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 09-07-2007, 02:20 PM
 
Join Date: Mar 2007
Location: USA
Posts: 207
John3 is on a distinguished road
5T G28 U0 one sided

Hi,

Does anybody know if this behavior can be corrected or if its "normal" for a Fanuc 5T:

I put a G28 U0 in a new program expecting it to HOME (Machine Zero) the cross feed (X-axis). My machine has front and rear turrets, the carriage has zero in the center and has +8.0 and -8.0 inches of travel.

When in the negative X range the G28 U0 worked as expected, the X-axis traveled positive to the Machine Zero Position and stopped with the X Zero Return Lamp on. When already in the positive X range, the carriage just takes off to the Positive limit and the machine goes into an Alarm.

Is there a prameter that affects this, or some programming trick or another command that will let me send the X-axis to machine zero, no matter where it is currently positioned?

Thanks for any comments,

John
Reply With Quote

  #2   Ban this user!
Old 09-07-2007, 07:32 PM
 
Join Date: Sep 2005
Location: USA
Age: 60
Posts: 755
Dan Fritz is on a distinguished road

The G28 U0 command should zero out the X axis just fine, but the DIRECTION of zero return is fixed with a parameter setting. If the zero-return switch is in the center (instead of at the extreme X+ limit), the you must be on the X+ side of the switch if you zero-return. Otherwise, it will just move in the +X direction and (not) hit the switch, then overtravel.

If you are on the X- side of zero and give it a G28 U0, does it stop in the middle, or does it go to near the +X limit and stop at zero?
If it stops in the middle, then you're already PAST the switch when you're on the X+ side of center.
Reply With Quote

  #3   Ban this user!
Old 09-07-2007, 08:29 PM
 
Join Date: Mar 2007
Location: USA
Posts: 207
John3 is on a distinguished road
Another Command?

Originally Posted by Dan Fritz View Post
The G28 U0 command should zero out the X axis just fine, but the DIRECTION of zero return is fixed with a parameter setting....
Are there any other commands available on a 5T that will cause the X-axis to travel directly to Machine Zero, from either + or - direction. (I don't need an intermediate point). What about G27 perhaps? (I surely don't understand it, even after reading Fanuc's Japenglish Manual)

John
Reply With Quote

  #4   Ban this user!
Old 09-07-2007, 09:27 PM
 
Join Date: Sep 2005
Location: USA
Age: 60
Posts: 755
Dan Fritz is on a distinguished road

You can use the intermediate point with G28 to go to an absolute position of a positive number, then zero-return. For example:

G28 X10000

This will move to an absolute position of X10000 (one inch) then zero return.
Reply With Quote

  #5   Ban this user!
Old 09-07-2007, 09:51 PM
 
Join Date: Mar 2007
Location: USA
Posts: 207
John3 is on a distinguished road

Originally Posted by Dan Fritz View Post
You can use the intermediate point with G28 to go to an absolute position of a positive number, then zero-return. For example:

G28 X10000

This will move to an absolute position of X10000 (one inch) then zero return.
Dan, as always, thanks for your quick and helpful answers.

Is that X=+1.000 inches in machine coordinates or X=+1.000 inches in current G50 coordinates?

John
Reply With Quote

Sponsored Links
  #6   Ban this user!
Old 09-07-2007, 10:00 PM
 
Join Date: Sep 2005
Location: USA
Age: 60
Posts: 755
Dan Fritz is on a distinguished road

If you use X with a G28, it moves to the absolute position (as defined by the G50 statement), then it zero-returns. If you use U with G28, it makes an INCREMENTAL move of the U amount, then it zero-returns. G28 U0 always goes straight home. G28 U-10000 will move minus one inch from where it is, then zero-return. G28 X-10000 will move to X minus 1 inch (which might be quite some distance), the it will zero-return.
Reply With Quote

  #7   Ban this user!
Old 12-11-2008, 10:59 PM
 
Join Date: Dec 2008
Location: usa
Age: 63
Posts: 22
Paul Pippenger is on a distinguished road
G28

The U value tells the slide to move to a point first,,,, then zero out
you can do z+ some amount,,then command G28 u minus some amount to always get the slide on the correct side of the switch before it zero returns.
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
Can MeshCAM do 4 or more sided milling? digits GRZ Software- MeshCAM 5 04-03-2008 05:14 PM
4 sided part cncuser1 Mastercam 12 05-01-2007 04:47 PM
2 Sided Part ? JMFabrications Mastercam 40 04-24-2007 08:21 PM
Double Sided Tape? Really? wildcat General Metalwork Discussion 4 12-03-2006 10:47 AM
double sided job setups july_favre General Metal Working Machines 2 06-14-2004 10:27 AM




All times are GMT -5. The time now is 07:37 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