fanuc 6m- work offset help

% (WORK OFFSETS SEPT 00) G10G90 L2 P0 X 00068870 Y-00098480 Z-00156530 B 00000000 G10G90 L2 P1 X 00000000 Y 00000000 Z 00000000 B 00000000 G10G90 L2 P2 X 00000084 Y 00000101 Z 00000000 B 00000000 G10G90 L2 P3 X 00000000 Y 00000000 Z 00000000 B 00000000 G10G90 L2 P4 X 00000000 Y 00000000 Z 00000000 B 00000000 G10G90 L2 P5 X 00000000 Y 00000000 Z 00000000 B 00000000 G10G90 L2 P6 X 00000000 Y 00000000 Z 00000000 B 00000000

Where as :

P0 X=distance g28 home to center of table,

P0 Y=distance g28 home to pallet surface and,

P0 Z=distance g28 home spindle gage line to center of pallet rotation.

Once you've carefully dialed in input qualified the above parameters, ( G53 ) you DONT f*ck with them unless there's been a terrible crash or somesuch....

Instead, you'll want to use the values P1 through P6 as G54 through G59 respectively as your work coordinates.

HTH

Thanks PT, Few questions

1. G10G90 L2 P0 X 00068870 Y-00098480 Z-00156530 B 00000000

What are these values assigned by you in xyz

1. P0 X=3Ddistance g28 home to center of table

we dont have this data, any ideas how to calculate this

thanks aga> > hello,

1. G10G90 L2 P0 X 00068870 Y-00098480 Z-00156530 B 00000000

What are these values assigned by you in xyz

1. P0 X=distance g28 home to center of table

we dont have this data, any ideas how to calculate this

Many ways, but for simplicity sake imagine bolting a cube to the exact center of the table, painstakingly bumping it around and indicating, etc be dead center rotating through B 0, B90, B180 and B270 degrees and testing in z.

Now if that cube is say 4in, and then you pickup one edge with an edgefinder, then if you now move over exactly 2in...this be your x rotary centerline.

====

Boot up the machine and set all origin at g28 position to Zero...(press x then origin, next press y then origin then pres z then origin and finally

4th/5th/ then origin....this gives you all zeros in the readout....now any manual jogging from here on out will give you the correct value and sign that needs to be input.

After setting X, leave that cube there, and bring the spindle gage line up to the block...you might need a 3in or larger block...but the reading and block length added together is then your z value.

Cutting tool hieghts will now be entered as positive values, and they will be actual tool lengths as measured in a tool presetter.

===

Be aware the command G90 Z0 will drive the spindle face to rotary centerline if no height offset is active and so operators must be extremely careful if jogging around using mdi commands

thanks again PT we got a local expert and finally got it right,the problem seems to be the INC/ABS issue, the machine seems to remember the INC and not ABS , so we got it to go home every time so that it takes the ABS values,now we took work offset, tool offset and every thing seems fine.

btw can u tell us some thing abt the LIBRARY AND PROGRM CHK page, does the 6m has this option at all, our other machines gave 0m,0i in which these features are standard.

we ran into one more problem,some times during tool change the spindle does not orient properly and trips off to an overload alarm but no alarm nos are displayed except for the red light indicating spindle overload.any ideas

thanks a lot again rags

Precisi> Thanks PT,

Those funtions may not be active...if they are, then something I've not found any use for.

Orient position can be adjusted...but actual method depends on actual spindle inverter model...ours has 3 'pots' ( actually they are rotary decade switches ) on the top card, but I'd need to have your actual card # in order to check my fanuc book.

FWIW, I had similar problems once, just before the encoder belt broke...and another time where the pully was slightly loose on it's shaft.....again, several setups exist and so yours might be completely different than ours in this function..

Good luck with it, once you get these running properly you'll find they are a very dependable controller.