Need Help!- Offset and tool setting

[mtnhntr]

How do you set the tool offsets on a 96 sl3 fanuc 11T the manual is confusing as all get out can someone explain in english

JB

[dbstream]

see attached. this might help

[underthetire]

You mean 86 sl3. And it will depend on if the machine is a negative x axis machine and set for manual absolute or not.

[FrankCNC]

You should have 3 offset screens,
Tool Offset (Wear)
Tool Offset (Geometry)
Work Zero Offset

Tool Offset (Wear) is used to adjust your diameters and lengths by using the Input and +Input soft keys below the screen.
i.e. 1.0 Input will place an offset of 1.0mm in the highlighted offset and overwrite an existing offset, 1.0 +Input will alter an existing offset by 1.0mm in the positive direction, -1.0 +Input will alter an existing offset by 1.0mm in the negative direction.

Tool Offset (Geometry) is used instead of the G50 program command in earlier controllers.
On our SL-7 with a Fanuc 11TA I have one tool I use as my setting tool,
The Tool Offset (Geometry) Z value for this tool will be Zero.
Call this tool up in MDI,
i.e. G0 T0303 EOB INSERT START
Touch this tool on the datum zero face of your work piece,
Then place the (Machine) Z coordinate displayed on the Absolute Position page in the Z coordinates (as a positive Figure) of the NO.00 (SHIFT) on the Work Zero Offset page.
i.e. 1000. INPUT

Machine a Diameter and then touch the tool on this diameter.
On the Tool Offset (Geometry) page cursor to the tools X value and
Type: X and the measured Diameter ( on the SL-7 it's a negative value)
Press the Right Arrow soft key below the screen and press the MEASURE key.
i.e. X-100. > MEASURE

Then manually index to the next tool you want to set,

Touch this tool on the Dia then on the Tool Offset (Geometry) page cursor to the tools X value and Type: X and the measured Diameter
press the Right Arrow soft key below the screen and press the MEASURE key.
i.e. X-100. > MEASURE
Touch this tool on the datum zero face of the work piece then on the Tool Offset (Geometry) page cursor to the tools Z value and Type: Z0
press the Right Arrow soft key below the screen and press the MEASURE key.
i.e. Z0. > MEASURE

Do the same for each following tool.

The Tools should now be set.

Just use G50 in your programs to set Max Spindle Speed not to set G50 X*** Z*** coordinates.
i.e.

( MWLNR RGH EXT 1.2R )

N10 G50 S280
G0 T0303 F0.35 M41
G96 S100 M3
G0 X-638. Z12. M8
G71 P11 Q12 U-0.5 W0. D3001
N11 G0 X-620.
N12 G1 Z-90.
G0 X-622. Z8.
G72 P13 Q14 U0. W0.15 D2001
N13 G0 Z0.
N14 G1 X-450.
G0 Z500. M9
T0 M5
M1

Hope this helps,
Frank.