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! > MetalWorking Machines > Haas Mills


Haas Mills Discuss Haas machinery here!


This forum is sponsored by:

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #1   Ban this user!
Old 02-05-2008, 04:31 PM
 
Join Date: Jun 2007
Location: USA
Posts: 7
QMI2007 is on a distinguished road
HAAS Radius error

I am using Mastercam X2 and have an issue when I post a simple 2D program out to my HAAS. It uses an R command for G2/G3 moves instead of I/J which is how it's always been. I have had problems since I downloaded X2-MR1. If there are two arcs tangent to each other(for instance if you were to mill the outside profile of the Mastercard logo) instead of going around the outside of both circles it will make its own arc connecting the end point of the first arc to the end point of the second arc in the shortest distance possible which instead of following the correct contour. Is there an arc tolerance or some other setting in the HAAS control that could eliminate this issue?
Tweet this Post!Share on Facebook
Reply With Quote

  #2   Ban this user!
Old 02-05-2008, 07:40 PM
CNCRim's Avatar  
Join Date: Feb 2006
Location: usa
Posts: 944
CNCRim is on a distinguished road

post a design file with toolpath we might see something. You can edit the post to output R instead I/J.
__________________
The best way to learn is trial error.
Tweet this Post!Share on Facebook
Reply With Quote

  #3   Ban this user!
Old 02-05-2008, 07:44 PM
 
Join Date: Jul 2005
Location: Canada
Posts: 11,419
Geof will become famous soon enough

It could be that the arc you need goes past 180 degrees. When you are using R for G02/G03 and the arc is larger than 180 degrees the R value has to be negative; if it is less than 180 degrees it is positive.
__________________
An open mind is a virtue...so long as all the common sense has not leaked out.
Tweet this Post!Share on Facebook
Reply With Quote

  #4   Ban this user!
Old 02-06-2008, 12:00 AM
Donkey Hotey's Avatar  
Join Date: Nov 2007
Location: USA
Posts: 1,636
Donkey Hotey is on a distinguished road

This really belongs in the Mastercam forum.

I had a similar problem last night. I was trying to clear a round pocket in MC X. When it posted, the command was a positive R value and caused an error on the Haas.

I haven't had time to experiment with it yet to find out why it posted that for one pocket but not the others.

Where did you get the post? Has it been modified?
__________________
Greg
Tweet this Post!Share on Facebook
Reply With Quote

  #5   Ban this user!
Old 02-06-2008, 12:02 PM
 
Join Date: Jun 2007
Location: USA
Posts: 7
QMI2007 is on a distinguished road

I dont think this is a Mastercam issue. Although it could be. The way I do things is the same as it always has been, these types of parts are new to this company though. I am less framiliar with Haas than I am with MCX that is why I feel there is some type of setting that is being overlooked and I dont have anyone here that really knows the machines either.
I have several Haas post processors, some that I have used for years at other companies, some were here when I started, some from colleagues which have always been fine. This problem has only begun occuring since running MCX2 MR1 in certain situations when posting with an R command. 85% of the time there is no problem but it seems to be popping up more on me. I did play around with it when it was in the machine, frustration set in and my only solution was re-posting certain toolpaths using I/J command.
For those who have had similar issues: I just had another one come up this morning. Helical milling a counterbore, and the last pass doesnt go around at final depth, it just reaches final depth and retracts out, thus leaving a spiral in the bottom of the hole??????
Tweet this Post!Share on Facebook
Reply With Quote

Sponsored Links
  #6   Ban this user!
Old 02-06-2008, 03:04 PM
 
Join Date: Jul 2005
Location: Canada
Posts: 11,419
Geof will become famous soon enough

Originally Posted by QMI2007 View Post
..... Helical milling a counterbore, and the last pass doesnt go around at final depth, it just reaches final depth and retracts out, thus leaving a spiral in the bottom of the hole??????
Show us the code.

I have made a mistake in a program that gave me this result. This is an example of the code:


G91 G03 I0. J-.4 Z-.1 F50. L4
This line goes around four times incrementing down 0.1 per circle. But there is a ramp at the bottom of the hole so you need to go around once more to take that out.

Instead of typing the complete line I copy this one using the editor and change the G91 to a G90 to get:

G90 G03 Io. J-.4 Z-.1 F50. L4

I do not want to go around four times so I take the L4 away:

G90 G03 I0. J-.4 Z-.1 F50.

And run the program....and wonder why I still have a ramp at the bottom of the hole???

I forgot to take out the Z-.1 so once I have gone back to absolute the Z moves up to -.1 absolute on the last circle.

When I find it I feel a bit silly.
__________________
An open mind is a virtue...so long as all the common sense has not leaked out.
Tweet this Post!Share on Facebook
Reply With Quote

  #7   Ban this user!
Old 02-06-2008, 03:52 PM
 
Join Date: Jun 2007
Location: USA
Posts: 7
QMI2007 is on a distinguished road

here is the code that did not leave the c'bore flat at the bottom:


Z5.37
G01 Z5.27 F40.
G41 X-4.165
G03 X-4.415 Z5.245 R.125
X-4.165 Z5.22 R.125
X-4.3362 Y.8912 Z5.2045 R.125
X-4.165 Y.775 R.125
X-4.3583 Y.8797 R.125
G01 G40 X-4.29 Y.775
G00 Z9.

when I post it with I/J it works fine though????
Tweet this Post!Share on Facebook
Reply With Quote

  #8   Ban this user!
Old 02-06-2008, 08:27 PM
 
Join Date: Nov 2003
Location: USA
Posts: 231
Haas_Apps is on a distinguished road
Program Error

I just put this program in MetaCut and it shows that there is a problem with the G-code. See attachment.
Attached Thumbnails
Click image for larger version

Name:	cnczone.jpg‎
Views:	71
Size:	5.1 KB
ID:	52625  
Tweet this Post!Share on Facebook
Reply With Quote

  #9  
Old 02-06-2008, 08:48 PM
HuFlungDung's Avatar
Moderator
 
Join Date: Mar 2003
Location: Canada
Posts: 4,823
HuFlungDung is on a distinguished road

My 1996 Haas VF3 may have some bug in the software, but the other day I was performing a clean circle operation in 10 holes in sequence. The operation consisted of two complete circles, no tool comp involved.

So it did the first three holes normally, then on the 4th hole it seemed to skip one of the circles, did a few more holes, then same thing again.

Only thing I had changed lately was to change my post output to permit complete circles to be cut with one command. So, I changed it back to half circle max per command, and then it worked fine.

I was using IJ arc centers, not R.
__________________
First you get good, then you get fast. Then grouchiness sets in.

(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Tweet this Post!Share on Facebook
Reply With Quote

  #10   Ban this user!
Old 02-07-2008, 11:34 AM
 
Join Date: Sep 2007
Location: USA
Posts: 116
SeymourDumore is on a distinguished road

First of all, that code snippet without the starting X and Y coords is useless as none of the backp[lotters can figure out where the paths start from.
Also, you seem to have the modal coords turned off in MCX. It isn't a problem for Haas but it is a problem for trying to figure out where your problem is.
One thing, the Haas is doing circles the very same way Pre or Post MCX, suggesting that the problem is in your post or how MCX handles the post. Pointing the finger at the control when your software has changed is not logical.
Anyway, as Geof said, R is positive for arcs less than 180 deg, and negative for above but not more than 359 degree. If the arc is a full circle (which the Haas can do just fine) you MUST use I and J, you can even omit the X and Y coords.
IOW the following code will make a 1" radius circle with it's center at 0,0:

G01 X0 Y.5
G02 I0 J-.5

Anyway, post the whole code and perhaps add the modal coords as well because the above snippet will make only one full circle and a bunch of small arcs within the circle.
Tweet this Post!Share on Facebook
Reply With Quote

Sponsored Links
  #11   Ban this user!
Old 02-07-2008, 11:48 AM
 
Join Date: Jul 2005
Location: Canada
Posts: 11,419
Geof will become famous soon enough

Originally Posted by SeymourDumore View Post
..... the above snippet will make only one full circle and a bunch of small arcs within the circle.
I did put in an arbitrary start position and ran it in a Haas simulator; it did the two semicircles to complete the full circle than gave a radius error and would not go further so I didn't go any further.
__________________
An open mind is a virtue...so long as all the common sense has not leaked out.
Tweet this Post!Share on Facebook
Reply With Quote

Reply

Tags
haas, mastercam




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
Haas Control: Radius dimensions instead of diameter Donkey Hotey Haas Lathes 7 05-28-2008 05:17 PM
Haas startup error Crash Haas Mills 5 12-04-2007 11:15 AM
Mach 3 with Mastercam X "Radius to end of Arc" error sweckard Mach Mill 6 07-06-2007 08:43 PM
Haas Overvoltage Error 119 cncnovice Haas Mills 1 06-29-2006 09:21 AM
HAAS 123 error marto74 Haas Mills 5 05-18-2005 03:24 PM




All times are GMT -5. The time now is 11:25 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