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 > Hard and High Speed Machining


Hard and High Speed Machining Discuss Hard and High speed Machining here!


Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #13  
Old 09-28-2007, 02:39 PM
*Registered User*
 
Join Date: Jul 2004
Location: USA
Age: 37
Posts: 374
fpworks is on a distinguished road

Scott_bob,
Very interesting to hear about this Numeryx setup. I firmly believe a more advanced control would dramatically improve the lifespan of the mechanical components in a Fadal as well. The -88 control is very hard on the machine.

You are correct...there is much tuning required to get accurate parts to run fast. If I wasn't concerned about speed, I could just copy the entire program from the Fadal to our Mazak, but then I wouldn't be taking advantage of our much more expensive machine, which I bought because it can run parts faster.

I will be certain to take a look at the Numeryx system at IMTS this upcoming year. When I bought our Mazak, I quickly saw the deficiency of the Fadal control. Lots of people are worried about "conversational" capability and menu interfaces when purchasing a new machine, but IMO the real advantage of a good control comes with MOTION control. All that other stuff is just user preference.

I would be somewhat concerned with Numeryx's "always on" lookahead feature. Reason being, I've found that adjustability of the lookahead feature is required to find the proper blend of [floor] finish quality, cycle time, and part accuracy between every part. Every part has different requirements, and the aforementioned items are all related by a give and take relationship.

BTW, for those who doubt the practicality of 400+ ipm, here is a video of our Mazak running one of our parts. (BTW, this is a wimpy cut that doesn't remotely challenge the machine) Parameters:
Spindle: 12,000 rpm
Feed: 210-460 ipm (variable by Mastercam highfeed option, AKA "adaptive feedrate")
Tool: 0.375" 2 flute uncoated carbide endmill
Engagement: 40% radial, 0.28" depth
Material: 6061 aluminum

http://www.foreprecisionworks.com/video/MVI_2165.AVI


This following video is facing with a .75" endmill at 460 ipm and 10,000 rpm (would go to 600 ipm, but there are too many tight direction changes and the workholding is questionable...ripped a part out at 525 ipm earlier)

http://www.foreprecisionworks.com/video/MVI_2164.AVI
Reply With Quote

  #14   Ban this user!
Old 10-13-2007, 06:02 PM
krustykrab's Avatar  
Join Date: Mar 2004
Location: Ontario, Canada
Posts: 87
krustykrab is on a distinguished road

Perhaps my settings, but couldn't download the video.

That sounds like a pretty healthy cut for an endmill that small.

I have a minicut 1" dia. high polish aluminum roughing endmill (interupted cut) that I like to use. Cuts like butter. I can take a 1/2" stepover and 1" d.o.c. with an rpm of about 1800 and feedrates of about 200 ipm. Does that seem good? I don't use a lot of endmills, so I like to learn more from other people. Most of my cnc machining is 3d using indexible high polished carbide cutters.

Anyway, back to your original post. I must have misunderstood your query. I will go back and read it, I apologize for not being more thorough.

ScottBob, I too have heard of Numerix from my Fadal service guy......who I see quite often :/. We did look into it about 5 years ago, I think. Their quote was $35,000 to install the controller and have all of the retrofitting, done.......new drives, scales, etc. To much peanut butter on my toast!
__________________
"'Tis a poor workman who blames his tools."
Reply With Quote

  #15  
Old 10-14-2007, 11:33 AM
*Registered User*
 
Join Date: Jul 2004
Location: USA
Age: 37
Posts: 374
fpworks is on a distinguished road

krustykrab,
No apologies required...we are all guilty of skimming posts as well.

Try saving it to your computer first, then viewing.

Your cutting parameters are healthy, no doubt. I'm not trying to pick, but your machining strategy is old school and there are better and faster ways to handle it, ONLY IF you have a machine that can handle higher feedrates. I'll try to explain:

In that cut, you are removing 100 cubic inches per minute, which is a descent amount of material. BUT, it isn't simply about material removal, because in real world applications, your cut will not always be 100 cubic inches per minute all the time, unless you are cutting straight lines every day.

For instance, I would handle that cut with the following parameters: 1" deep, 0.2 stepover, but feed at 450 ipm, which is relatively conservative. Note that the material removal rate is about 10% less than your cut, but it will cut almost any profiling or pocketing geometry faster. (the effect will be more pronounced with more complex geometry) Please feel free to enter these parameters into your CAM system and see for yourself.

Why? If you were to take the average material removal rate during the cut, it will stay consistently higher. The toolpath has the opportunity to be more efficient with a smaller stepover. (follows geometry more closely AND less air cutting time)

I know this may be difficult to understand at first...it was for me, but this is the sole reason behind high speed machining...faster, lighter cuts produce parts faster than heavier, slower cuts. With the Fadal control, this concept simply doesn't apply...however, keep reading ;-)

This phenomenon is why adaptive feedrate (from your cam system) works so well. (I apologize if you already know how it works, but I'll write here briefly for others) Since your cutter will not always be at your stepover or angular engagement that you specified in your cutting parameters, you will leave quite a bit of time on the table. Adaptive feedrate will post a new feed (sometimes on every line) based on the volumetric removal rate in which your cutter is engaged.

Having said that, and referring back to the video in which I specified 210-460 ipm with a 0.375 endmill...I am cheating, since the stepover is not maintained when the feed is commanded at 460 ipm. The adaptive feedrate makes it so that when the cutter is fully engaged, the feed is 210 ipm. As the stepover decreases (even to air cutting, which is eventual) the feed progresses to 460 ipm.

Since nothing is free, the ability to feed at these higher rates brings forth accuracy problems, and for the control to "prepare" for these [programmed] high speed corners so that it doesn't tear up the machine, and can maintain accuracy. (hence my original question in the post)

To give some further examples...when we started our business, we had a CAM software that was unable to post neither adaptive feedrates nor a high speed toolpath with nice rounded corners. Also, we were also using our Fadal with 6000 rpm max and using old school techniques...heavier, slower cuts.

With our Mazak and higher end CAM software, AND applying the aforementioned techniques, here are the examples of our production improvements:

Part 1: Before=21 minutes, After=5:15
Part 2: Before=35 minutes, After=12 minutes

Granted, 2-3 minutes on each part was also saved in toolchanges, axis acceleration, and rapids. BTW, applying the adaptive feedrate on our Fadal saved ALONE saved four minutes on each part on "Part 2." (not reflected in the above times)
Reply With Quote

Sponsored Links
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 Off
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Ball-Bar measuring technique and mapping ballscrew AKFALAR Linear and Rotary Motion 2 05-06-2007 08:20 PM
What's your technique for routing out parts originator General Metalwork Discussion 4 02-04-2007 01:33 AM
Textbook for technique/theory mill sharpening carlnpa General Metalwork Discussion 5 12-10-2005 05:53 PM
Control Technique Digitax DBE 750 AC Servo-Drive GalaticDan Servo Motors and Drives 6 09-16-2005 06:32 AM
Roughing/Finishing??? trevorhinze BobCad-Cam 1 08-02-2005 05:14 AM




All times are GMT -5. The time now is 10:33 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