[gmilosevic]

I'm new to Okuma machines and the IGF programming system. The other day I wrote a program for our lathe & all of the G02'S & G03"s came out backwards. meaning the instead of the code being a G02 it posted out as a G03 and vice versa. Can someone tell me why by looking at the program, I don't see a way to attach a IGF file. Thanks in advance any help would be appreciated. :drowning:

$A5136-FC-OD-GM.MIN%
G13
VTLIN[1]=3
VTLFN[1]=1
VTLL[1]=1.6000
VTLA2[1]=5.0000
VTLA1[1]=80.0000
VTLIN[1]=3
VTLFN[1]=1
VTLL[1]=1.6000
VTLA2[1]=5.0000
VTLA1[1]=80.0000
VTLIN[1]=1
VTLFN[1]=1
VTLL[1]=1.6000
VTLA2[1]=55.0000
VTLA1[1]=80.0000
VTLIN[1]=1
VTLFN[1]=1
VTLL[1]=1.6000
VTLA2[1]=5.0000
VTLA1[1]=80.0000
VTLIN[12]=7
VTLFN[12]=3
VTLL[12]=1.6000
VTLA2[12]=35.0000
VTLA1[12]=55.0000
VTLIN[9]=2
VTLFN[9]=1
VTLD[9]=1.5000
VTLL[9]=6.0000
VTLA2[9]=5.0000
VTLA1[9]=80.0000
VTLIN[7]=8
VTLFN[7]=1
VTLD[7]=2.0000
VTLL[7]=6.0000
VTLA2[7]=5.0000
VTLA1[7]=80.0000
VWKR=393.7007
VCHKL=0.4000
VCHKD=7.1000
VCHKX=7.1000
VCHKZ=0.0000
DEF WORK
PS LC,[17,0],[6,35]
PS LC,[0,0],[17,71]
PS LC,[0,0],[23,14],0
END
DRAW
N0001 G13
N0002 G00 X30 Z50
N0003 G50 S2500
NAT01
N0050 G97 S796 M44 M03 M08
N0051 G00 X3.6 Z2.4 T010101
N0052 Z2.3
N0053 G96 G110 S750
N0054 G85 N0055 D0.1 F0.012 U0.01 W0.01
N0055 G82
N0056 G00 Z2.131
N0057 G01 X3.46 G41 E0.012
N0058 X1.4
N0059 G40 I-0.0004
N0060 G80
N0061 G00 Z2.4
N0062 G97 S796 M09
NAT01
N0100 G97 S398 M42 M08
N0101 T010101
N0102 G00 X7.2
N0103 Z1.723
N0104 G96 G110 S750
N0105 G85 N0106 D0.1 F0.012 U0.01 W0.01
N0106 G82
N0107 G01 Z1.484 G41 E0.012
N0108 X3.5 E0.012
N0109 G40 I-0.0004
N0110 G80
N0111 G00 Z2.4
N0112 G97 S398 M09
NAT01
N0150 G97 S398 M08
N0151 G00 X7.2
N0152 T010101
N0153 Z1.6
N0154 G96 G110 S750
N0155 G85 N0156 D0.2 F0.012 U0.01 W0.01
N0156 G81
N0157 G00 X6.5529
N0158 G01 Z1.4833 G42 E0.012
N0159 X6.699 Z1.4682 E0.012
N0160 Z0.5 E0.012
N0161 G40 K-0.0004
N0162 G80
N0163 G00 X7.2
N0164 G97 S398 M09
NAT01
N0200 G97 S819 M08
N0201 T010101
N0202 G00 Z2.2
N0203 X3.5
N0204 G96 G110 S750
N0205 G85 N0206 D0.2 F0.012 U0.01 W0.01
N0206 G81
N0207 G00 X2.9921
N0208 G01 Z2.131 G42 E0.012
N0209 Z1.9468
N0210 G02 X3.1417 Z1.7161 I0.393 K-0.0001
N0211 G01 Z1.4783
N0212 G40 K-0.0004
N0213 G80
N0214 G00 X7.2
N0215 G97 S819 M09
N0216 X30 Z50 T0100
(FINISH PROFILE DNMG-432)
NAT12
N0250 G97 S314 M08
N0251 G00 X7.2 Z1.6 T121212
N0252 G96 G110 S591
N0253 G87 N0254
N0254 G81
N0255 G01 X6.8 Z0.5 G42 F0.012
N0256 X6.6929
N0257 Z1.4534

(ALL OF THE G02'S & G03'S ARE REVERSED WHY)

N0258 G03 X6.6855 Z1.4582 I0.0013 K0.0048
N0259 G01 X6.5429 Z1.4773
N0260 G03 X6.5277 Z1.4783 I-0.0034 K0.0037
N0261 G01 X3.3196
N0262 G03 X3.3131 Z1.4772 I-0.0031 K0.0039
N0263 G01 X3.1415 Z1.439
N0264 Z1.7161
N0265 G02 X2.9921 Z1.9468 I-0.393 K0.0002
N0266 G01 Z2.123
N0267 G03 X2.9861 Z2.126 I0.0017 K0.0047
N0268 G01 X1.4
N0269 Z2.226
N0270 G40 K-0.0004
N0271 G80
N0272 G00 X7.2
N0273 Z1.6
N0274 G97 S314 M09
N0275 X30 Z50 T1200

NAT09
N0300 G97 S1616 M44 M08
N0301 G00 X1.3 Z2.4 T090909
N0302 G96 G110 S550
N0303 G85 N0304 D0.2 F0.015 U0.01 W0.01
N0304 G81
N0305 G00 X2.1
N0306 G01 Z2.126 G41 E0.015
N0307 X1.875 Z1.936
N0308 G40 K-0.0004
N0309 G80
N0310 G00 X1.3
N0311 G97 S1616 M09
N0312 Z2.4
N0313 X30 Z50 T0900
NAT07
N0350 G97 S2204 M08
N0351 G00 X1.3 Z2.4 T070707
N0352 G96 G110 S750
N0353 G87 N0354
N0354 G81
N0355 G00 X2.1
N0356 G01 Z2.126 G41 F0.012
N0357 X1.875 Z1.936
N0358 X1.3
N0359 G40 K-0.0004
N0360 G80
N0361 G00 X1.3
N0362 Z2.4
N0363 G97 S2204 M05 M09
N0364 X30 Z50 T0700
N0365 M02

[deadlykitten]

hello

just replace in your code G02 with G03 and vice-versa if it works, don't bother yourself ...
...or
put the drawing here, and i will give you code that should work for your required operation // sometimes is easier to restart rather than look for mistakes ...

kindly !

[deadlykitten]

what is this part ? do i need it ?

$A5136-FC-OD-GM.MIN%
G13
VTLIN[1]=3
VTLFN[1]=1
...
VCHKX=7.1000
VCHKZ=0.0000
DEF WORK
PS LC,[17,0],[6,35]
PS LC,[0,0],[17,71]
PS LC,[0,0],[23,14],0

[OkumaWiz]

You have an error is your shape definition. If you look at line N255 there is a Z0.5. You then start feeding Z positive using a G42 and your G2/G3 are reversed which indicates shape errors primarily with reference, start, and end points. Look at them In IGF for errors.

N0251 G00 X7.2 Z1.6 T121212
N0252 G96 G110 S591
N0253 G87 N0254
N0254 G81
N0255 G01 X6.8 Z0.5 G42 F0.012
N0256 X6.6929
N0257 Z1.4534


Best regards,

PS> Kitten - you're trying to hijack a thread again.... ;-)

[deadlykitten]

i am glad you have the patience to read code ... about hijacking, i changed my mind

i think is just some auto-generated code that does what it does and i can leave without it

[gmilosevic]

Thanks for the advice. I did change the G02's & 3's it worked with a little bit of tweaking.

I also need to write a program for Okuma LU15M that requires live tooling. I cant find a programming manual anywhere. does anyone have a sample program and a list of G & M Codes for live tooling? I have to drill, Tap, & Mill a slot in the lathe & I don't have a clue what the codes are.

[deadlykitten]

( drill / mill going like a drill )

V1=1800 (n ... o/min)
V2=0.12 (f ...mm/o)
V3=15 ( X coordinate)
V4=-2.8 ( Y coordinate) (XY coordinates on spindle frontal surface, where x0y0/origin is on spindle / machine main axis)

M110 ( switch from S to C mode )
SB=V1 M13 M08
G137 ( switch from XC to xoy mode )
G0 X=V3 Y=V4 Z5 ( come in front of hole @ 5mm clearance )
M147 ( break )
G01 Z-30 F=V2 G95 ( cut inside for 30mm )
G04 F=0.7/V1 * 60 ( wait for the tool to complete 0.7rotations )(G04 F... =wait for F milisenconds )
G01 Z=VSIOZ+0.3 F=V2 G95 ( disengage contact between tool nose and material at cutting feed, among 0.2 ..0.3 ..0.5 mm )
G00 Z5 ( go back in front of part )
M12 ( tool rotation stops )
M146 ( remove break )
G136 ( back to XC mode )
M109 ( back to S mode )

if process is not so powerful, you can remove M147 and M146, but it is recomended to use them

After tool has reached bottom you can use both, or only one of this, or none
G04 F=0.7/V1 * 60 ( wait for the tool to complete 0.7rotations )(G04 F... =wait for F milisenconds )
G01 Z=VSIOZ+0.3 F=V2 G95
-if none is used, than consider hole to have no bottom; if it has bottom, than you will retract the tool while it's teeth will be cutting, and you fill force the tool ... wear is not visible, but exists
- G04 can be there without the G01
- G01 only asures that tool retracting will not begin at full speed when tool nose is at hole bottom

now, for driling with tool retraction :

V100=-30
G01 Z=V100 F=V2 G95
G04 F=0.7/V1 * 60
G01 Z=VSIOZ+0.3 F=V2 G95
G00 Z5
G00 Z=V100+0.5

V100=-60
G01 Z=V100 F=V2 G95
G04 F=0.7/V1 * 60
G01 Z=VSIOZ+0.3 F=V2 G95
G00 Z5
G00 Z=V100+0.5

V100=-70 ( on last cutting, drill only 10mm at 70%feed ) ( you must reduce feed as hole gets deeper )
G01 Z=V100 F=V2*0.7 G95
G04 F=0.7/V1 * 60
G01 Z=VSIOZ+0.3 F=V2 G95
G00 Z5
(G00 Z=V100+0.5) ( no need to reenter once you finished )

also, when hole gets deper tool might get stuck when retracting, because it has chips on it

also, retracting from deeper holes, if is done at high speeds, will make the chips to fall from tool inside the hole, and when tool reenters you may crash those chips; these happens on 2insert drills; so retract like this :

G01 Z=VSIOZ+0.3 F=V2 G95
G01 Z5 F1000 G94
...or
G01 Z=VSIOZ+0.3 F=V2 G95
G01 Z5 F=V2*30 G95 ( idea is to reduce speed when leaving/re-entering )

now, for driling with chip-breaking :

V100=-30
G01 Z=V100 F=V2 G95
G04 F=0.7/V1 * 60
G01 Z=VSIOZ+0.3 F=V2 G95 ( only break the chip segment, and continue )

V100=-60
G01 Z=V100 F=V2 G95
G04 F=0.7/V1 * 60
G01 Z=VSIOZ+0.3 F=V2 G95

so you can interrupt cutting for "tool retraction" or "chip-breaking" at some Z positions;if distance between these positions is equal, and also you wish/can keep always same feed, than you can use a simple code like the one that i don't have it now, but i'll give to you

let's drill a deep hole :

V1=1800 ( n ... o/min )
V2=0.12 ( f ...mm/o )
V3=15 ( X coordinate)
V4=-2.8 ( Y coordinate)

M110
SB=V1 M13 M08
G137
G0 X=V3 Y=V4 Z5
M147
CALL OSUB V100=-45 V101=V2*1 V102=0
CALL OSUB V100=-60 V101=V2*1 V102=0
CALL OSUB V100=-70 V101=V2*0.7 V102=1
M12
M146
G136
M109

...OSUB

...G01 Z=V100 F=V101 G95
...G04 F=0.7/V1 * 60
...G01 Z=VSIOZ+0.3 F=V2 G95
...G00 Z5
...IF [ V102 EQ 1 ] GOTO N0001
...G00 Z=V100+0.5
...N0001

...RTS

now going for multiple holes with same geometry :

V1=1800 ( n ... o/min )
V2=0.12 ( f ...mm/o )

M110
SB=V1 M13 M08
G137

CALL OS01 V3=x_1 v4=y_1
CALL OS01 V3=x_2 v4=y_2
...
CALL OS01 V3=x_n v4=y_n

M12
G136
M109

...OS01
...G0 X=V3 Y=V4 Z5
...M147
...CALL OSUB V100=-45 V101=V2*1 V102=0
...CALL OSUB V100=-60 V101=V2*1 V102=0
...CALL OSUB V100=-70 V101=V2*0.7 V102=1
...M146
...RTS

...OSUB

...G01 Z=V100 F=V101 G95
...G04 F=0.7/V1 * 60
...G01 Z=VSIOZ+0.3 F=V2 G95
...G00 Z5
...IF [ V102 EQ 1 ] GOTO N0001
...G00 Z=V100+0.5
...N0001

...RTS

now puting some load-monitor on that, so to use nice the little tool
for more details about load-monitor search trough recent forums- there is one about it
only inside cutting procedure

...OSUB

...VLMON[1]=2 ( monitor Z axis ON )
...G01 Z=V100 F=V101 G95
...G04 F=0.7/V1 * 60
...G01 Z=VSIOZ+0.3 F=V2 G95
...VLMON[1]=0 ( monitor Z axis OFF )
...G00 Z5
...IF [ V102 EQ 1 ] GOTO N0001
...G00 Z=V100+0.5
...N0001

...RTS

this ensures safe cutting, but some times tools have problem when retracting or reentering the hole, for different reasons, like :
- tool bended, and when retract it scretches the hole, or when reenters it misses and go to bend some more
- wall is thin and jaws deform material after cutting, and tool stucks at retreat
- insert breaks nasty, and can not retreat at all the tool
all this does not happen often, but is enough to happen once
so use load monitor on retact/reenter code, but use on a diferent adress :
- all this above can happen when tool retract / reenter effort is greater than cutting effort

...OSUB

...VLMON[1]=2
...G01 Z=V100 F=V101 G95
...G04 F=0.7/V1 * 60
...G01 Z=VSIOZ+0.3 F=V2 G95
...VLMON[1]=0
...VLMON[2]=2
...G00 Z5
...IF [ V102 EQ 1 ] GOTO N0001
...G00 Z=V100+0.5
...N0001
...VLMON[2]=0

...RTS


kindly!

( i have never done tapping on M axis )
( if you need complex milling, just let me know )

[gmilosevic]

Thank you deadlykitten, I have worked with c axis on Mori Seiki's and HAAS machines and I didn't have to use macros. Do you have anything without the macros that may be useful to me. I am a newbe with the Okuma control, still working on the basics.

Thanks
Gmilosevic

[deadlykitten]

i was going to give you simple code, but please wait until i get one )

the reason i wrote all that is it because it covers particular cases that you might get into, and simple code will not help you there

is harder to learn it, but once you got it is way faster

[deadlykitten]

does anyone have a sample program and a list of G & M Codes for live tooling? I have to drill, Tap, & Mill a slot in the lathe & I don't have a clue what the codes are.

// this goes for whatever goes left : drill / mill / center ...


G271
CLEAR
DRAW
N0001 G00 X500 Z200 ( turret safe position )
N0002 G50 S2000 ( S axis limit )
NAT07
N0100 M110 ( S > C )
N0101 G94 M146 M15 M08 ( ... )
N0102 G00 X55.714 Z3 T0707 SB=1600 (X/2=SQRT[x*x+y*y])
N0103 G137 C0 ( spindle oriented; can be skipped if after M110 and before M110 is active M109/modal )
N0104 G00 X10 Y26 ( hole position )
N0105 G183 X10 Y26 Z-50 K0 F320 E0.07 D106 L106 ( F320 = 1600 x 0.2 )
( e : bottom delay )
( d : step / chip breaking )
( l : tool retracting )
( G183 : machine intrinsec code )
N0106 G180
N0107 G00 X10 Y26 Z3 ( final position, before retract )
N0108 G136 ( spindle no more oriented )
N0109 G95 M12 M09
N0110 M109
N0111 G00 X500 Z200 T0700
N0112 M02

[deadlykitten]

Do you have anything without the macros that may be useful to me. I am a newbe with the Okuma control, still working on the basics.

this is igf / is it good 4 you ?

hope it works on " Okuma LU-35 OSP 7000L " ... ?!

about tapping, go syncro-holders ... kindly!

[gmilosevic]

Thanks everyone, I will let you know how it all turns out.

Goran.

[Chispas]

Thanks everyone, I will let you know how it all turns out.

Goran.

Ja sa pocetnik u IGF
U stvari volio bih da naucim IGF na Okuma 7000L