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 09-18-2009, 03:07 PM
 
Join Date: Apr 2009
Location: Sweden
Posts: 25
driftmaster is on a distinguished road
Fanuc tool lenght compensation??

Hello.

Machine is mori seiki sh 5000 with fanuc MSG 501.
Here's the deal, i wonder if this is possible...

Machine running 4 different jobs, some with same tools, different people programming of course.
In some of the programs lets say tool T23 needs tool lenght (H) added with 0.10 (mm) in next job it needs to be -0.10..and so on..( meaby in third job it needs to be 0.15...)
Needles to say, much hassle.

Ofcourse im aware i could have several H codes, but that could cause problems later on when running the program again.

So is there any extra code that could be used just in program that could give you possibility to alter the tool lenght?
Reply With Quote

  #2   Ban this user!
Old 09-18-2009, 03:42 PM
 
Join Date: Nov 2006
Location: UK
Posts: 121
ChattaMan is on a distinguished road

I've no idea what a Fanuc MSG 501 control is but on the controls I use, I would adjust the different tool lengths with the wear offset.

In the prog use G10.

In prog one...
G10 L11 P23 R0.1

In next prog...
G10 L11 P23 R-0.1

In next prog...
G10 L11 P23 R0.15

G10 = parameter setting
L11 = wear offset (on newer control use L13)
P23 = corresponding offset number
R0.1 = amount of wear adjustment.
Reply With Quote

  #3   Ban this user!
Old 09-18-2009, 03:42 PM
beege's Avatar  
Join Date: Feb 2008
Location: USA
Posts: 518
beege is on a distinguished road

Used to be G45, G46, G47 and G48 would increase/decrease moves by an offset amount. Don't recall if it was usable in G41 or G42, though.

G45 - single increase
G46 - single decrease
G47 - double increase
G48 - double decrease

These were used in place of cutter compensation a long time ago.
Reply With Quote

  #4   Ban this user!
Old 09-19-2009, 12:51 AM
 
Join Date: Feb 2006
Location: United States
Posts: 273
dpuch is on a distinguished road

If you have custom macro A or B check your manual for macro variables in the 2000-3999 range, or 10001-19999 range. These allow just setting #2123=-0.1

This is the same as ChattaMan described, just a different way to code it.
Reply With Quote

  #5   Ban this user!
Old 09-19-2009, 02:22 AM
dcoupar's Avatar  
Join Date: Mar 2003
Location: USA
Posts: 2,312
dcoupar is on a distinguished road

Why not set the tools to a common standard and use the G54, G55, G56, etc. Z offset?
Reply With Quote

Sponsored Links
  #6   Ban this user!
Old 09-19-2009, 04:13 AM
 
Join Date: Apr 2009
Location: Sweden
Posts: 25
driftmaster is on a distinguished road

Originally Posted by ChattaMan View Post
I've no idea what a Fanuc MSG 501 control is but on the controls I use, I would adjust the different tool lengths with the wear offset.

In the prog use G10.

In prog one...
G10 L11 P23 R0.1

In next prog...
G10 L11 P23 R-0.1

In next prog...
G10 L11 P23 R0.15

G10 = parameter setting
L11 = wear offset (on newer control use L13)
P23 = corresponding offset number
R0.1 = amount of wear adjustment.
Hi.
Very good, exactly what i was looking for.
I will try this on monday and see if it works.

Thanks alot!
Reply With Quote

  #7   Ban this user!
Old 09-19-2009, 05:06 PM
 
Join Date: Apr 2009
Location: Sweden
Posts: 25
driftmaster is on a distinguished road

Originally Posted by driftmaster View Post
Hi.
Very good, exactly what i was looking for.
I will try this on monday and see if it works.

Thanks alot!
ChattaMan;

I'd like to ask one more thing.
The line with "G10 L11 P23 R0.1"
Where should i place this?

Lets say line like this after tool change.
"G43 Z10 H23"
Do i put the "G10 L11 P23 R0.1" before or after, or where should it be placed to work?
Reply With Quote

  #8   Ban this user!
Old 09-19-2009, 08:53 PM
beege's Avatar  
Join Date: Feb 2008
Location: USA
Posts: 518
beege is on a distinguished road

Oh and I believe if you use G91 with the G10 thing, you adjust incrementally, and G90 replaces the value absolutely.
Reply With Quote

  #9   Ban this user!
Old 09-21-2009, 12:46 PM
samu's Avatar  
Join Date: Feb 2007
Location: quebec
Posts: 216
samu is on a distinguished road

Originally Posted by driftmaster View Post
ChattaMan;

I'd like to ask one more thing.
The line with "G10 L11 P23 R0.1"
Where should i place this?

Lets say line like this after tool change.
"G43 Z10 H23"
Do i put the "G10 L11 P23 R0.1" before or after, or where should it be placed to work?
you need to put the line G10 L11 P23 R0.1 before calling tool length compensation(G43 Hxx)
Reply With Quote

  #10   Ban this user!
Old 09-21-2009, 12:53 PM
 
Join Date: Feb 2006
Location: United States
Posts: 273
dpuch is on a distinguished road

Originally Posted by samu View Post
you need to put the line G10 L11 P23 R0.1 before calling tool length compensation(G43 Hxx)
Yes before, But possibly you will need to inhibit the read ahead buffer as well. I think 4 lines are standard, and optionally it will read something like 15 lines.

Anyhow if you think it isn't working, look for a buffer inhibit G or M code in your manual and put that between the G10 line and the one with G43. It may be overly cautions for the G10, but definitely consider doing this if you use the Macro variable.
Reply With Quote

Sponsored Links
  #11   Ban this user!
Old 09-21-2009, 02:28 PM
 
Join Date: Mar 2005
Location: Silicon Valley, CA
Posts: 982
psychomill is on a distinguished road

As Coupar mentions and points to.... Why bother?

Machine running 4 different jobs, some with same tools, different people programming of course.
In some of the programs lets say tool T23 needs tool lenght (H) added with 0.10 (mm) in next job it needs to be -0.10..and so on..( meaby in third job it needs to be 0.15...)
Needles to say, much hassle.
Just set a tool length on the offset page and use work offsets (G54-G59) to control the zero point. No need to G10 anything....
__________________
It's just a part..... cutter still goes round and round....
Reply With Quote

  #12   Ban this user!
Old 09-21-2009, 03:07 PM
 
Join Date: Feb 2006
Location: United States
Posts: 273
dpuch is on a distinguished road

Originally Posted by psychomill View Post
As Coupar mentions and points to.... Why bother?

Just set a tool length on the offset page and use work offsets (G54-G59) to control the zero point. No need to G10 anything....
Not specific to this problem, but there are others that would solved via changing offset wear via code in the program.

It may be more than 1 tool per program, and not in the same direction and amount. Or radius offsets, differing cutting conditions could require different offsets between parts of features.

Another possibility is a rotary table. Fixture offsets often do not rotate with the part. So either offset the tool, or use several fixture offsets with translated axis values.
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
Fanuc 5T Tool Nose Compensation John3 Fanuc 1 07-15-2007 10:58 PM
tool lenght question jedioliver Visual Mill 7 09-22-2006 10:27 AM
Tool compensation bg_izio General CNC (Mill and Lathe) Control Software (NC) 3 05-03-2006 08:40 PM
Tool compensation bg_izio CamSoft Products 3 04-27-2006 10:43 AM




All times are GMT -5. The time now is 09:59 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