G91 B axis move?

[DocHod]

Hi all can anyone give me a reason why I would get a improper G code alarm when all I want to do is move the B axis away from the part after it is cutoff in a G91 move I have the sample blocks of the program below any help I would be grateful , this is a Fanuc 18i controller on a Doosan 2500 lsy.
O7000
N100G0G90G40G80
G28U0.V0.
M1
N900(CUTTOFF)
M131(interlock by-pass sub spin.)
M110(close tooling by-pass)
M169T0200
G0X1.762Z0.T0202B-27.5
G4U100
G98
G1B-29.0F150.
G96S600M4
M204
M168
G99
G1X1.43F.003
G0X1.602
Z.06
G1X1.563
G3X1.438Z0.R.0625
G0X1.602
Z-.06
G1X1.563
G2X1.438Z0.R.0625
G1X-.03
G91B.02(RETRACT SUBSPIN .02 BEFORE X AXIS MOVES UP. improper G code alarm )
G0G90X8.0
M205
G28B0.
Z10.M9
G80
M30

[dcoupar]

As far as I know, there is no incremental command for B on the 2500SY. (X=U, Z=W, C=H, etc.), but there is no incremental B. You might consider using macro variables, instead of hard coded dimensions, i.e.:

in #504, put -29.0
in #505, put -28.98

O7000
N100G0G90G40G80
G28U0.V0.
M1
N900(CUTTOFF)
M131(interlock by-pass sub spin.)
M110(close tooling by-pass)
M169T0200
G0X1.762Z0.T0202B-27.5
G4U100
G98

G1B#504F150.

G96S600M4
M204
M168
G99
G1X1.43F.003
G0X1.602
Z.06
G1X1.563
G3X1.438Z0.R.0625
G0X1.602
Z-.06
G1X1.563
G2X1.438Z0.R.0625
G1X-.03

B#505(RETRACT SUBSPIN .02 BEFORE X AXIS MOVES UP. improper G code alarm )

G0G90X8.0
M205
G28B0.
Z10.M9
G80
M30

[Kai_DK]

Using a MS SL150smc I can confirm that there's no incremental axis for B.
I use G0G53Bxx to be sure where my sub-spindle is locateted, no matter which datum thats currently active.

[cnc-king]

the lathes do not use g91 for incremental moves

X = U
Z = W
Y = V
C = H
A = A
B = B

a xis for the mill mode on the subspindle and b for the subspindle
i usually command G53B0 after part off then move the x out of the way
the x will move even if the b is still moving

[DocHod]

I find it to be strange that Doosan would choose to not be able to move the B axis (sub spindle) in a G91 incremntal move when other machine builders do use the G91 move for the subspindle , we have a Viper VT 23 lathe that I can do a G91 move on the sub spindle . I will take your advice when I talk to the service people that we bought the machine from to make sure this is totaly true , thanks for your input.

[dcoupar]

Your Viper is probably set to use G-Code System B or C, which switch between absolute and incremental coordinates with G-codes (G90/G91). Doosan uses G-Code System A, which uses address characters to switch between absolute/incremental (X/U Z/W C/H) but Fanuc (not Doosan) doesn't provide an incremental address for B. System A allows mixed absolute/incremental commands within a block, i.e. X & W, or U & Z... System B & C do not.