2336 Alarm B - OSP7000M / MC-60VAE

[Tytan]

The alarm "2336 Alarm B Wrong T command" comes up when a program reads the tool change block and the tool being called is already in the spindle.

Is there a parameter that can be changed to remedie this issue?

I don't have a manual for this machine, so any input is greatly appreciated.

Similar Threads:

• okuma osp7000m back up
• Need Help!- Setting up OSP7000M DNC
• OKuma Osp7000M manuals
• MC-60VAE
• DPRNT on OSP7000M/OSP700M?

[budgieW]

The short answer is no

Change your programs to

G0 Z999.
N1 IF [VTLCN EQ 2] N2
T2
M6
N2 G0 Z999.
G15 H1

[Algirdas]

I don't understand, what the proper action is if part program calls the tool already clamped in spindle. It is an error in part program, I guess.
The situation if part program was interrupted makes diference. There are several ways to restart the part program and it is the normal way to continue work.
I can't imagine situation where part program detects the spindle tool. Operator must be sure about machine preparation before launching part program, according Okuma philosophy.

[broby]

My opinion is that the problem is with the Programmer/Operator.
The machine is supposed to create an error condition when the program calls up a tool number that is already in the spindle!
If the operator is trying to do a sequence restart, then they are starting on the wrong line.
If T1 is in the spindle and then the program calls T1 again, of course this is going to be a problem.
By all means, you could use coding to check the tool number first, but why? You (the programmer) already should know what tool number is in the spindle, otherwise what are you trying to do?
Use the following M codes to control tool change actions:
M6 Tool exchange with staged tool
M63 No Next Tool.
M64 Return Staged tool to magazine

A typical program (for our MA600H and MC600H Mills anyway) would follow this method

T1 (Pre-stage tool#1)
M6 (Tool 1 into Spindle)
T2 (Pre-stage Tool#2)
N1...
.Program for tool#1
.
M6 (Swap T1 for T2)
T3 (Pre-stage Tool#3)
N2...
.Program for Tool#2
.
M6 (Swap T2 for T3)
M63 (No more tools required, i.e. Pre-Stage tool pot is now empty)
N3...
.Program for Tool#3
.
M6 (Return T3 to magazine, Spindle and Pre-Stage pot now empty)
M2 (end of program)

Restarting points would be N1 for Tool 1, N2 for T2, N3 for T3...
Can even put the restart line number on the T# lines, so that a restart will make sure the "Next" tool is called up, from memory, our machines do not alarm if the tool is already staged... but if it is not in the pre-stage pot and then the next M6 command is reached, an alarm will occur.
Hope this helps?
Cheers
Brian.

[Tytan]

Thanks guys…
Since I program for a shop that consists of mostly operators, rather than machinists, I think the short macro will be most useful... or perhaps operator messages in the program that identify restart lines *shrugs*

I’m surprised, however, that there is no parameter options for this… it seems rather dubious to give an alarm for calling a tool that is already where it is supposed to be, lol. I suppose its the older machine... back when there were still more machinists than operators, lol.

Anyway… thank again!

[broby]

Thanks guys…
Since I program for a shop that consists of mostly operators, rather than machinists, I think the short macro will be most useful... or perhaps operator messages in the program that identify restart lines *shrugs*

I’m surprised, however, that there is no parameter options for this… it seems rather dubious to give an alarm for calling a tool that is already where it is supposed to be, lol. I suppose its the older machine... back when there were still more machinists than operators, lol.

Anyway… thank again!

Not confined to "Older" machines... same for all machines.

[Superman]

Has anyone mentioned about creating a "User M or G code" and a library file ?

ie
create a macro - similar to budgieW's suggestion and assigning it to an M-code
that new M-code is used to replace the M06, the macro would decide what is in the spindle, look at what is to come in, or to be put away- the macro does actually use the M06 in it's operation
It works similar to associating a macro to a code, and calling it up like a sub-routine. But instead of a CALL statement it is an M or G code that runs it.

The .LIB library file and user M-code macro would need to be set on all machines that would use this new code

[budgieW]

Save this to a LIB file

OTCK (G116 GET NOMINATED TOOL)
IF [PT EQ EMPTY] NERR
IF [PT EQ VTLCN] NEND
IF [PT EQ VNTOL] NM6
IF [VNTOL EQ 0] NCT
M64
NCT T=PT
NM6 M6
NEND G56 H=PT D=PT
GOTO NRTS
NERR M63
M6
NRTS RTS

Then assign OTCK to G116 in the custom G and M codes

Then program
G116 T1

If T1 is in the spindle the program will carry on. If T1 is not in the spindle then the machine will go and get it

[Algirdas]

... T=PT
...
G56 H=PT D=PT
Just curious, what specification OSP will understand that? Is it enough "User task 2"?

[broby]

... T=PT
...
G56 H=PT D=PT
Just curious, what specification OSP will understand that? Is it enough "User task 2"?

Well mr Al... If you know anything about programming Okumas, you would know that is the correct way of referencing letter arguments from within a macro. The preceding 'P' on the variable 'PT' tells the code that you are referring to the 'T' code on the G code call statement line.

I am still left wondering if the original problem is with incorrect programming or operators who do not know how to do restarts correctly?
If it a programming issue... See above example... If it a restarting issue, then either better program documentation is required or operator training is required.

[budgieW]

There are many ways to do this, Below are 2 options

1, Use this format and retstart at N1

G00 G17 G21 G40 G80 G90
G30 P32
IF [VTLCN EQ 7] N1 (SPINDLE TOOL CHECK)
T7 (16MM TIPS - TOOL 7)
M6
N1 (SPINDLE TOOL JUMP)
S9500 M03
G15 H1
M11 (UNLOCK)
G00 G90 X49.866 Y1.065 A15. M15
M10 (LOCK)
G56 H=VTLCN Z100. M08
M510
G131 J2 E0.025 F20000 (HICUT PRO ROUGHING)
Z63.
G01 Z58. F1200.
X49.876 Z57.752

Or use this formatwith the below G116 macro and restart at N1, You will need to have custom G/M codes and user task 2 options

G00 G17 G21 G40 G80 G90
G30 P32
N1 G116 T4 (6MM BALLNOSE SHORT)
S8500 M03
G15 H1
G00 G90 X-74.277 Y62.083
G56 H=VTLCN Z25. M12
G131 J2 E0.01 F10000 (HI CUT PRO ON)
G01 Z4.9 F10000.
X-74.278 Z4.837 F2250.
X-74.281 Y62.084 Z4.775

[deadlykitten]

hello budgie i know that this thread is from 2011ad, but i recently started using Hi-Cut Pro, and i was searching for such threads

please, about this code :

    G131 J2 E0.01 F10000
    G01                  Z4.9   F10000
        X-74.278         Z4.837 F2250
        X-74.281 Y62.084 Z4.775

are those coordinates for a 3D toolpath ?

it seems that HiCut_feed_upper_limit is the same with the feed for "rapid" approach ( 10k ), and after that the toolpath is cut at 2250; the cnc may struggle a bit to target 0.01 precision at 10000mm/min ... i would try this :

    G01                  Z4.9   F10000
    G131 J2 E0.01 F2250*1.2            (*)
        X-74.278         Z4.837 F2250
        X-74.281 Y62.084 Z4.775

(*)
(   upper_feed_limit a bit bigger than programmed value, but not too big, so to avoid machining at "exact" feed value )
(   i don't know if using HiCut_feed_upper_limit = 10000 has same effect like = 2250*1.20, but i know that using )
(HiCut_feed_upper_limit = programed_feed_value will lead to force feed corrections, because during machining the feed )
(may go over 2250 )
(   feed oscilations around programmed feed value is a normal thing, and the feed corection should not be )
(forced also by the HiCut function )

or this :

    G131 J2 E1 F10000         (*1)
    G00                  Z4.9 (*2)
    G01 X-74.278         Z4.837 F2250
        X-74.281 Y62.084 Z4.775

(*1)
(   machining tolerance will always be below 1, because encoders cinematic is pretty sharp; this will )
(allow the machine to move more "freely&smooth", especially when the toolpaths segments are tangent, or )
(close to being tangent )
(   E0.01 will output a greater accuracy near toolpath joints and machining time will be bigger )
(   still, E1 will perform faster and may deliver a nice result )

(*2)
(   Hi-Cut is disabled during rapids )

kindly

[Superman]

WTF are you doing kitty ?

This thread is about a tool change error. ....
....NOT tolerance control

.................go and start another thread and talk with yourself there

[deadlykitten]

hy super / i could bet that you would be the 1st ( & maybe the only one ) to reply

i know what this thread is about, but i was simply looking for code samples about Hi-Cut Pro, because i just started using it, and i needed to see other approaches

you can not dodge bullets if you are predictable ! you need a zig-zag random fly; use HiCut when going left



also, back in 2011, why didn't you asked budgiew about sharing a Hi-Cut code inside a tool-changer thread ?

[Superman]

also, back in 2011, why didn't you asked budgiew about sharing a Hi-Cut code inside a tool-changer thread ?

The same reason I didn't query his use of G15 or any other code in his post...... it is there to show context with the thread topic ( a tool change / machine usage error )
- plus he didn't give any reference to anything other than showing the G/M macro usage to bypass the thread topic error

[deadlykitten]

if you are bulletproof, you don't even have to dodge ...

is it possible to fly on the back, and watch the sky ? or, like the sharks, if you turn 180, you fall asleep ?

if you stay upside down while levitating, do you feel the blood rushing to your head ? gravity affects you ?

[kurmay]

S u p e r m a n
u 1 1 1 1 0 0 0
p 1 1 1 1 0 0 0
e 1 1 1 1 0 0 0
r 1 1 1 1 0 0 0
m 0 0 0 0 0 0 0
a 0 0 0 0 0 0 0
n 0 0 0 0 0 0 0

[deadlykitten]

Antarctica's inhabitants !!!

[kurmay]

I think the superman has blown here, it is too cold.

[deadlykitten]

i heard rumors about a story with chuck norris and superman ... and superman won !!!

youtube.com/watch?v=hZ7a-jwBuq4