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 > G-Code Programing


G-Code Programing Discuss G-code programing and problems here!


This forum is sponsored by:

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #1   Ban this user!
Old 10-30-2007, 10:04 PM
 
Join Date: Jan 2005
Location: USA
Posts: 49
DocHod is on a distinguished road
G91 B axis move?

Hi all can anyone give me a reason why I would get a improper G code alarm when all I want to do is move the B axis away from the part after it is cutoff in a G91 move I have the sample blocks of the program below any help I would be grateful , this is a Fanuc 18i controller on a Doosan 2500 lsy.
O7000
N100G0G90G40G80
G28U0.V0.
M1
N900(CUTTOFF)
M131(interlock by-pass sub spin.)
M110(close tooling by-pass)
M169T0200
G0X1.762Z0.T0202B-27.5
G4U100
G98
G1B-29.0F150.
G96S600M4
M204
M168
G99
G1X1.43F.003
G0X1.602
Z.06
G1X1.563
G3X1.438Z0.R.0625
G0X1.602
Z-.06
G1X1.563
G2X1.438Z0.R.0625
G1X-.03
G91B.02(RETRACT SUBSPIN .02 BEFORE X AXIS MOVES UP. improper G code alarm )
G0G90X8.0
M205
G28B0.
Z10.M9
G80
M30
Reply With Quote

  #2   Ban this user!
Old 10-30-2007, 11:24 PM
dcoupar's Avatar  
Join Date: Mar 2003
Location: USA
Posts: 2,312
dcoupar is on a distinguished road

As far as I know, there is no incremental command for B on the 2500SY. (X=U, Z=W, C=H, etc.), but there is no incremental B. You might consider using macro variables, instead of hard coded dimensions, i.e.:

in #504, put -29.0
in #505, put -28.98

O7000
N100G0G90G40G80
G28U0.V0.
M1
N900(CUTTOFF)
M131(interlock by-pass sub spin.)
M110(close tooling by-pass)
M169T0200
G0X1.762Z0.T0202B-27.5
G4U100
G98

G1B#504F150.

G96S600M4
M204
M168
G99
G1X1.43F.003
G0X1.602
Z.06
G1X1.563
G3X1.438Z0.R.0625
G0X1.602
Z-.06
G1X1.563
G2X1.438Z0.R.0625
G1X-.03

B#505(RETRACT SUBSPIN .02 BEFORE X AXIS MOVES UP. improper G code alarm )

G0G90X8.0
M205
G28B0.
Z10.M9
G80
M30
Reply With Quote

  #3   Ban this user!
Old 10-31-2007, 07:23 AM
 
Join Date: May 2007
Location: Denmark
Posts: 50
Kai_DK is on a distinguished road

Using a MS SL150smc I can confirm that there's no incremental axis for B.
I use G0G53Bxx to be sure where my sub-spindle is locateted, no matter which datum thats currently active.
Reply With Quote

  #4   Ban this user!
Old 10-31-2007, 12:13 PM
cnc-king's Avatar  
Join Date: Jul 2003
Location: united states
Posts: 232
cnc-king is on a distinguished road

the lathes do not use g91 for incremental moves

X = U
Z = W
Y = V
C = H
A = A
B = B

a xis for the mill mode on the subspindle and b for the subspindle
i usually command G53B0 after part off then move the x out of the way
the x will move even if the b is still moving
__________________
If you can ENVISION it I can make it
Reply With Quote

  #5   Ban this user!
Old 11-01-2007, 08:43 PM
 
Join Date: Jan 2005
Location: USA
Posts: 49
DocHod is on a distinguished road

I find it to be strange that Doosan would choose to not be able to move the B axis (sub spindle) in a G91 incremntal move when other machine builders do use the G91 move for the subspindle , we have a Viper VT 23 lathe that I can do a G91 move on the sub spindle . I will take your advice when I talk to the service people that we bought the machine from to make sure this is totaly true , thanks for your input.
Reply With Quote

Sponsored Links
  #6   Ban this user!
Old 11-01-2007, 11:56 PM
dcoupar's Avatar  
Join Date: Mar 2003
Location: USA
Posts: 2,312
dcoupar is on a distinguished road

Your Viper is probably set to use G-Code System B or C, which switch between absolute and incremental coordinates with G-codes (G90/G91). Doosan uses G-Code System A, which uses address characters to switch between absolute/incremental (X/U Z/W C/H) but Fanuc (not Doosan) doesn't provide an incremental address for B. System A allows mixed absolute/incremental commands within a block, i.e. X & W, or U & Z... System B & C do not.
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
What method did you use to move the x-y-z axis? widgitmaster Polls 4 01-07-2008 01:35 AM
How do you move an axis manually ? Eurisko DIY-CNC Router Table Machines 6 04-06-2007 09:00 PM
Axis move during feed hold 1ctoolfool Haas Mills 3 09-12-2006 10:12 AM
Mach 1 x-axis will not move Redline Mach Software (ArtSoft software) 3 07-05-2005 12:01 AM
Speed how fast an axis can move? jlagran he General CNC (Mill and Lathe) Control Software (NC) 0 01-04-2005 10:05 PM




All times are GMT -5. The time now is 10:04 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