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 > Mastercam


Mastercam Discuss Mastercam software here.


This forum is sponsored by:

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #1   Ban this user!
Old 02-18-2006, 11:37 AM
 
Join Date: Feb 2006
Location: UNITED STATES
Posts: 1
CNCZART is on a distinguished road
Angry Lathe Post Problems

I've Been Running Mcamx For About 4 Months Now And Most Problems Are Straghtened Out Except One.
When I Post My G71 Canned Cycle I Get No Depth Of Cut.
I'm Using A Converted V9 Post That I Had Tweaked Nicely For My Machines But I Lost The Depth Of Cut When Going To Mcamx
Any Help???
Reply With Quote

  #2   Ban this user!
Old 02-19-2006, 06:55 AM
 
Join Date: Jan 2005
Location: USA
Posts: 23
post_guy is on a distinguished road

Here's some information I received on updating lathe posts for X, sounds like exactly what you are encountering... hope it helps:

Important information for updating Lathe posts for X:

The order of positional information in the Lathe NCI lines has changed in X. In earlier versions we output Z X Y and mapped the coordinates in the post, now we output X Y Z (just like in Mill). This change means we have to modify every lathe post to remove the mapping. The update post utility will automagically fix the mapping issue if the logic matches that found in MPLFAN, MPLGEN or MPL_EZ. Here’s what gets changed:

Modifications for Mill Turn posts (X lathe NCI change)

Version 9 (current)

map_home : yes #Use home positions as entered or map to machine axis

pmatrix_su #Setup mapping matrix
hmtx1 = matt(m1)
if cuttype <> one, hmtx1 = mmul(hmtx1, smtx1)
if cuttype = one, mmtx1 = matt(m1)
if cuttype = two, mmtx1 = matt(smtx1)
if cuttype = -2, mmtx1 = matt(bmtx1)
if cuttype = three | cuttype = five, mmtx1 = matt(cmtx1)
if cuttype = four, mmtx1 = matt(amtx1)
if cuttype <> one, mmtx1 = mmul(mmtx1, smtx1)

Version X (required)

map_home : yes #Use home positions as entered or map to machine axis

pmatrix_su #Setup mapping matrix
hmtx1 = matt(m1)
hmtx1 = mmul(hmtx1, smtx1)
if cuttype = one, mmtx1 = matt(m1)
if cuttype = two, mmtx1 = matt(smtx1)
if cuttype = -2, mmtx1 = matt(bmtx1)
if cuttype = three | cuttype = five, mmtx1 = matt(cmtx1)
if cuttype = four, mmtx1 = matt(amtx1)
mmtx1 = mmul(mmtx1, smtx1)

Modification to pmatrix_su for 2X lathe posts (mplgen and mpl_ez based)

pmatrix_su #Setup mapping matrix
# hmtx1 = matt(m1$)
# mmtx1 = matt(m1$)

In some cases, the cuttype variable is prefixed with c1_ so update post can not automatically fix it. You will need to make the following modification manually in these cases:

pmatrix_su #Setup mapping matrix
hmtx1 = matt(m1$)
#if c1_cuttype <> one, hmtx1 = mmul(hmtx1, smtx1) #No longer needed
hmtx1 = mmul(hmtx1, smtx1) #Replaced by this
if c1_cuttype = one, mmtx1 = matt(m1$)
if c1_cuttype = two, mmtx1 = matt(smtx1)
if c1_cuttype = -2,mmtx1 = matt(bmtx1)
if c1_cuttype = 3 | c1_cuttype = 5, mmtx1 = matt(cmtx1)
if c1_cuttype = 4, mmtx1 = matt(amtx1)
#if c1_cuttype <> one, mmtx1 = mmul(mmtx1, smtx1) #No longer needed
mmtx1 = mmul(mmtx1, smtx1) #Replaced by this

The second change in X deals with parameter values read by the posts. In earlier versions of Mastercam parameter values were sometimes reused in several toolpaths with a different meaning for each tool path, this lead to a lot of confusion. So, when we created X we had a developer spend a lot of time going through all of the parameters and had him reassign the shared parameters so each has a unique meaning. That’s not to say that they are no longer shared, just that if a parameter means one thing in one tool path, it will mean the same thing in another (if it is available for that toolpath).

The most common symptom of failure to update the parameter values used is faulty output in canned cycles, although other errors in code generation may also occur.

Unfortunately, there is no way for the update post c-hook to really determine if a number in a post is actually a parameter value or if it is being used for something else so we are forced to go through the posts manually to modify the values if needed.

With this in mind we put together the information contained in the MastercamX_Post_Parameter_Ref.pdf file that is included with the installation in the \mcamx\documents\ folder (you can also launch it from Start/All Programs/MastercamX/Documentation/. This file contains all of the parameters available at the time of release (it has since been updated for MR1/SP2). You can launch the .pdf, search for a parameter and see if it has changed pretty quickly (it usually only takes a few minutes to go through the values in the post). In most cases, the parameters are in lookup tables (especially if the post is MPLFAN or MPLGEN based).

Here is the section from Generic Fanuc 2X Lathe.pst (updated MPLGEN) and Generic Fanuc 4X MT_Lathe.pst (updated MPLFAN):
#--------------------------------------------------------------------------
# Parameter information lookup tables, see pparameter
#--------------------------------------------------------------------------
fprmtbl 1 5 #Rough cut parameters
13343 depthcc #Was 10200
10407 clearcc #Was 10201
10202 xstckcc
10203 zstckcc
10214 directcc

fprmtbl 2 4 #Finish cut parameters
13341 ncutscc #Was 10100
10101 depthcc
10102 xstckcc
10103 zstckcc

fprmtbl 3 5 #Groove cut parameters
13358 stepcc #Was 10301
13138 directcc #Was 10306
13352 dopeckcc #Was 10312
10316 depthcc
13364 clearcc #Was 10320

fprmtbl 104 4 #Thread cut parameters
10811 xmaj_thd #Was 10411
10813 zstrt_thd #Was 10413
10814 zend_thd #Was 10414
10819 face_thd #Was 10419

Chances are you may be able to cut and paste the above section right into your post. If you have any additional values in your parameter tables, look them up in the .pdf file mentioned above to see if they have changed.
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 06:29 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