What's new
What's new

fanuc alarm 011-no feedrate commanded

jimliu5360

Plastic
Joined
Oct 31, 2013
Location
fullerton, ca
hi all,
I am new for the cnc program and I got a alarm message from my fanuc programming and it showed " no feedrate commanded"
I don't know how to fix it because I already specify the feedrate when I do the program.
any idea?
BTW, if you are familiar with fanuc oi-mc controller, the company will pay your time for coming or email&phone support!
please contact me for detail
Thanks!
 
What software are you running? I get this error randomly. We use PowerMill here.

Open the file in Note Pad and make sure there is a Feedrate after the G1.


N10 G1 Z3.3063 F500.
 
Here is a lathe example from my website(doccnc.com), are you learning a lathe or a mill?
02010*
N1 G50 S2000 *
N2 T0101*
N3 G96 S500 M3*
N4 G0 G42 X2.0 Z.1 M8* (Set comp to the right)
N5 G1 Z-1.0 F.008*(Comp is calculated by control where needed based on size of noseradius, shape of part and the tool shape)
N6 X2.5 Z-1.7*
N7 Z-2.5*
N8 X3.2*
N9 G0 G40 X6.0 Z6.0 *(Make sure to cancel comp)
M30*
There are a lot of examples to learn from for free.
If you need training right there, let me know: Heinz.
 
Many Fanucs default to G91G1 on reset or startup. If you don't program G0 to get the machine moving, it will be trying to move in linear interpolation and no feed has yet been specified.

My guess is that's your problem.
 
Ok its obviously a mill since he said oi-Mc.

Try this
G94 G01 G91 X5.0 F5 (The G94 is feed per minute)
G90

Your control might be stuck in G95, feed per revolution, and should not move unless the spindle is running.
 
I am having the same problem with alarm 011 no feed rate commanded this has just started happening with in the last 2 months
the control is a fanuc oi-t on a daewoo lynx 210 2 axis lathe

here is a sample of the beginning of the program these are programs that have not had this alarm for about 7 years
it always alarms out at the g28u0.w0.
today i inserted G0G90G99 prior to the n1 still no difference until I added f30. after the g99 then it ran good
this program actually ran 3 pcs. before the alarm came up
%
:4098(38/357 SEAT)
G54
G50S3500
N1
(ROUGH TURN)
(DNMG332)
G28U0.W0.
G97M3S1500T0101
M8
G0X1.Z.1

any ideas would be welcome
 
I am having the same problem with alarm 011 no feed rate commanded this has just started happening with in the last 2 months
the control is a fanuc oi-t on a daewoo lynx 210 2 axis lathe

here is a sample of the beginning of the program these are programs that have not had this alarm for about 7 years
it always alarms out at the g28u0.w0.
today i inserted G0G90G99 prior to the n1 still no difference until I added f30. after the g99 then it ran good
this program actually ran 3 pcs. before the alarm came up
%
:4098(38/357 SEAT)
G54
G50S3500
N1
(ROUGH TURN)
(DNMG332)
G28U0.W0.
G97M3S1500T0101
M8
G0X1.Z.1

any ideas would be welcome

Maybe try this...

:4098(38/357 SEAT)
G50S3500
G00 G28 U0.0 W0.0 (Probably don't need the G00)
N1
(ROUGH TURN)
(DNMG332)
T101
G97 M3 S1500
G0 G54 X1.Z.1 M8
G01 Z0.5 F1.0 (Or whatever safety distance you want)
 
Never heard about G28 needing a feedrate. I am curious to know the reason.
Is there a chance that G28 is redefined using macros?
 
I don't this is not a problem with the g28 being redefined
most of the time the problem occurs at power up but the last time it occurred the machine had already run thru 2-3 pcs then the alarm showed up the only soulution i have found so far is to add a feed rate at the beginning of the program (the feed rate does not matter)-- 30. to 300. i have put in to the program when it reaches the g28 it is always a rapid travel (G0)Thanks for the replies
 
I just had this problem using mastercam and a HAAS mill.
We ran the program once, and then we started the program the next day and used HAAS's program restart feature where it looks through the code to make sure it doesn't miss necessary codes. Well it errored out (320 no feed rate) on part of the program that we had already run. Luckily it gave us the line that it was having a problem with so we added an F10 there. Started the program again and it was fine. The controller scanned through the program, and started on the line that we wanted to continue from. I don't know how we could have run the program through the first time without a problem but when it scanned it it threw up an error. Thoughts?
 
I don't know about Haas, but there is a possibility :A code such as G01 needs a feed rate at least in its first call. It assumes the same feed rate in subsequent calls if F is not specified. If a program is run from the middle, it is possible that F is missing.
 
hi all,
I am new for the cnc program and I got a alarm message from my fanuc programming and it showed " no feedrate commanded"
I don't know how to fix it because I already specify the feedrate when I do the program.
any idea?
BTW, if you are familiar with fanuc oi-mc controller, the company will pay your time for coming or email&phone support!
please contact me for detail
Thanks!

.
many machines when
1) reset pressed
2) M2 or M30 used
.
resets to the defaults often G54, G1, G90, G80, F not stated or zero, etc
.
this is a safety thing. its suppose to alarm out. often if program doesnt stated
G1 with F or G0 and it just stated a coordinate like X,Z or XY it is suppose to alarm and stop.
.
at good restart point you need to check
work offset active or stated like G55 or G54
G17 or G18 or G19
G1 with F1.0 or whatever feed you want or G0
G94 or G95 how feed is stated inch per min or per rev
S100 M3 or turn spindle on
M8 turn coolant on
G43 H1
G41 D2 or what ever tool comp needed make sure active
it often defaults also to H0 D0 so obviously if thats not correct comp for current tool thats also a problem
G80 turn drill mode off as if active and you give XY or XZ it will drill a hole
.
it alarms out as you can easily scrap a part many ways if the defaults are active and thats not what you need or want
 
I just had this problem using mastercam and a HAAS mill.
We ran the program once, and then we started the program the next day and used HAAS's program restart feature where it looks through the code to make sure it doesn't miss necessary codes. Well it errored out (320 no feed rate) on part of the program that we had already run. Luckily it gave us the line that it was having a problem with so we added an F10 there. Started the program again and it was fine. The controller scanned through the program, and started on the line that we wanted to continue from. I don't know how we could have run the program through the first time without a problem but when it scanned it it threw up an error. Thoughts?

When you power down it doesn't keep track of all the defaults and safety lines. So in the morning, you're asking it to move but not specifying how fast. If it's been running it will default to the last known feedrate.
 
My guess is you have commanded a G93 which needs a feedrate on every line.

Haas controls default to G90 and G95. So G93 would not only need to be inserted intentionally into the program, but on power up, and Restart it would need to read it before cycle start.

Plus you need to activate the 4th parameters. While I've never tried using G93 without a 4th :), I'm guessing the Haas control won't allow it.

R
 








 
Back
Top