[rcs60]

The machine is a daewoo Lynx 210 lathe
Control is a Fanuc oi-t
alarm 011 feed rate not commanded happens at the g28u0.w0. line of the program

%
:4098(38/357 SEAT)
G54
G50S3500
N1
(ROUGH TURN)
(DNMG332)
G28U0.W0.
G97M3S1500T0101
M8
G0X1.Z.1
G96S400
G1X.925Z0.F.06
X-.1F.005
Z.05F.06
X.500
Z0.F.004
X.5885
G3X.7535Z-.077R.077
G1Z-.260
X.835Z-.35
Z-1.925F.008
X.925F.02
G0X1.5Z.1
G97S1500
G28U0.W0.
M9
/M01

the only thing that works is to add a feed rate at the beginning of the program then the program works good and the feed rate can be taken out of the program
most times this alarm occurs at start up but this last time it happened after the machine ran 2 pcs.
these are programs that have worked for over 7 years with no trouble before

[Superman]

So where are your safety codes ?

These are normally the default settings the machine sets at startup

ie

%
Oxxxx ( comment ) ( short comment on this line allows to show up on DIR list )
G20                    ( Safety line #1 ) ( This an inch program, verify the M/C is set to inches, if not STOP )
G00 G18 G40 G80 G99 M9 ( Safety line #2 ) ( Set Rapid, XZ Plane, Cancel Tool Compensation, Cancel Canned Cycle, Feed per Rev, Coolant OFF )
G54 M5                 ( Set co-ord system, stop spindle )
G50 S3500              ( Limit maximum RPM )
G28 U0 Y0              ( Go home ) ( tool MUST be clear of any obstruction ) 
M1
()
N1 ...

Even if you 1/2 way thru a program, the safety codes would set the machine back to the initial settings

[blizzzard30]

Try G98 G28 U0 W0;G99 G97 M3 S1500 T0101;

[dcoupar]

Sounds like it's defaulting to G01 at startup and reset?
What happens if you add a G00 in the G28 U0. W0. block?