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 05-06-2004, 06:10 PM
tex tex is offline
 
Join Date: Apr 2004
Location: Serbia and Montenegro
Age: 48
Posts: 60
tex is on a distinguished road
Thread deburring

I have a lot of trouble deburring (blunting) threads at the beginning and at the end of them. The G-codes that I do are generally for 1/6" pitch rounded threads on a HAAS SL-30 lathe (supposed to have Fanuc6T controller or similar).

Any ideas about how to make a G-code for "cleaning" the start and finish portion of the thread?
Tweet this Post!Share on Facebook
Reply With Quote

  #2   Ban this user!
Old 05-06-2004, 07:04 PM
WOLOG's Avatar  
Join Date: Oct 2003
Location: HOUMA,LA
Posts: 352
WOLOG is on a distinguished road

Do you mean a thread clip where you are cutting part of the thread off to allow for easy makeup?

If you do, use a grooving insert. program another threading cycle using the grooving tool and the same thread info. The part you have to play around with is the amount of thread you want to remove. Set your "Z" length accordingly. Now move your "Z" starting position until you "clip just the starting thread and not the second thread. Make sure that you use a M24 before the G76 line.

If you don't understand what I am saying, I can Email you a sample program so that you can see what you need to do.

As far as the rear of the thread, I never had to worry about that.

Good luck

By the way, I have a Haas SL-30 Big Bore.
Tweet this Post!Share on Facebook
Reply With Quote

  #3  
Old 05-06-2004, 07:10 PM
Rekd's Avatar
Community Moderator
 
Join Date: Apr 2003
Location: teh Debug Window
Posts: 1,877
Rekd is on a distinguished road

Are you deburring before you thread? That's how I do it.

'Rekd
__________________
Matt
San Diego, Ca

___ o o o_
[l_,[_____],
l---L - □lllllll□-
( )_) ( )_)--)_)

(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

  #4   Ban this user!
Old 05-06-2004, 07:23 PM
tex tex is offline
 
Join Date: Apr 2004
Location: Serbia and Montenegro
Age: 48
Posts: 60
tex is on a distinguished road

I'm working on SL-30 Big Bore......it's not mine, though...

The beginning of a thread is "sharp" and needs to be "flattened", so it would look better and nobody could cut himself while twisting it in his hands...here's a sample of a sequence I use for making an OD thread:

G99 M24
X72.2 Z0
M19 P180
G97 S400 M03
G76 D0.8 X65. Z-19. K2.5 F4.23

This cycle is making an almost perfect 70mm thread with 4.23 pitch (1/6"). I do the spring pass afterwards.

In this case I am using M24, but when I do IDs I use M23.

I have tried different "P" and "X" settings, but to no avail. Never thought about changing "Z", though......I wonder whether a grooving insert would follow the same thread lead if I change "Z".

I have tried to do the deburring operation in a tapered way (with an “I” command), but without any success.

If it would be not much trouble to you, please contact me on:

tex707@net.yu

and send an operation code that could do the job. I'm almost desperate about this...
Tweet this Post!Share on Facebook
Reply With Quote

  #5   Ban this user!
Old 05-06-2004, 07:29 PM
tex tex is offline
 
Join Date: Apr 2004
Location: Serbia and Montenegro
Age: 48
Posts: 60
tex is on a distinguished road

Originally posted by Rekd
Are you deburring before you thread? That's how I do it.

'Rekd
I am not quite sure what you mean...if I do the deburring before I do the thread, the threading insert would leave the sharp edges at the beginning and at the end of a thread. I do a spring pass after a deburring pass and the abovementioned sharp edges are still there...
Tweet this Post!Share on Facebook
Reply With Quote

Sponsored Links
  #6  
Old 05-06-2004, 10:33 PM
Rekd's Avatar
Community Moderator
 
Join Date: Apr 2003
Location: teh Debug Window
Posts: 1,877
Rekd is on a distinguished road

I chamfer meh holes before I thread them. Usually .015 or so bigger than the major dia. Pretty much anything left after that, like razor edges or small burrs can be taken off with scotch-brite or what ever.

'Rekd
__________________
Matt
San Diego, Ca

___ o o o_
[l_,[_____],
l---L - □lllllll□-
( )_) ( )_)--)_)

(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

Last edited by Rekd; 05-06-2004 at 10:45 PM.
Tweet this Post!Share on Facebook
Reply With Quote

  #7   Ban this user!
Old 05-06-2004, 10:46 PM
 
Join Date: Jul 2003
Location: usa
Posts: 5
cncrunner is on a distinguished road

Give this a try:
1. Run your finish chamfer/turning tool.
2. Run the threading cycle, no spring passes required.
3. Call the finish chamfer/turning tool back up and run it again. This will remove the burrs from the o.d.
4. Last, run the threading cycle again. You can increase the depth of cut so that it those not take as many passes. This will remove the burrs that were kicked in from the turning tool.

This process may seem long, but it those not add much cycle time when done correctly. You will get a burr free thread every time.

Bill.
Tweet this Post!Share on Facebook
Reply With Quote

  #8   Ban this user!
Old 05-07-2004, 02:47 AM
tex tex is offline
 
Join Date: Apr 2004
Location: Serbia and Montenegro
Age: 48
Posts: 60
tex is on a distinguished road

Chamfering/threading/rechamfering/spring pass does not work...that's the first thing I've tried. The customers want a product with "flattened" thread beginning and end....
Tweet this Post!Share on Facebook
Reply With Quote

  #9   Ban this user!
Old 05-07-2004, 03:20 AM
tex tex is offline
 
Join Date: Apr 2004
Location: Serbia and Montenegro
Age: 48
Posts: 60
tex is on a distinguished road

I suppose that you guys understand my problem, but I've attached these screenshots to make everythnig easier. You can see the way "my" thread looks like at the top shot and the portion that should be "flattened" with a grooving tool at the bottom one.
Attached Thumbnails
Click image for larger version

Name:	complete2.jpg‎
Views:	368
Size:	33.1 KB
ID:	2256  
Tweet this Post!Share on Facebook
Reply With Quote

  #10   Ban this user!
Old 05-07-2004, 01:46 PM
WOLOG's Avatar  
Join Date: Oct 2003
Location: HOUMA,LA
Posts: 352
WOLOG is on a distinguished road

TEX,

Did you get the email I sent you earlier today?
It had an attached file for a clipped 3 pitch acme male thread. That is what you are looking for. If you didn't get the file, I will send it to you again.
Attached Files
File Type: txt thread clip example.txt‎ (780 Bytes, 167 views)
Tweet this Post!Share on Facebook
Reply With Quote

Sponsored Links
  #11   Ban this user!
Old 05-07-2004, 01:53 PM
tex tex is offline
 
Join Date: Apr 2004
Location: Serbia and Montenegro
Age: 48
Posts: 60
tex is on a distinguished road

Originally posted by WOLOG
TEX,

Did you get the email I sent you earlier today?
It had an attached file for a clipped 3 pitch acme male thread. That is what you are looking for. If you didn't get the file, I will send it to you again.

No, I haven't received any mail from you yet. You could try to resend it using these two addresses:

tex707@net.yu
tex707@shortonfinal.net

Is the file any different from the file you've attached in this post?

One question about the program...what does "A14" command stand for, and how come you do not use "M19" command to position a spindle at the right angle before you apply a second tool..?...seems like these are two questions...

WOLOG, thank you very much for your effort to help me...and all you guys, you're great!

Last edited by tex; 05-07-2004 at 02:02 PM.
Tweet this Post!Share on Facebook
Reply With Quote

  #12   Ban this user!
Old 05-07-2004, 02:48 PM
WOLOG's Avatar  
Join Date: Oct 2003
Location: HOUMA,LA
Posts: 352
WOLOG is on a distinguished road

Tex, it is the same file. The A14 is a 14 degree infeed angle for the acme thread. The M19 spindle orientation should not ne an issue for this. My software "geopath" codes the threading cycle like the example. The start position X2. Z.2 M08 determines the start position. If you change the start position to X2. Z.3, you are out of lead. In order to clip the thread, you must split the lead. You have to actually cut the creat of the thread and not the root as you did in the first threading cycle. It will take a few minutes to figure out where the correct start position and the correct Z length needs to be to only cut the starting thread.

I am going buy a digital camera tonight. I hope to send you a picture of the 4" 3 pitch acme connection that the g-code file describes. As soon as you see the picture, it will all make sense.

give me some specifics on your machine, maybe I can figure out your M19 question.
Does it have live tooling?

I hope this helps
|James
Tweet this Post!Share on Facebook
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
Thread mill programming software? cncwhiz G-Code Programing 6 12-31-2008 02:48 PM
Thread milling, can anyone help jtrav General CAM Discussion 16 03-06-2006 03:25 PM
Hard-to-machine thread tex G-Code Programing 30 11-04-2005 01:17 PM
for engraving pcb which is a good thread size for the lead screw? NickLatech DIY-CNC Router Table Machines 11 01-17-2005 09:37 PM
Thread milling cutterdia / hole ratio HuFlungDung Machine Problems, Solutions , Wireless DNC, serial port 3 12-31-2003 09:44 PM




All times are GMT -5. The time now is 11:35 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