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 12-20-2005, 09:20 AM
 
Join Date: Dec 2005
Location: canada
Posts: 7
jianjianca is on a distinguished road
change offset in program

quick question, a job about making 5 parts from a stock material.
program as

p001
p001
p001 (need to change tool #3 offset here)
p001
p001

change tool # 3 offset back to zero.

anybody can tell me how to change the program or make a simple marco to change the offset automatically, thanks.

it s easy to get mistake when do it manually
Reply With Quote

  #2   Ban this user!
Old 12-20-2005, 10:15 AM
 
Join Date: Jul 2005
Location: Canada
Posts: 11,563
Geof will become famous soon enough

Which offset do you want to change; length or diameter? G10 is the code for entering offsets from a program.

For example:

G10 L12 G90 P3 R0.5 will enter a tool diameter offset of 0.5 or any other value you put for R.

G10 L10 G90 P3 R5.0 will enter a tool length offset of 5.0 or any other value you put for R.

Some words of caution: Using a G10 command to change your tool length offset can be very, very risky. If you make a typo you may finish up putting the tool much further down than you intended.
Reply With Quote

  #3   Ban this user!
Old 12-20-2005, 10:26 AM
 
Join Date: Dec 2005
Location: canada
Posts: 7
jianjianca is on a distinguished road

does g10 work for lathe machine also? how can i check if the tool length changed or not while the program runing. thanks a lot
Reply With Quote

  #4   Ban this user!
Old 12-20-2005, 10:44 AM
 
Join Date: Jul 2005
Location: Canada
Posts: 11,563
Geof will become famous soon enough

Yes G10 works on the lathe. Are you trying to take a length of stock in the chuck and machine and part-off 5 complete pieces? You can do this but the easiest way is to change work zeroes not tool offsets.
Reply With Quote

  #5   Ban this user!
Old 12-20-2005, 04:32 PM
 
Join Date: Sep 2005
Location: canada
Posts: 26
bob in windsor is on a distinguished road

Try finding the system variable number for tool offsets on your control.For example on Fanuc 16m insert #2013=0 where you need it changed.Do it on a test run above the part first and check your offset table after it reads that line.
Reply With Quote

Sponsored Links
  #6   Ban this user!
Old 12-20-2005, 10:27 PM
 
Join Date: Dec 2005
Location: canada
Posts: 7
jianjianca is on a distinguished road

Originally Posted by Geof
Yes G10 works on the lathe. Are you trying to take a length of stock in the chuck and machine and part-off 5 complete pieces? You can do this but the easiest way is to change work zeroes not tool offsets.
sorry, it s radius offset. i dont know why they change it. anyway , it s according to the real situation.

and thanks to bob, i will try to figure out the var and the address, but seems making the problem more complicated.
Reply With Quote

  #7   Ban this user!
Old 12-21-2005, 11:16 AM
 
Join Date: Dec 2005
Location: canada
Posts: 7
jianjianca is on a distinguished road

to geof, if i wanna use g11 to cancel the offset, do i need to add any parameter on it? thx
Reply With Quote

  #8   Ban this user!
Old 12-21-2005, 12:44 PM
 
Join Date: Jul 2005
Location: Canada
Posts: 11,563
Geof will become famous soon enough

Originally Posted by jianjianca
to geof, if i wanna use g11 to cancel the offset, do i need to add any parameter on it? thx
I don't completely understand this question. G10 is the code for setting offsets; in other words entering values into the offset tables. When you talk about cancelling that is related to using the offset value that is in the table.

These examples are for a Haas control running in Fanuc mode, the principles should be the same for most controls.

For example G10 L10 G90 P3 R0.03 will enter the value of 0.03 in the tool nose radius column for tool 3.

In a program you use this value when you have a tool compensation command G41 D03 or G42 D03 and you cancel the tool compensation using G40.

Similarly G10 L10 G90 P3 X-5.0 Z-5.0 will enter these values in the X and Z columns in the offset tables and when you do a tool command T303 these values will be used for the tool offset.

In fanuc I do not know how to cancel the tool offset but you can set the X and Z values back to zero using G10 L10 G90 P3 X0. Z0.
Reply With Quote

  #9   Ban this user!
Old 12-21-2005, 12:58 PM
 
Join Date: Dec 2005
Location: canada
Posts: 7
jianjianca is on a distinguished road

to Geof, yes, u r right, i can set it back to zero. i just checked the G Code table, G10 is to set tool offset( u already show me how to use it), and G11 is to cancel tool offset( i want to know the detail). got another problem, i found another explain for G10 code is to set the origin.
Reply With Quote

  #10   Ban this user!
Old 12-21-2005, 01:54 PM
 
Join Date: Jul 2005
Location: Canada
Posts: 11,563
Geof will become famous soon enough

I cannot help you with G11 because it is not used on the Haas.

G10 can be used to set a lot of things including the origin, G54, G55 etc. It depends on the L value and P value. You should be able to find these somewhere in your explanation.
Reply With Quote

Sponsored Links
  #11   Ban this user!
Old 12-22-2005, 12:44 AM
 
Join Date: Dec 2005
Location: canada
Posts: 7
jianjianca is on a distinguished road

To Geof, thx alot again, i tried g11 on misubishi, it didnt work, and G10 L12 too. when i use G10 L10 G90 P10 x1. ; the tool data changed , but not the tool offset. can u tell me where i can find a table for those detail parameters.
Reply With Quote

  #12   Ban this user!
Old 12-22-2005, 10:48 AM
 
Join Date: Jul 2005
Location: Canada
Posts: 11,563
Geof will become famous soon enough

I don't know where to find any online references. Here is information taken from one of my machine manuals.

L selects geometry, wear, shift or work coordinates, with a P choosing the actual entry.

L1 is wear, P1 is tool 1, P2 tool 2, etc.

L2 is work coordinate, P2 is G54, P3 is G55, etc.

L 10 is geometry, P1 tool 1, etc

The actual values are identified by X, Y, for work coordinates (L2), R, for geometry or wear.

The best way to sort it out is as you are doing testing things on a machine and finding what is entered.
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





All times are GMT -5. The time now is 08:05 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