LB3000EX M110 Error

[BrentGM]

I have an LB3000EX with and OSP-P300L controller. Every time I try an M110 code and spits out a 2672-01 Alarm-B C-axis sync command format. I look in the book for the alarm diagnosis and its all just jibberish. Now for the weird part, if I restart the machine on the line after the code the C-axis will clamp and do everything as it should. I tried re-running a program that I know has been proven and worked with the M110 and that would alarm out as well. Not sure if this is a parameter issue or machine issue but I've been stuck at the same line of program for 3 days.

N0001 G140
N0002 G00 X50 Z50
N0003 G50 S3000
NAT08
N0100 G00 X50 Z50
N0101 M110
N0102 G94 M146 M15
N0103 X.4515 Z-0.15 T080808
N0104 C0
N0105 G138 C90.

If i start from beginning the program will fault out at line 101, if I restart from line 102 the program will run fine.

Any help is greatly appreciated!

Similar Threads:

• Need Help!- Kiaturn 15lms code m110 sub spindle trouble
• how to check if Caxis in on / M110 ?
• Need Help!- mastercam post for okuma lb3000ex
• Okuma LB3000EX-MYW or Takisawa EX910?
• Need Help!- OKUMA LB3000EX MYW MASTERCAM POST

[deadlykitten]

G140 ( is there a 2nd spindle ? )
G50 S3000
G00 X50 Z50
M110
G94 M15 ( M146 )
G00 X0.4515 Z-0.15 C90 T0808(08)
G138
//
G136 M12
M109

[BrentGM]

Yes but it's not being used

[deadlykitten]

try replacing M110 with G271; maybe it will work, but i doubt it; seems like the controller believes that there is a sync; i don't have a 2nd spindle, but i would try some codes that disables the sync ( i guess there exist something )

G140
G271
G50 S3000
G00 X50 Z50
( M110 )
G94 M15 ( M146 )
G00 X0.4515 Z-0.15 C90 T0808(08)
G138
//
G136 M12
M109

i am sorry, i can not say anything else / kindly

[BrentGM]

I tried replacing M110 with G271 and unfortunately when I call up G271 the machine calls up a subprogram that reads

VBNCT=1
M110
VBNCT=0
RTMCR

[deadlykitten]

yup, the G271 calls a sub / i really don't know what RTMCR does, but i hoped that maybe it will fix that issue of yours

look for "sync cancel codes", or "machine default state codes"

i am sorry, i can not provide exact codes, since i don't have experience with 2nd spindle

i think you should reduce your program length to a minimal few lines ( thus eliminate everything that is not related to this problem ), and post that short version here; maybe someone sees something

the initial code you posted is only a paragraph; maybe there is a sync code ( or something ) later inside your program, and it remains enabled ( thus it is not canceled by M02 or by reset button, but the restart sequence handles that by default )

if you go power off, power on, MDI , M110, do you still receive that error ?

kindly

[OkumaWiz]

It appears that your c-axis is trying to perform synchronized rotation. Is by chance an M151 active earlier in the program? Do you have the sync function and use the M888-M890 with the c-axis?

Try the M110 in MDI to see if you get the alarm.

[bdots]

It appears that your c-axis is trying to perform synchronized rotation. Is by chance an M151 active earlier in the program? Do you have the sync function and use the M888-M890 with the c-axis?

Try the M110 in MDI to see if you get the alarm.

I am having the exact same problem as the original poster, however my issue started occurring after the Multus I run was shut down and then powered back up.
Even attempting to use M110 in MDI gives me the same C-axis sync command alarm. I've tried a multitude of codes to get the C-axis to lock, but it keeps coming back with various alarms telling me the C-axis is not connected or unclamped.
I can use G19 with a C value and the spindle will lock in place and rotate the amount I tell it to, but it seems to have lost it's "home" C zero position.
I'm hoping there's just a G or M code I can give it that I've overlooked, but am unsure what direction to go next.
If anybody that has posted in this thread has any advice, it would be much appreciated!

[deadlykitten]

hy seems your machine remained hung, for whatever reason; so far, i had not experience such an error, but i would try some combination of these :

M888 C-axis synchronized control OFF OPTION
M889 C-axis synchronized control ON (A turret command) OPTION
M890 C-axis synchronized control ON (B turret command) OPTION
M891 Sub spindle C-axis joint OFF OPTION
M892 Sub spindle C-axis joint ON OPTION

M150 Synchronized rotation OFF OPTION
M151 Synchronized rotation ON OPTION

I can use G19 with a C value and the spindle will lock in place

before you start experimenting, use m19 on both, so to be sure that they are both phased, not only main spindle ...

[bdots]

M888 for the win! Thanks much, you saved me a ton of time and headache.
No idea how it looped itself into needing that code to snap itself out, but I'll take it.
Strangely enough, the spindles now no longer orientates themselves to C zero with the M110 code as they did before, I have to manually tell them to go to C zero after the M110. But that's just a minor inconvenience and one I'm not too worried about.

Thank you again sir, much appreciated!

[OkumaWiz]

M888 for the win! Thanks much, you saved me a ton of time and headache.
No idea how it looped itself into needing that code to snap itself out, but I'll take it.
Strangely enough, the spindles now no longer orientates themselves to C zero with the M110 code as they did before, I have to manually tell them to go to C zero after the M110. But that's just a minor inconvenience and one I'm not too worried about.

Thank you again sir, much appreciated!

Check your parameters because there is one that will eliminate the secondary C0 move when set to ON.

Look in Multiple machining parameters:

Return of the C-axis to the home position when it is connected
Select whether to return the C-axis to the home position when executing the C-axis connection command




Initial setting: Do not

Change to do.

Best regards,

[deadlykitten]

Strangely enough, the spindles now no longer orientates themselves to C zero with the M110 code as they did before

hy just like mr wizard said : optional para \ multiple machining \ 08 c-axis return to origin, or bit #39.5

M110 engages C axis, then may/may not index to C0, depending on that parameter state, thus :
... one setting needs more time, and leaves c axis indexed at origin c0
... the other setting is faster, and leaves c axis indexed at actual spindle phase, thus random c axis position ( is similar to engaging c axis in manual mode ); example where to use this setting :
...... your operation is careless about using c0 as reference, like driling at x0, or non center milling operations on parts that won't be subject to restart ( like many small ones, where it does not matter if you trash a few )
...... as a cycle-time-reduction technique, when turret aproach comand block involves also C, thus C axis will no longer be indexed to origin as before (alone), but toghether with turret motion; there are more details about this, but i guess is enough for now

M888 for the win! Thanks much, you saved me a ton of time and headache

nice glad it worked, i didn't ever used it, because i don't have c axis syncronized option, but i heard of it before ?!