Improper G Code

[lfacio12]

I've got a programming problem with an Okuma & Howa ACT 3 lathe with Fanuc 15-T control... thanks to DCoupar I got the rough canned cycle syntax which is the following
G71 P100 Q200 U0.025 W0.010 D0.050 F0.008 S700
and when I run my program it gives me an Improper G Code alarm when it gets to this line... Does anyone know why its giving me this error
Thanks

[gandp]

I've got a programming problem with an Okuma & Howa ACT 3 lathe with Fanuc 15-T control... thanks to DCoupar I got the rough canned cycle syntax which is the following
G71 P100 Q200 U0.025 W0.010 D0.050 F0.008 S700
and when I run my program it gives me an Improper G Code alarm when it gets to this line... Does anyone know why its giving me this error
Thanks

Put the S700 a line above the G71 line and use no decimal when expressing D value. In your case your D value is D500.

[lfacio12]

Gandp, I've made the changes you suggested but it's still giving me the Improper G Code Alarm.... This lathe has recently been purchased by the company I work for and I'm wondering if there is such a situation where this lathe doesn't support canned cycles....Any ideas?

[stevo1]

Improper G-code typically means that the machine does not support the canned cycles that you are programming. IOW the canned cycle option is not activated in the control.

Stevo

[gandp]

Improper G-code typically means that the machine does not support the canned cycles that you are programming. IOW the canned cycle option is not activated in the control.

Stevo

Ok, that may be the case, but could it also be the "2 line" method he needs here? Example

G71 U.05 (.05 depth per cut)
G71 P100 Q200 U.025 W.01 F.008

[lfacio12]

I've tried the "2 line" command and I'm still getting the same error.... I'm thinking that i don't have the canned cycle option enabled on this machine... how do I enable this feature?

[gandp]

pm sent

[rajanvadakkepat]

try this method.
G71 U 0.20 R0.50;
G71 P 100 Q200 U0.01 W0.0 F 0.0002;
N100 G0 X ... Z 0.0;
G1 X.....
..
...
...
N200 G 0 Z 2.0;
G28 U0.0 W0.0

[gandp]

try this method.
G71 U 0.20 R0.50;
G71 P 100 Q200 U0.01 W0.0 F 0.0002;
N100 G0 X ... Z 0.0;
G1 X.....
..
...
...
N200 G 0 Z 2.0;
G28 U0.0 W0.0

Oh that's right rajanvadakkepat. It's been a while for me with this. Would this be for the 15t or did fanuc use this style after that? The R value is depth of cut and the U is finish allowance? I don't know why they couldn't keep it to one line anyway.

[angelw]

try this method.
G71 U 0.20 R0.50;
G71 P 100 Q200 U0.01 W0.0 F 0.0002;
N100 G0 X ... Z 0.0;
G1 X.....
..
...
...
N200 G 0 Z 2.0;
G28 U0.0 W0.0

I doubt that the way in which the G71 cycle is programmed will generate an Improper G Code alarm. If the control uses the two block G71 system, omitting the first block results in the values previously set being used, as the values are modal and non-volatile with power off, it does not cause an Improper G Code alarm.

Stevo's comment regarding the control not supporting the canned cycles being programmed is correct and the most likely cause of this alarm condition.

Regards,

Bill

[lfacio12]

Thanks guys for your input... i've tried all the methods suggested and the machine still gives me an Improper G Code alarm. As Bill has suggested, I really do think that this machine does not have canned cycles enabled and so I guess I'm stuck at programming line by line.

[sinha_nsit]

G90 and G94 might be available which will simplify programming a little bit.