PDA

View Full Version : Need Help! MC-4VAE/OSP5020M - Alarm B 539



LancoUSA
02-01-2008, 04:49 PM
Starting up our old Okuma, using Mastercam X2 to generate code. When trying out a new program that only uses one tool, machine runs great all the way through to the end. Upon restarting machine to run again I am getting an Alarm B, 539 Wrong T command – Code 1, which indicates: The T number same as active tool number is specified.

The problem is that now the Active tool is tool 1, which now remains in the spindle. There is no need to change, as there are no other tools required.

I have to go back into manual mode and send the tool back to the carousel before going in Auto to run again.

The program starts and ends like this:

(Beginning)
$01.MIN%
G15 H0
T1 M6
G0 G90 X-3.907 Y-31.306 S22500 M3
G56 Z3. H1
G1 Z-.2 F25
< Body of the program, everything working fine>
(End)
G0 Z1.
Z3.
M2
%

Is there a way to cancel the Active tool 1 at the end of program so it can be run again when pressing Cycle Start? Right now when hitting again results in the Alarm as noted above.

Thanks for any input! I hope to get this old beast up and running again.

bizdad
02-02-2008, 05:52 AM
well,...

it seems that the origional 5020 controll gave a M63 command
this means: tools change, with empty spindle return.

yhis can be removed by a M64 command

regards from the Netherland (europe)

Billmac
02-04-2008, 09:55 AM
On the 5000 control, you have press the "BLOCK SKIP 1" button and in the T1 M6 line of the program add a slash and it should look like this:

/T1 M6

The machine will skip that block and you should not get an error.

slavetothemetal
02-04-2008, 01:58 PM
On the safer side, replace T1 M6 with these lines,
IF[VTLCN EQ 1]GOTO N1
IF[VTLNN EQ 1]GOTO N2
T1M6
GOTO N1
N2 M6
N1(START OF FILE)
This way, if the tool has been called or is in the spindle, no alarms.

broby
02-05-2008, 07:42 AM
Also if you use tool offsets HA for the tool length and DA for Cutter Rad Comp, the machine will then make sure it is using the "Active" tools first offset information.
To use the second or third offsets on the tool use HB/DB and HC/DC
Much easier to use when manually editing any information. This way if you change tool numbers you do not have to search and replace all the instances of T1 H1 D1 for example.
This, combined with Slaves suggestions should get you around your problem.
Cheers
Brian.