Robo drill Fanuc 16 - 18

[jorgehrr]

Machine Center

I usually send turret home for indexing programming:
G91G28Z0.

I stared working in a different machine and they have:
G49G53Z0

What is the difference and witch one is the best choice.


Thank you in advance

Cheers

[dcoupar]

G91G28Z0 does a "Return to Reference Position" in Z with no intermediate move specified. You could program G91G28Z5.0 and Z would rapid up 5.0 THEN do the "Return to Reference Position".

G49G53Z0 rapids to Z0 in the Machine Coordinate System (G53) and cancels Tool Length Comp (G43/G44).

Six of one, half-dozen of the other, IMHO. I've seen G91G28Z0 used more often than G49G53Z0.

[jorgehrr]

Thank you for you replay.

I need to standardize the programs, so I'll use
G91G28Z0.

Thank you

Jorge

[mmurning]

i use go g49 zo, it works best

[gwood]

Fanuc Machining Center
? I usually send turret home for indexing programming:
G91G28Z0.
I started working on a different machine and they have:
G49G53Z0
What is the difference and which one is the best choice?
Jorgehrr
************Reply************
G91G28Z0. (INCREMENTAL / RAPID TO 1ST REF POSITION)
Moves an INCremental distance of zero in Z, and then rapids the
Z Gage Line (No Tool Length Active) to Machine Z=0. Normally top of stroke
on most Fanuc machine commissions.
Always follow this line with a
G90 (ABSOLUTE MODE) to avoid wrecks!

G53 Always cancels the Active Tool Length, then rapids to Machine Coordinates.
On some newer software bases the dropping of the LENGHT Offset
can be made with no movement. On most older Fanuc's, and depending on who commissioned the machine the cancellation of the offset will cause a Rapid movement Down into the part; and then G53 rapid up in machine coordinates.
On the later 18iMBs I always commission the parameters to activate with no move.

I know that the N101 G91G28Z0; followed by N102 G90; is effective and reliable without a wreck not dependant on the parameters set by the builder/user
Greg W.

[jorgehrr]

Thank you all for your replays.

Jorge