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! > CAM Software > EdgeCam


EdgeCam Discuss EdgeCam software here.


This forum is sponsored by:

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #1   Ban this user!
Old 01-11-2011, 06:52 AM
 
Join Date: Jun 2010
Location: Sweden
Age: 38
Posts: 54
tummen is on a distinguished road
Speed change

Im using Heidenhain TNC in my mashine and to change the S parameter i need to output:
123 TOOL CALL 1 Z S2000
at the normal toolchange
or later a
456 TOOL CALL S3000
line when the speed changes.
my problem is that if i change the speed between different instructions but still using the same tool I don“t get a new tool call
I think in ISO you just add Sxxxx on a normal line and you are done.
I guess there are two solutions.
one is to force a toolchange at every speed change
and one is to check if speed is not = old speed and then output my new speed value.
Does anyone have a solution or atleast a hint to offer?

Last edited by tummen; 01-11-2011 at 06:54 AM. Reason: spelling
Reply With Quote

  #2   Ban this user!
Old 01-12-2011, 07:30 AM
 
Join Date: Oct 2009
Location: USA
Posts: 33
jsanders is on a distinguished road

You're 2nd idea is the way to go, a check on logic to see if the speed is changed. Keep in mind that "negative logic" works best here. The layout is below. Refer to the Code Wizard help or *.MXT source code for the variable names and syntax. You may also need to create a variable to hold the old speed value.
%If NEWSPEED = OLDSPEED @NO_SPEED_CHANGE
CNC code output "456 TOOL CALL S3000" goes here
@NO_SPEED_CHANGE
Reply With Quote

  #3   Ban this user!
Old 01-12-2011, 01:05 PM
 
Join Date: Jun 2010
Location: Sweden
Age: 38
Posts: 54
tummen is on a distinguished road

All values that are used in code wizzard has a flag if they should be skipped if they did not change. there must be some value behind every value that it checks against.
Anyone seen how to reach for this old value?
i can in this case save the old speed for later but since edgecam can deside in every output if it is needed (modal) then maybe i could do the same?
Reply With Quote

  #4   Ban this user!
Old 01-13-2011, 06:18 AM
 
Join Date: Oct 2009
Location: USA
Posts: 33
jsanders is on a distinguished road

Save the old speed. That is the only way you have to determine if the value is changed.
Reply With Quote

  #5   Ban this user!
Old 01-16-2011, 05:25 PM
 
Join Date: Jun 2010
Location: Sweden
Age: 38
Posts: 54
tummen is on a distinguished road
My Solution

After reading the intermediate file from compiling of the post i found that almost all vars have a xxxHOLD that holds xxx“s old value
the code below was therefore my attempt.

;CODE:%IF #SPEED=#SPEEDHOLD @SKIP1
[DELETE][BLKNUM] TOOL CALL S[<C>SPEED]
;CODE:@SKIP1

but i did not need it in the end i found a reference to another variable that i then traced to misc funktions, outpuut speed change on separat row.
this solved my problem.
Reply With Quote

Sponsored Links
Reply

Tags
code wizard, heidenhain tnc 426, speed, tool call




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
Build Thread- Super-PID speed controller installation to Fixed speed Router Khalid DIY-CNC Router Table Machines 14 11-13-2010 04:29 AM
Need Help!- Rebild low speed Mazak VQC 20/40B Mazatrol M-2 to 10000/RPM hight speed sve0019 Mazak, Mitsubishi, Mazatrol 0 08-07-2010 12:41 PM
Need Help!- Fanuc O-TD-controlled lathe machine at low speed and fixed speed problem. bursa017 Fanuc 0 06-11-2010 01:59 AM
Cutting speed locked to Z torch height control speed Beefy Mach Plasma / Laser 1 02-14-2010 05:14 PM
BPSeriesI / Centroid control- Spindle speed all out of whack with speed dial? peter.blais Bridgeport and Hardinge Mills 9 08-08-2006 03:29 AM




All times are GMT -5. The time now is 01:31 AM.





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