CNCzone.com-The Largest Machinist Community on the net!



Home Page Mark Forums Read Today's Posts My Replies Classifieds Reviews Photo Gallery Web Links Share Files Advertise With Us Ad List
Go Back   CNCzone.com-The Largest Machinist Community on the net! > Machine Controllers Software and Solutions > Fanuc


Fanuc Discuss Fanuc controllers here!


This forum is sponsored by:

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #1   Ban this user!
Old 01-28-2011, 04:12 PM
 
Join Date: Feb 2010
Location: USA
Age: 40
Posts: 39
mark029 is on a distinguished road
alarm

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.
Reply With Quote

  #2   Ban this user!
Old 01-28-2011, 04:22 PM
 
Join Date: Jun 2010
Location: USA
Posts: 158
cnc2149 is on a distinguished road

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).
Reply With Quote

  #3   Ban this user!
Old 01-28-2011, 04:33 PM
 
Join Date: Feb 2010
Location: USA
Age: 40
Posts: 39
mark029 is on a distinguished road

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.
Reply With Quote

  #4   Ban this user!
Old 01-28-2011, 04:35 PM
 
Join Date: Jun 2010
Location: USA
Posts: 158
cnc2149 is on a distinguished road

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.
Reply With Quote

  #5   Ban this user!
Old 01-28-2011, 05:26 PM
 
Join Date: Feb 2010
Location: USA
Age: 40
Posts: 39
mark029 is on a distinguished road

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.
Reply With Quote

Sponsored Links
  #6   Ban this user!
Old 01-29-2011, 07:53 AM
 
Join Date: Feb 2010
Location: USA
Age: 40
Posts: 39
mark029 is on a distinguished road

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?
Reply With Quote

  #7   Ban this user!
Old 01-29-2011, 09:19 AM
 
Join Date: Jun 2008
Location: United States
Posts: 1,507
stevo1 is on a distinguished road

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
Reply With Quote

  #8   Ban this user!
Old 01-29-2011, 11:46 AM
 
Join Date: Feb 2010
Location: USA
Age: 40
Posts: 39
mark029 is on a distinguished road

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.
Reply With Quote

  #9   Ban this user!
Old 01-29-2011, 12:01 PM
 
Join Date: Jun 2008
Location: United States
Posts: 1,507
stevo1 is on a distinguished road

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
Reply With Quote

  #10   Ban this user!
Old 01-29-2011, 12:29 PM
 
Join Date: Feb 2010
Location: USA
Age: 40
Posts: 39
mark029 is on a distinguished road

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?
Reply With Quote

Sponsored Links
  #11   Ban this user!
Old 01-30-2011, 02:18 AM
 
Join Date: Sep 2010
Location: Australia
Posts: 733
angelw is on a distinguished road

Originally Posted by mark029 View Post
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,
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
Reply With Quote

  #12   Ban this user!
Old 01-30-2011, 08:30 AM
 
Join Date: Feb 2010
Location: USA
Age: 40
Posts: 39
mark029 is on a distinguished road

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.
Reply With Quote

Reply




Currently Active Users Viewing This Thread: 1 (0 members and 1 guests)
 
Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
NEED HEELP ALARM #414 Y AXIS SERVO ALARM? PICMAN Fanuc 6 04-29-2011 05:20 PM
Need Help!- 750 ALARM SPINDLE-1 ALARM DETECT (AL11) PICMAN Fanuc 9 03-27-2011 06:14 PM
Problem- (ALARM 414 SERVO ALARM) Y-AXIS DETECT ERROR? PICMAN Fanuc 8 01-19-2011 01:10 PM
ALARM shuttle drawbar alarm haas timmydabull Haas Mills 27 10-30-2009 08:27 PM
Need Help!- DAEWOO 8 Steady rest pressure alarm, External feed hold alarm doubleeagle Daewoo/Doosan 4 06-12-2009 03:15 PM




All times are GMT -5. The time now is 01:02 PM.





Powered by vBulletin® Version 3.8.7
Copyright ©2000 - 2012, vBulletin Solutions, Inc.
Content Relevant URLs by vBSEO
Template-Modifications by TMS

1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 17 18 19 20 21 22 23 24 25 26 27 28 29 30 31 32 33 34 35 36 37 38 39 40 41 42 43 44 45 46 47 48 49 50 51 52 53 54 55 56 57 58 59 60 61 62 63 64 65 66 67 68 69 70 71 72 73 74 75 76 77 78 79 80 81 82 83 84 85 86 87 88 89 90 91 92 93 94 95 96 97 98 99 100 101 102 103 104 105 106 107 108 109 110 111 112 113 114 115 116 117 118 119 120 121 122 123 124 125 126 127 128 129 130 131 132 133 134 135 136 137 138 139 140 141 142 143 144 145 146 147 148 149 150 151 152 153 154 155 156 157 158 159 160 161 162 163 164 165 166 167 168 169 170 171 172 173 174 175 176 177 178 179 180 181 182 183 184 185 186 187 188 189 190 191 192 193 194 195 196 197 198 199 200 201 202 203 204 205 206 207 208 209 210 211 212 213 214 215 216 217 218 219 220 221 222 223 224 225 226 227 228 229 230 231 232 233 234 235 236 237 238 239 240 241 242 243 244 245 246 247 248 249 250 251 252 253 254 255 256 257 258 259 260 261 262 263 264 265 266 267 268 269 270 271 272 273 274 275 276 277 278 279 280 281 282 283 284 285 286 287 288 289 290 291 292 293 294 295 296 297 298 299 300 301 302 303 304 305 306 307 308 309 310 311 312 313 314 315 316 317 318 319 320 321 322 323 324 325 326 327 328 329 330 331 332 333 334 335 336 337 338 339 340 341 342 343 344 345 346 347 348 349 350 351 352 353 354 355 356 357 358 359 360 361