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 > TurboCNC


TurboCNC Discuss TurboCNC controller software here!


Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #1  
Old 06-17-2003, 07:55 PM
*Registered*
 
Join Date: Mar 2003
Posts: 109
smitty is on a distinguished road
Lathe programing help

Yes it is me again!!
But this time, I am ready to make parts again, but need a little help in the programing area.
I have included a picture of the parts that I make, along with the stock parts. The shinny one is the one I made out of Titanium.
The radius is made with a radius cutter, but now I have the lathe I should be able to make this much quicker.
When programming a radius hows is that done? I'm sure that this will need numerous cuts to get to the final diameter, but not sure on where to start.
Any advice greatly needed,
Smitty
Attached Thumbnails
Click image for larger version

Name:	im000732.jpg‎
Views:	294
Size:	47.8 KB
ID:	353  
Tweet this Post!Share on Facebook
Reply With Quote

  #2  
Old 06-18-2003, 12:13 AM
HuFlungDung's Avatar
Moderator
 
Join Date: Mar 2003
Location: Canada
Posts: 4,823
HuFlungDung is on a distinguished road

Smitty, are you going to write your programs by hand? Are you good with a calculator, and do you understand a bit of trigonometric functions?

I'd highly recommend you get some software to help you out, maybe Bobcad 17 would do for a start, yet be quite cheap.

I haven't gathered from the discussions exactly what TurboCNC expects for arc parameters but here is the general rule: from wherever your machine (tool) is positioned right now, an arc command needs to contain an X and a Z coordinate for the endpoint of the arc coming up, plus it needs an I and a K coordinate to tell it where the center of the arc's radius is located.

If your machine can move a maximum of 90 degrees per arc command, then it needs no G02 or G03 to tell it the direction to move around the circle, this is typical of some controllers. However, usually a G02 or a G03 is needed to command the direction clockwise or counterclockwise movement when the arc is being traversed.

So
G02 Xx.xxx Zz.zzz I.iii Kk.kkk
is what the generic command would look like. I corresponds to the X coordinate of the arc center, and K corresponds to the Z coordinate of the arc center.

Some controllers will instead accept a R parameter which is the radius, so you would see
G03 Xx.xxx Zz.zzz Rr.rrr

Some controllers are very exacting about the accuracy of the arc center coordinates, and high precision is required for the calculation. The controller checks it current position, looks at the end coordinate of the arc, and then determines whether it can actually get there if the center is where you have specified. If not, then it may give you an error, and not move at all, or else, it will make a correction (linear movement) at the end of whatever portion of the arc it does attempt to do, which will create a gouge or something undesirable in your toolpath.

When you make the calculations for the arc coordinates, you need to know whether the controller expects the arc center coordinates to be in absolute coordinates (from a main part zero point), or incremental coordinates (point to point movement).

In addition, for lathe tools, you need to make a tiny allowance for the tool nose radius of the insert you are cutting with. Since your toolpath is typically planned for a theoretically sharp point, this means in real life, that if you use the "sharp point path" for a final path, the radii you cut will be slightly larger than the specification, let's say by .015 to .031 inch, as these are typical tool radii.

So then, you need to allow for this by drawing your part paths slightly undersize by the amount of the tool nose radius. Or, use tool nose radius compensation at the controller to do this for you on the standard full-scale part profile.

One other trick in lathe programming is of course, that X is usually a diametral figure (Z is not) rather than the actual length of the radius, so a quarter circle starting on the centerline at X0Z0 and moving through a 90 degree sweep on a 1" radius, would be written something like
G02 X2.000 Z-1.000 I0.000 K-1.000. If X were a radius value then you wouldn't have to remember to double the X values all the time.

Now you know why you need some software to give you a hand
__________________
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)

Last edited by HuFlungDung; 06-18-2003 at 12:34 AM.
Tweet this Post!Share on Facebook
Reply With Quote

  #3  
Old 06-18-2003, 12:49 AM
*Registered*
 
Join Date: Mar 2003
Posts: 109
smitty is on a distinguished road

I see that I am in for some serious work!
Thanks for the help, this might be a little over my head.
Might have to go back tothe radius cutter for now, until I can get a grip on this!
Smitty
Tweet this Post!Share on Facebook
Reply With Quote

  #4   Ban this user!
Old 06-18-2003, 09:46 AM
WOODKNACK's Avatar  
Join Date: Mar 2003
Location: Maine
Posts: 271
WOODKNACK is on a distinguished road

Is that for a RC car Or Truck?
__________________
My little piece of the web!
http://users.adelphia.net/~wjdupont

Tweet this Post!Share on Facebook
Reply With Quote

  #5  
Old 06-18-2003, 09:51 AM
*Registered*
 
Join Date: Mar 2003
Posts: 109
smitty is on a distinguished road

1/8 scale on-road race car. Mugen MRX3
Any idea where I might find a decent program that won't break the bank. I have been reading about Bobcad, and the reviews are not in their favor. I have Vector when I bought the Mill, but it will not load, might give them a call.
SMitty
Tweet this Post!Share on Facebook
Reply With Quote

Sponsored Links
  #6   Ban this user!
Old 06-18-2003, 10:01 AM
wjbzone's Avatar  
Join Date: Apr 2003
Location: United States
Posts: 396
wjbzone is on a distinguished road

Smitty,
I program a lot of lathe parts, but only use turbocnc for my mill.

The parts you have look fairly easy to program using a Cad program to get the points.

Do you have it on a cad program? I might be able to give you some examples or help.

Bill
Tweet this Post!Share on Facebook
Reply With Quote

  #7  
Old 06-18-2003, 10:15 AM
*Registered*
 
Join Date: Mar 2003
Posts: 109
smitty is on a distinguished road

I have Vector when I bought my Mill, but it will not load. I will call them today and see what they can do. Other than that, no CAD programs.
Thanks for the help
Smitty
Tweet this Post!Share on Facebook
Reply With Quote

  #8  
Old 06-18-2003, 12:01 PM
HuFlungDung's Avatar
Moderator
 
Join Date: Mar 2003
Location: Canada
Posts: 4,823
HuFlungDung is on a distinguished road

Vector is pretty much the same thing as Bobcad, so I've heard. If you have a copy already, there is no harm in trying to get it working.

Bobcad or Vector level programs are plenty good enough, IMO, for hobbyists just getting started in simple nc programming. But, if you can't get Vector working, watch the Bobcad site for 1/2 price specials, which appear quite frequently.

Maybe some of the other guys can vouch for the "bestest, cheapest" CADCAM that they know of.
__________________
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

  #9  
Old 06-19-2003, 08:46 PM
*Registered*
 
Join Date: Mar 2003
Posts: 109
smitty is on a distinguished road

And the list goes on,
I need to cut a groove in this part, but do not want to cut it all at once. I tried G78, plunged into fast. I also tried G83, but that won't work either, say's that I must be in the same direction of Z, but I am using X.
Any ideas?
Thanks
Tweet this Post!Share on Facebook
Reply With Quote

  #10  
Old 06-19-2003, 08:49 PM
*Registered*
 
Join Date: Mar 2003
Posts: 109
smitty is on a distinguished road

As for the CAD program, I called Vector, and they will fix me up! Just need to register the program I have, after they send me the diskette. So, hopefully I can get this running soon.
Smitty
Tweet this Post!Share on Facebook
Reply With Quote

Sponsored Links
  #11  
Old 06-19-2003, 10:50 PM
HuFlungDung's Avatar
Moderator
 
Join Date: Mar 2003
Location: Canada
Posts: 4,823
HuFlungDung is on a distinguished road

Well Smitty, glad you're getting fixed up with some software.

Yes, as you have found out, there are limitations to the use of canned cycles on lathes.

The G81, G82, G83, G84 are all designed to operate with predetermined motions in the Z direction, since the assumption is made that you will be drilling a hole, with the drill point positioned right at X0 on the lathe's centerline. These cycles cannot be used in the X direction.

However, there is no real magic to these canned cycles, they are simply a shortcut to a common procedure, but you do have to learn about what axis are active for the duration and what they do.

For "peck grooving" which it sounds like what you are doing, a canned cycle would work if you were cutting a groove in the face of a part held in the chuck. But for the direction you are working in which is X, you'll have to write that one out longhand.

Now I don't want to burden you with information overload, but be aware that you can write a small subroutine to accomplish the peck movements in X. It will not be modal, which means you have to call it every time you want to use it. But, once it is written, you can write your main program very quickly, planning your main program moves to each groove location, followed by one run through the subroutine.

By contrast, canned cycles in the G8x series, remain active until cancelled. This is what modality means. This is not all that useful on a lathe, but on a mill, it allows for one rapid move to occur between each execution of a hole drilling cycle.

important Shut off a canned cycle in the G8x series with a G80, which is the shorthand command for cancelling the active cycle. It is a good idea to place certain commands at the beginning of your program, just to make sure that all such things are shut off before the program runs again. Sometimes, you'll abort a program part way through, and if a G8x cycle was still active, it may go yet again after the first positioning move is read even when your program starts over.

For example, the very first lines of your main program should contain things like
G54 (cancel work offsets, applicable to mills)
G40 (cancel tool radius comp)
G80 (cancel any canned cycle)
G90 or G91 (Tell the machine whether the main program is going to be in absolute or incremental coordinate systems.

So if you want to know about writing subroutines, just post a brief answer describing how you would call up one for your controller

BTW, I do not know anything about Turbocnc, so what I have written above is to be understood to be general gcode rules.
__________________
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)

Last edited by HuFlungDung; 06-19-2003 at 11:58 PM.
Tweet this Post!Share on Facebook
Reply With Quote

  #12  
Old 06-20-2003, 12:14 AM
*Registered*
 
Join Date: Mar 2003
Posts: 109
smitty is on a distinguished road

HFD,
You are just a wealth of Inforamtion!! Very glad I have stumbled upon this site for sure!
Now, as for subroutines, how is that accomplished? I do believe that Turbocnc follows most G code rules, so if you feel up to it, show me the way! My groove is .060 deep, but I also am machining Titanium, so I was only going in .005 at a time to be safe.
I was playing around with other codes, and came across G77, now that one alone save me 25 lines.
Smitty
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
Using your CNC Mill as a CNC Lathe lstool Knee Vertical Mills 10 08-02-2010 01:06 AM
Help me buy my first Mini Lathe Highfly Mini Lathe 20 05-10-2005 03:07 AM
OneCNC XR Series Lathe CAD/CAM Released: OneCNC Product Announcements & Manufacturer News 0 03-07-2005 05:20 PM
Just got a taig lathe. anoel Mini Lathe 2 01-18-2005 05:29 AM
non-circular lathe turning Help! oldguy General Metal Working Machines 2 04-06-2004 12:55 PM




All times are GMT -5. The time now is 07:55 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