.5025 Z-3.5915 F.006
N711 G00 Z-2.3429
N716 X12.3625
N721 G01 Z-3.6415 F.006
N726 X12.4625 Z-3.5915 F.006
N731 G00 Z-2.3429
N736 X12.3225
N741 G01 Z-3.6415 F.006
N746 X12.4225 Z-3.5915 F.006
N751 G00 Z-2.3429
N756 X12.2825
N761 G01 Z-3.6415 F.006
N766 X12.3825 Z-3.5915 F.006
N771 G00 Z-2.3429
N776 X12.2425
N781 G01 Z-3.6415 F.006
N786 X12.3425 Z-3.5915 F.006
N791 G00 Z-2.3429
N796 X12.2025
N801 G01 Z-3.6415 F.006
N806 X12.3025 Z-3.5915 F.006
N811 G00 Z-2.3429
N816 X12.2
N821 G01 X12.1625 F.006
N826 Z-3.6415 F.006
N831 X12.2 F.006
N836 X12.3 Z-3.5915 F.006
N841 G00 Z-2.3429
N846 X12.1625
N851 G01 X12.1225 F.006
N856 Z-3.6415 F.006
N861 X12.1625 F.006
N866 X12.2625 Z-3.5915 F.006
N871 G00 Z-2.3429
N876 X12.1225
N881 G01 X12.0825 F.006
N886 Z-3.6415 F.006
N891 X12.1225 F.006
N896 X12.2225 Z-3.5915 F.006
N901 G00 Z-2.3429
N906 X12.0825
N911 G01 X12.0425 F.006
N916 Z-3.6415 F.006
N921 X12.0825 F.006
N926 X12.1825 Z-3.5915 F.006
N931 G00 Z-2.3429
N936 X12.0425
N941 G01 X12.0085 F.006
N946 Z-3.6415 F.006
N951 X12.0425 F.006
N956 X12.1425 Z-3.5915 F.006
N961 G00 X15.0
N966 Z10.0
N971
N976
N981 M01 M05 M09 P50

(Machine Setup - 1 ID GROOVE ROUGH )
(TOOL #5 )

G14
N5001 G00 X15.0 Z10.0 S300 T0505 M03 P40
N5006 G50 S1000
N5011 G97 S300 M08
N5016 G00 X10.64 Z.1
N5021 Z-1.5642
N5026 G01 X10.74 Z-1.6142 F.005
N5031 Z-2.7166 F.005
N5036 X10.64 Z-2.6666 F.005
N5041 G00 Z-1.5642
N5046 X10.68
N5051 G01 X10.78 Z-1.6142 F.005
N5056 Z-2.7166 F.005
N5061 X10.68 Z-2.6666 F.005
N5066 G00 Z-1.5642
N5071 X10.72
N5076 G01 X10.82 Z-1.6142 F.005
N5081 Z-2.7166 F.005
N5086 X10.72 Z-2.6666 F.005
N5091 G00 Z-1.5642
N5096 X10.726
N5101 G01 X10.826 Z-1.6142 F.005
N5106 X10.86 Z-1.6776 F.005
N5111 Z-2.6532 F.005
N5116 X10.826 Z-2.7166 F.005
N5121 X10.726 Z-2.6666 F.005
N5126 G00 Z-1.6276
N5131 X10.76
N5136 G01 X10.86 Z-1.6776 F.005
N5141 X10.9 Z-1.7523 F.005
N5146 Z-2.5785 F.005
N5151 X10.86 Z-2.6532 F.005
N5156 X10.76 Z-2.6032 F.005
N5161 G00 Z-1.7023
N5166 X10.8
N5171 G01 X10.9 Z-1.7523 F.005
N5176 X10.9104 Z-1.7717 F.005
N5181 X10.94 F.005
N5186 Z-2.5591 F.005
N5191 X10.9104 F.005
N5196 X10.9 Z-2.5785 F.005
N5201 X10.8 Z-2.5285 F.005
N5206 G00 Z-1.7717
N5211 X10.94
N5216 G01 X10.98 F.005
N5221 Z-2.5591 F.005
N5226 X10.94 F.005
N5231 X10.84 Z-2.5091 F.005
N5236 G00 Z-1.7717
N5241 X10.98
N5246 G01 X11.0174 F.005
N5251 X11.02 F.005
N5256 Z-2.5591 F.005
N5261 X11.0174 F.005
N5266 X10.98 F.005
N5271 X10.88 Z-2.5091 F.005
N5276 G00 Z-1.7717
N5281 X11.02
N5286 G03 X11.06 Z-1.778 K-.0012 I-.039 F.005
N5291 G01 Z-2.5528 F.005
N5296 G03 X11.02 Z-2.5591 K-.0212 I.0327 F.005
N5301 G01 X10.92 Z-2.5091 F.005
N5306 G00 Z-1.778
N5311 X11.06
N5316 G03 X11.0962 Z-1.8111 K-.0213 I-.0332 F.005
N5321 G01 Z-2.5197 F.005
N5326 G03 X11.06 Z-2.5528 K-.0394 I0. F.005
N5331 G01 X10.96 Z-2.5028 F.005
N5336 G00 X10.598
N5341 Z5.0
N5346 X15.
N5351 M01 M05 M09 P50

(Machine Setup - 1 OD Groove Finish )
(TOOL #4 )
G13
N5356 G00 X15. Z5.0 S300 T0404 M03 P60
N5361 G50 S1000
N5366 G97 S300 M08
N5371 G00 X12.7625 Z-3.7115
N5376 X12.3
N5381 G01 X12.2 Z-3.6615 F.005
N5386 X11.9685 F.005
N5391 Z-2.3233 F.005
N5396 G00 X12.3
N5401 Z-2.2729
N5406 G01 X12.2 Z-2.3229 F.005
N5411 X11.9685 F.005
N5416 Z-2.3233 F.005
N5421 G00 X15.
N5426 Z5.0
N5431 M01 M05 M09 P70

(Machine Setup - 1 ID GROOVE Finish )
(TOOL #5 )
G14
N5436 G00 X15. Z5.0 S300 T0505 M03 P60
N5441 G50 S1000
N5446 G97 S300 M08
N5451 G00 X12.7625 Z.1
N5456 X10.698
N5461 Z-1.5642
N5466 X10.732
N5471 G01 X10.832 Z-1.6142 F.005
N5476 X10.9164 Z-1.7717 F.005
N5481 X11.0234 F.005
N5486 G03 X11.1022 Z-1.8111 K0. I-.0394 F.005
N5491 G01 Z-2.5197 F.005
N5496 G03 X11.0234 Z-2.5591 K-.0394 I0. F.005
N5501 G01 X10.9164 F.005
N5506 X10.832 Z-2.7166 F.005
N5511 X10.732 Z-2.6666 F.005
N5516 G00 Z5.0
N5521 X15.
N5526 M01 M05 M09 P70

(Machine Setup - 1 OD Finish )
(TOOL #6 )
G13
N5531 G00 X15. Z8. S500 T0606 M03 P80
N5536 G50 S1000
N5541 G97 S500 M08
N5546 G00 X12.7625 Z.05
N5551 X12.1734
N5556 G01 X12.0734 Z0. F.005
N5561 X12.2 Z-.2362 F.005
N5566 Z-4.915 F.005
N5571 X12.446 F.005
N5576 Z-5.2363 F.005
N5581 X12.2185 Z-5.35 F.005
N5586 X12.3185 Z-5.3 F.005
N5591 G00 X15.
N5596 Z8.
N5601 M01 M05 M09 P90

(Machine Setup - 1 ID Basic Finish )
(TOOL #6 )
G14
N5606 G00 X15. Z5.0 S500 T0606 M03 P80
N5611 G50 S1000
N5616 G97 S500 M08
N5621 G00 X12.7625 Z.1
N5626 X10.698
N5631 Z.05
N5636 X10.8586
N5641 G01 X10.9586 Z0. F.005
N5646 X10.832 Z-.2362 F.005
N5651 Z-5.0788 F.005
N5656 X10.9773 Z-5.35 F.005
N5661 X10.8773 Z-5.3 F.005
N5666 G00 Z5.1634
N5671 M01 M05 M09 P90

(Machine Setup - 1 Cutoff )
(TOOL #12 )
G13
N5676 G00 X15. Z8. S200 T1212 M03 P95
N5681 G50 S1000
N5686 G97 S300 M08
N5691 G00 X12.7625 Z-5.44
N5696 G01 X10.5586 F.005
N5701 G00 X15.
N5706 Z8. P105
N5711 M24 P110
N5716 G80
N5721
N5726
N5731 M01 M05 M09

( CATCH TOOL #10)
G14
N5732 G00 X15.0 Z8.0 S200 T1010 M03 P95
N5733 G00 X0.0
N5734 G00 Z2.0
N5735 G00 Z-5.0
N5736 G00 Z1.0 P105
N5737 M24 P110
N5759 M02
N5760 M30
%

[kawman]

The alarm i get is 2286-11, it makes no sense to me, cause i can hack the program up and parts of it will work fine, even with almost the exact same positioning,

[budgieW]

What line does it stop at?

[kawman]

LINE 5016

[fordav11]

that alarm means there is at least one X/Z in the program that is bigger than the variable limit.
in your case it is a PLUS variable limit. so either Z+ something or X+ something is too big.
either increase the variable limits or decrease the X/Z sizes in the program

[kawman]

i believe i figured it out today, once i took out the tool comp G42 and G41 it seemed to work, a little background on what im doing, i am trying to go off of the former programmers code, and i noticed that he would always send the machines to X25.0 Z10.0 for tool change, and we also have newer Geno okumas single turret with the osp200L and programming like that works fine no problem, i even use tool comp on those machines and it works fine, at the beginning of this thread i posted code from the former programmer, so you can see what im working off of, is there a special way to use tool comp on the dual turret machines? and thanks for your help fordav11

[budgieW]

If you use G41/G42 you will need to tell the machine which nose radius offset to use, so the offset call will be T020202

[fordav11]

if G41/G42 is the cause of the alarm, to fix the problem you need to put a G40 (tool nose radius comp cancel) at the end of the last rapid movement of the tool or somewhere where tool nose radius compensation is no longer required.
So for example......
N270 G00 X15. G40

also, if you are using CAM software and POST'ing code you don't need to use TNR comp you can just give it the nose radius and it will work it out and auto-generate correct g-code with the TNR comp included. That way you don't have to worry about it causing other issues and it's one less thing to check on the offset page.

regardless, you should ALWAYS cancel a G41/G42 at the end of each tool section before moving onto the next tool otherwise you may encounter undesirable results.

budgieW:
on my OSP7000L the tool radius is selected with the last 2 digits of the 4-digit tool number and the radius number is typed in the offset page at the end in the R column. T020202 does not work on my machine but my machine only has the most basic capability (no IGF, no TLM, 30M memory etc).
I have seen programs with Txxxxxx (6 digits) where tool nose radius comp was not being used so I figured it's for something else like tool life management or something?

[kawman]

Ok fordav11 so you are saying i don't really have to use the G41/42 as long as i have the TNR filled out on the offset page at the machine? it seems to be working ok with just straight G code no G41/42, i always seem to have some issues with chamfer size but i imagine that is the software, i will try the 6 digit tool line Txxxxxx and see if that does anything

[kawman]

I changed the tool format to T xxxxxx and then it would take the G41/42, so i got that figured out

[kawman]

what format is the stock displayed

DEF WORK
PS LC,[-46,0],[47,12]
PS LC,[-46,0],[47,05],0
END
DRAW

can someone tell me how this works? i am guessing that it is metric, this is just something i copied from the former programmer, thanks again for all your help guys