Problem- c axis feed rate on a turn /mill machine

[bike]

Have an OM-LTD turn mill machine and can not get the feed rate for the C axis mill mode to work. I have anFANUC 18i-T controld. Any one been through this before??

N366( TOOL #03 OFFSET #03)
N368( 1.00 END MILL )
N370( MILL THE O.D. )
N372( OP# 12 )
N374G97S19100M3
N376G0X38.8876Z3.C.007M8
N378G12.1
N380X38.8876C0Z3.
N382Z-.25
N384G42G1C.3F11.46 Feed here at full c axis rate
N386G3X38.6876C.3R.5
N388G2X38.6876C-.0025R19.3438
N390X-38.6876C.0025R19.3438
N392X38.6876C-.0025R19.3438
N394X38.6876C-.005R19.3438
N396G3X38.8874C-.305R.5
N398G1G40X38.8876C-.005
N400C-.005Z3.
N402G13.1
N404G18
N406M9
N408G28U.0W.0 M05
N410T0300
N412M0


thanks Bike

[CNCRim]

check to see if you still have G94(feed per rev) or G95 feed(feed per min).... G95 is what you want.

Other thing, I don't see and code switch to milling mode.

[g-codeguy]

Not familiar with your control. How is M3 starting the live tooling instead of the main spindle? Or does the main spindle use a different M-code?

[cnc-king]

Originally Posted by newtexas2006 check to see if you still have G94(feed per rev) or G95 feed(feed per min).... G95 is what you want. Other thing, I don't see and code switch to milling mode.

G94 & G95 are for the mills

the lathe uses

G98 Feed per Minute
G99 Feed per Rev

and he needs to active his mill mode
the live tool uses a different M code than the main spindle

[Stebedeff]

I have a Deawoo Puma with Fanuc 18 . I always use M33 G97 S... to start the " mill " Do you call it "live tooling" in the US? Always wonderd what "live tooling" meant.
Then G98 G00 X.. Z.. C.. M08.
When done with the milling call G99 or you'll get a "NO FEEDRATE" alarm when you go back to turning.
As for G12.1, I use G112 or I get "inproper G-code alarm". Same for G13.1 ( G113 ).

[g-codeguy]

Originally Posted by Stebedeff I have a Deawoo Puma with Fanuc 18 . I always use M33 G97 S... to start the " mill " Do you call it "live tooling" in the US? Always wonderd what "live tooling" meant. Then G98 G00 X.. Z.. C.. M08. When done with the milling call G99 or you'll get a "NO FEEDRATE" alarm when you go back to turning. As for G12.1, I use G112 or I get "inproper G-code alarm". Same for G13.1 ( G113 ).

Pretty much how we do it. Guess it got called "live tooling" because the tools move whereas standard tools are "dead". Hope one doesn't say "Hi" to me one day. LOL.