Fanuc O-MB incremental input

[Paxo]

Mpe the parameter for radius/diameter that you are referin to is parameter 0001 bit 4, if set to 1 offset becomes diameter designation. If set to 0 offset becomes radius designation. Beware, if you dont know the correct way to alter this setting you could easily loose all your parameters. For more info drop me a email.

[MPE racing]

Thanks Paxo, I just had a look at Parameter 0001 and my bit 4 is set to 0. I'll change that to diameter...Thanks again

Greig
Motorcycle Performance Engineering
Brisbane

[Mortek]

Not Enough Fixture Offsets

I also have found this to be one of the best ways.I have worked for one
company that used to use G92 but found this to be a little more dangerous
especially if it requires jumping in prog i.e. say when the tool/tips need
replacing.Things don,t always go to plan as expected at first, it takes time
for proving method,etc.

We use the Zero Offsets in the program and it works just fine.
> I use this way to do it.
>
> N5 (TESTING OF USING ZERO OFFZET IN PROGRAM)
> N10 G10 L2 P1 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G54)
> N15 G10 L2 P2 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G55)
> N20 G10 L2 P3 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G56)
> N25 G10 L2 P4 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G57)
> N30 G10 L2 P5 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G58)
> N35 G10 L2 P6 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G59)
> N40 G90 M61 (CHANGE PALLETT TO NR 1)
> N45 P2000 T2 M98 ( CHANGE TOOL TO TOOL NUMBER 2)
> N50 G54 ( CALL OF ZERO OFFSET NUMER 1)
> N55 G0 G43 X99.99 Y99.99 Z15.00
> N60 ( CONTINUE OF THE PROGRAM....)
N90 M30

EXAMPLE OF A PROGRAM WITH OFFSETTS CHANGES, REMEMBER TO
LOOK CLOSELY AND YOU HAVE TO PUT THE USE OF G10 AHEAD OF
THE CALL OF YOUR ZERO OFFSETT. THATS VERY IMPORTANT, OTHERWISE
YOU JUST WRITE THE VALUES TO THE OFFSETT PAGE AND DONT
GET THE VALUES UNTILL NEXT PART,

The "L" refers to the Type of offsets you are setting when used with G10
(it does refer to repeats when used with sub calls). For example L2
refers to Work offsets, L10 to Tool offsets (yes you can offset tools
with G10) L11 - Tool Wear, L12 - Diameter offset, L13 Diameter Wear.
These may vary on your control and I would consult the manuals to see
which apply. You probably have figured out that "P" points to which
address to set.

Ken

[smabhyan]

Dear MPE Racing,

Press OFFSET / SETTING Key. Press Right Page-Up Key & 'OTHERS' Key, till you see a Softkey 'MEASURE'. Select any Free Work-Offset (G54, G55 etc.). Highlight the X or Y Value and press The 'MEASURE' Softkey, the Value in the 'Machine Co-ordinate system will be recorded in the respective G-Offset Table.

Now simply call the G-Offset in the program.

The Method Suggested by MORTEK is also good. However, you need Optional Work Offsets Beyond G59.

SMA

[Mortek]

The ability to load #'s into the offset registers solves the lack of more fixture offsets. I had a Chiron machine with the 180 degree rotating table (making two pallets so to say) I used all 6 offsets on each side of the table. I would load the new offsets in the program each time the table turned, enabling the use of more offsets.

Ken

[MPE racing]

smabhyam, my controller must be a bit different to yours.
The one I have is an O-MB. Even the G54 etc are just called, 01 02 03 04 etc......And you can't highlight the x or y line. You have to type it in to change it.

Maybe there is a parameter for that too.....who knows...

Greig

[Paxo]

Mpe racing, here's something that maybe of interest. These are unlisted parameters but her goes anyway.. Parameter 910 bit 1, for g54-g59, Parameter 911 bit 3 give you a clock!. I havent had chance to try them on a OMB control but I have used them on a OMT and OMC. As usual dont mess about with the parameters unless you know what your up to.

Next..........

[MPE racing]

Thanks Paxo, I'll have a look at it

Greig