Whats a 504 alarm on a fanuc om? I'm working on my tool changer and getting this alarm. I loaded the program at the control panel by hand.
The 504 alarm is either a FANUC Hardware Overtravel or it is a Custom Macro generated alarm in one of your programs/macros. You didn't mention any text that was displayed but I suspect it is a macro message. You would have to look for a statement of #3000 = 4 (MESSAGE TEXT HERE) somewhere in the macro. This statement adds 500 to the numeric value in the right hand side and trips an alarm message and displays 504 (MESSAGE TEXT HERE).
At the bottom of the program there is a line that reads: N101#3000=4 (unit mode error). I'm new to all of this and am having time getting this going.
you may want to look in the machine builder's documentation since they probably included this message description in their tool change macro, etc. It is not a FANUC generated message so you won't see any reference in the FANUC manuals. 'Unit Mode' almost sounds like and inch/metric issue but that would be a guess.
I loaded this program today. When I bought this machine it had lost its settings. I had to reload all parameters and now I'm doing this. I'm wondering if I have the right program or not.
The book says it needs to use metric system (G21) before auto tool change. Do I need to insert a G21 into the program? If so, where do I put it?
Mark,
Post your tool change program so we can take a look at it. I suspect that cnc2149 is correct that you will probably find that it is an issue with inch/metric. Your program is probably using a condition with the #4006 variable to check and see what mode the machine is in.
It could very well be that the macro needs to switch to metric before doing a tool change. However I would not just do this without someone looking at your code first.
Stevo
Ok Stevo, here ya are. Well maybe it didn't load. Don't see it on here as a attchment. I'll send you one in a private message.
Ok I got the program via PM. Yes it appears the reason that you are getting the alarm is form the condition using #4006. Highlighted in red below is where the condition is and where it is going to and alarming out. It is odd that it needs to be in metric to do the tool change because I see no movements other then the G30 which it should not matter.
Anyhow you can do a few things. You can put another variable in the macro to capture what mode you are in G20 or G21. Then change it to G21 to do the tool change and switch back to the previous setting of G20. Now there are many things that I do not know like does your G20 and G21 call programs. If so that could be a problem.
Your other option is to see if you can run the program in inch mode and if so you can remove the condition that is alarming.
Ok Stevo, lets try it this way.
O9020
IF[#1000EQ1]GOTO102
M31T#20
G04X0.05
#145=0
#146=0
#147=0
IF[#1000EQ1]GOTO299
IF[#4006EQ20]GOTO101
IF[#20EQ0]GOTO100
IF[#20GE21]GOTO100
IF[#20EQ#0]GOTO100
#149=#4003
#148=#4001
G0G91G80G49M19
M66
WHILE[#1002EQ0]DO1
#146=#146+1.
IF[#146GE4.]GOTO99
G30Z0
END1
M41
M32
WHILE[#1003EQ0]DO1
#147=#147+1.
IF[#147GE4.]GOTO98
G28Z0
END1
T#20
WHILE[#1002EQ0]DO1
#145=#145+1.
IF[#145GE4.]GOTO99
G30Z0
END1
M33
G#148G#149
M42
GOTO299
N98#3000=1
N99#3000=2
N100#3000=3
N101#3000=4
N102#3000=5
N299M34
N300M99
Stevo
Stevo, all this sounds great. Problem is that I don't understand alot of this stuff yet. I understand the metric/inch issue but I'm not sure on how fix what you described to me. I understand you want to change the program to do a certain function and then change it back when thats completed. Just have no idea how to change it. Make sense?
Mark,Originally Posted by mark029
Take a look at parameters 0220 to 0229 to see if any of them are set to 20 or 21. These parameters hold the G code value that will be used to call a Macro program having a corresponding program number. As Steve stated, one of the unknowns is if G20 or G21 are being used to call other Macro programs. Clearly, they seem not to be used to do so in the listed program O9020, but there are a number of M codes in this program that may be calling nested Macro programs, and the G20/G21 Macro call could be used there. The only way of knowing is to execute the program in Single Block to see exactly what the logic of the Macro program does. Do do this, you have to set bit 5 of parameter 0011 to 1 for macro statements to execute and stop in Single Block.
If you don't find 20 or 21 in any of the parameters from 0220 to 0229 inclusive, you could expect that these G codes are not being used to call a Macro program, and your program could be modified to eliminate the error you currently experience when running it, as follows.
Regards,
Bill
O9020
IF[#1000EQ1]GOTO102
M31T#20
G04X0.05
#145=0
#146=0
#147=0
IF[#1000EQ1]GOTO299
IF[#4006EQ20]GOTO101 (DELETE THIS BLOCK)
IF[#20EQ0]GOTO100
IF[#20GE21]GOTO100
IF[#20EQ#0]GOTO100
#1=#4006 (INSERT TO CAPTURE THE CURRENT G20/G21 VALUE)
G21 (INSERT TO FORCE G21)
#149=#4003
#148=#4001
G0G91G80G49M19
M66
WHILE[#1002EQ0]DO1
#146=#146+1.
IF[#146GE4.]GOTO99
G30Z0
END1
M41
M32
WHILE[#1003EQ0]DO1
#147=#147+1.
IF[#147GE4.]GOTO98
G28Z0
END1
T#20
WHILE[#1002EQ0]DO1
#145=#145+1.
IF[#145GE4.]GOTO99
G30Z0
END1
M33
G#148G#149
M42
GOTO299
N98#3000=1
N99#3000=2
N100#3000=3
N101#3000=4 (DELETE THIS BLOCK BECAUSE A G20 CONDITION WILL NOT EXIST)
N102#3000=5
N299M34
G#1 (INSERT TO SET THE G20/G21 CONDITION AS IT WAS BEFORE CALLING THIS PROGRAM)
N300M99
Progress!!! It ran untill the magazine almost made it to the spindle and then it put up an alarm reading: 1004 mag LS31,LS32?. The magazine moves very slow for some reason. Even when I move it manually it moves slow. Also, the program stopped at M41. And when I turned the machine on I had a LS33 alarm. I indexed the magazine and that alarm went away. There wasn't a 20 or 21 in those parameters you mentioned. I also changed par. 11 to match what you recomended.
Posting Permissions
| | |
LinkBack URL
About LinkBacks
