Faunuc 6t error code 010

[mechan12]

I have a faunuc 6t on a morie sekie 3l lathe and yesterday it started giving me a 010 error code. I looked up the code and it stands for trying to use a g code the machine is not able to ( like not a relesed opiction)
the g code i was trying to us is a g50 to set my tool positions .
I belive some how it has locked out the parametere for the g code.
Dose anyone know whic parametere it is and what it needs to be set at .
thanks for your help
mechan12
ps the machine will run the other g codes with no problom
mechan 12

[ezjn]

Could you send me your program to look at to see if i see anything wrong it sound like theres a problem in the program

[mechan12]

i know it is not the program cause i went to a program i had been running that moring and it dose the same thing and so i went to a program i keep stored in the machine that i wrote a year ago and it dose the same thing . when it reads a g5o code the code is writing as follows g50 x-7.374 z10.0 s2500 ;

[mechan12]

here is the program
g50 x-7.374 z10.0 s3000;
go t808 m7;
m42;
g96 s 400 m3;
go z0.1;
go x-1.55 m8;
g71 p1 q2 uoooo woooo d0300 f0.0100;
n1 g0 x-1.0 ;
n2 g1 z-1.5;
g0 x-7.374 m9;
g0 z10.0 m5;
g0 t800;
g50 x-8.17 z7.375 s400;
g0 t101 m17 ;
m41;
g97 s400 m3;
go z0.1;
g0 x0.0 m8;
g1 z-0.2 f0.002;
g0 z0.1 m9;
g0 x-8.17;
g0 z7.375;
g0 t100;
g50 x-8.17 z2.456 s400;
g0 t505 m17;
m41;
g97 s400 m3;
g0 z0.1;
g0 x0.0 m8;
g1 z-3.0 f0.002;
g0 z0.5 ;
g0 z-2.9;
g1 z-4.5;
g0 z0.5;
g0 z-4.4;
g1 z-4.75;
g0 z0.5;
g0 x-8.17 m9;
g0 z2.456;
g0 t500;
m30;
the fault is 010 witch in the book says an unusable g code was commanded.(this alarm is generated also when a g code with which the control is not equipped as an option is commanded.)
thanks for your help
mechan12

[Sung daecheol]

Dear Mr. mechan12,
G50 is not option, is a basic function.
Could you send me Parameter data from No.0 ~ to No.4, and from No.300 to No.304.?

[Dan Fritz]

Sung daecheol is right that G50 is a standard feature, not an option. There is, however, another reason why G50 might not work.

Check parameter 007, bit 5 (the 6th bit from the right). If this bit is a "1", then the Fanuc will use "Special G-codes", which are different from the JIS (Japanese Industrial Standard) G-codes. Normally, the Fanuc 6T uses G50 to preset the position registers, but if this bit is set to "1", the G50 no longer works and G92 presets the registers instead. G50 might then throw the alarm #10.

Another parameter that affects G-codes is the option parameter #302 bit #5 (the 6th bit from the right). This bit is called "EIA G-codes". As far as I know, the only difference between "EIA G-codes" and "Special G-codes" is that G20/21 for inch metric becomes G70/71 in EIA.

In the 6T operators manual, you will see that the list of G-codes has 3 columns. Which column you use is determined by parameter 007, bit 5 and parameter 302 bit 5. I suggest that you set both of these parameters to "0" to be sure that all the JIS G-codes work properly.

[mechan12]

here is the paramters that are in the machine
0000=10101010
0001=01101101
0002=11101000
0003=10101000
0004=00000000
0005=00000010
0006=11010001
0007=11000000
300=00011100
301=10101010
302=01101101
303=11101000
304=10101000
305=00000000
Some more info when i got to the shop i found out that the machine was stuck in mm mode and g 20 didnt work eather ,but when i read this i went back and g92 works and g 70 and g71 sets the inch and metric mode now
thanks again for the help you all are giving me
mechan12