Need G68 mirror code for 3T

[Axxtion]

I've got a Fanuc 3T on a Victor flat bed with 2 turrets. I have been programming the front turret with X+ and the rear turret with X- forever, and the post on my cad/cam doesn't support this. I have written a macro in my editing software to handle this. I would like to use the G68 mirror code for the rear turret so that i can program both turrets using X+. I understand that G68 was an option on this control. The machine is about 28 years old and I don't want to call Fanuc. How can I switch this on?

Similar Threads:

• Newbie- Mirror imaging
• Newbie- Mirror Parts
• Mirror - is this a bug?
• Mirror image G-code
• Mirror thickness

[Al_The_Man]

I don't think there is any separate option parameters on the 3T like there is on later Fanuc's (Par.900's and 9000's). I would guess they are situated within the general parameters, if you have the manual detailing parameters, you will notice that there are a lot of 'unused' bits, these maybe the ones used for the options.
Failing actual proof of which turns the G68 on, if you can find someone with a machine with this option turned on, you could compare your parameter list with his and see the differences, and if they are not mentioned in the manual then it is likely they could be one of the options you are looking for.
Its a long shot but maybe worth it.
Al.

[n174k]

Axxtion,

Post your email address

[Axxtion]

Thanx guys but i got it figured out. it works great

all the best

[Ozcad]

Thanx guys but i got it figured out. it works great

all the best

Hi I also have acquired a Victor twin tool
post lathe would really like your help with the syntax for G68

Regards
Nick

[Axxtion]

Hey Nick,

Here's an old program. T1-T4 are front post using G69 and T5-T8 are the rear post using G68.

%
O1( 30524-0100 01V.NC )
G28U0.W0.
( VICTOR 3T )
( 3/2/06 AT 5:26 PM )
( )
( TOOLS )
( TOOL 1: 0.03125 RAD. 80-DEG. DIAMOND )
( TOOL 3: 0.008 RAD. GROOVING )
( TOOL 5: 0.500 DIA. DRILL )
( TOOL 6: 0.007 RAD. 80-DEG. DIAMOND )
( )
( OPERATION 1: CONTOUR )
( PROFILE )
G69
( TOOL 1: 0.03125 RAD. 80-DEG. DIAMOND )
G50X0.Z0.
S9T0100M3
G0X1.4375Z5.T0101
Z.1
G1Z.002F.006
X-.0625
( OPERATION 2: ROUGH )
( PROFILE )
G69
( TOOL 1: 0.03125 RAD. 80-DEG. DIAMOND )
G0Z.1
X1.5
Z.0688
G1X1.25F.006
X1.1
Z-.2813
X1.25Z-.2812
G0Z.0688
G1X.95
Z-.2813
X1.1
G0Z.0688
G1X.884
Z-.2812
X.95Z-.2813
( OPERATION 3: CONTOUR )
( PROFILE )
G69
( TOOL 1: 0.03125 RAD. 80-DEG. DIAMOND )
G0X1.5
Z.05
X.5
G1X.417F.006
Z0.
X.7842
G3X.834Z-.0103K-.0352
G1X.8534Z-.02
G3X.874Z-.0449I-.0249K-.025
G1Z-.2812
G0X1.5
Z5.
X0.Z0.T0100
M1
( OPERATION 4: HOLES )
( PROFILE )
G68
( TOOL 5: 0.5 DIA. DRILL )
N1G50X0.Z0.
S9T0500M3
G0X0.Z1.T0505
Z.1
G1F.006
Z-.35
G0Z1.
X0.Z0.T0500
M1
( OPERATION 5: ROUGH )
( PROFILE )
G68
( TOOL 6: 0.007 RAD. 80-DEG. DIAMOND )
( CIRCLE MACHINE QCMI-500 BAR )
N2G50X0.Z0.
S9T0600M3
G0X.5Z1.T0606
Z.1
Z.093
G1F.006
X.65
Z-.207
X.5
G0Z.093
G1X.74
Z-.207
X.65
( OPERATION 6: CONTOUR )
( PROFILE )
G68
( TOOL 6: 0.007 RAD. 80-DEG. DIAMOND )
( CIRCLE MACHINE QCMI-500 BAR )
G0X.5
Z.0706
X.7
G1X.7819F.006
X.8526Z.0352
X.7564Z-.0129
G2X.75Z-.0207I.0078K-.0078
G1Z-.1863
G0X.7
Z1.
X0.Z0.T0600
M1
( OPERATION 7: CONTOUR )
( PROFILE )
G69
( TOOL 3: 0.008 RAD. GROOVING )
( .118 WIDE )
N3G50X0.Z0.
S9T0300M3
G0X1.5Z5.T0303
Z.1
Z-.1626
G1X.9915F.006
X.9208Z-.1979
X.8477Z-.2345
G3X.8307Z-.238I-.0085K.0085
G1X.5315
M9
M5
G0X1.5
G0Z5.
X0.Z0.T0300
G69
M30
%

My old post would not generate G68 or G69.

I used an editor that has macro ablility and wrote the following to edit the program.

Top
Find "
( TOOL 1"
Replace All "
G69
( TOOL 1"
Top
Find "
( TOOL 2"
Replace All "
G69
( TOOL 2"
Top
Find "
( TOOL 3"
Replace All "
G69
( TOOL 3"
Top
Find "
( TOOL 4"
Replace All "
G69
( TOOL 4"
Top
Find "
( TOOL 5"
Replace All "
G68
( TOOL 5"
Top
Find "
( TOOL 6"
Replace All "
G68
( TOOL 6"
Top
Find "
( TOOL 7"
Replace All "
G68
( TOOL 7"
Top
Find "
( TOOL 8"
Replace All "
G68
( TOOL 8"
Top