adaptive vs contour for nested parts from plate
Close
Login to Your Account
Results 1 to 15 of 15
  1. #1
    Join Date
    Sep 2011
    Location
    Idaho
    Posts
    99
    Post Thanks / Like
    Likes (Given)
    28
    Likes (Received)
    16

    Default adaptive vs contour for nested parts from plate

    Which do you think will have longer tool life- adaptive or contour? Using 1/4" 3-flute Lakeshore Carbide rougher in 7075. Both have similar run times. The adaptive removes a higher volume of material. The contour only uses the first 1/8" of bit.

    I could fill in some of the empty areas for the adaptive but then I'm worried that the numerous small arcs of the widened slots will starve the ballscrews of oil and wear out the ballscrews.

    BTW waterjet would of course be more ideal but I'm a bit short on time once the material arrives.

    Thoughts?

    2d-adaptive_1.jpg

    2d-contour_1.jpg

  2. #2
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    9,313
    Post Thanks / Like
    Likes (Given)
    2207
    Likes (Received)
    6458

    Default

    My quick take - presuming this is a VMC with good coolant or mist for displacing chips, I'd go contour. But if the part allows, I'd have a deeper than 1/8" pass, with perhaps a lower FPT to keep chip to cutter gullet numbers reasonable.

    Rational being that 7075 is a clean cutting, relatively low abrasion material, and shouldn't pose excess risk for breaking in the cut. And as a low-modulus material, the main benefit of an adaptive path (lower cutting force at the tool edge) isn't really needed.

    Just be sure that coolant/mist chip removal is adequate and doesn't get masked by part features or clamping.

  3. Likes eaglemike, sigmatero, mmurray70 liked this post
  4. #3
    Join Date
    Sep 2011
    Location
    Idaho
    Posts
    99
    Post Thanks / Like
    Likes (Given)
    28
    Likes (Received)
    16

    Default

    Thanks. Yes, 10hp CAT40 VMC with boxed ways so don't think stiffness is an issue I was going off of Lakeshore's recommendation of 1/2 tool diameter but my gut says I can profile a bit steeper to get closer to 1D.

    Good point about the coolant being masked- that's gotten me before. I have three different spray nozzles that spray hard so will aim them from different directions to hopefully help blast chips out of the slots.

    http://www.lakeshorecarbide.com/pdf/VFA.pdf

  5. #4
    Join Date
    Jul 2005
    Location
    central Illinois
    Posts
    245
    Post Thanks / Like
    Likes (Given)
    1187
    Likes (Received)
    99

    Default

    Would you please elaborate on how this starves the ball screws and explain this please? I think I'm going to learn something new I was unaware of.

    "but then I'm worried that the numerous small arcs of the widened slots will starve the ballscrews of oil and wear out the ballscrews."

    Thanks!
    Old Gus

  6. #5
    Join Date
    Sep 2011
    Location
    Idaho
    Posts
    99
    Post Thanks / Like
    Likes (Given)
    28
    Likes (Received)
    16

    Default

    Not sure if it's an old wives tail or not and for this part it's probably not a concern but I've been told that if you do numerous repetitive small motions in a single direction, like troichoidal narrow slots, it can wear out the ballscrew since one axis is basically just vibrating back and forth. Again, not sure how true this is but I suppose it makes sense. In my case I have lots of movement in every direction plus it's not a repetitive production part so it's probably not a big deal.

  7. Likes gusmadison liked this post
  8. #6
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,171
    Post Thanks / Like
    Likes (Given)
    220
    Likes (Received)
    710

    Default

    Im saying the adaptive will win easily and save enough money on tooling to pay what ever needs replacing down the road especially in tougher materials
    Don


    Sent from my iPhone using Tapatalk Pro

  9. #7
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    958
    Post Thanks / Like
    Likes (Given)
    84
    Likes (Received)
    348

    Default

    Quote Originally Posted by Milland View Post
    My quick take - presuming this is a VMC with good coolant or mist for displacing chips, I'd go contour. But if the part allows, I'd have a deeper than 1/8" pass, with perhaps a lower FPT to keep chip to cutter gullet numbers reasonable.

    Rational being that 7075 is a clean cutting, relatively low abrasion material, and shouldn't pose excess risk for breaking in the cut. And as a low-modulus material, the main benefit of an adaptive path (lower cutting force at the tool edge) isn't really needed.

    Just be sure that coolant/mist chip removal is adequate and doesn't get masked by part features or clamping.
    agreed
    We do these parts like this all the time on a vacuum plate, I run contour generally with a 3/16 endmill and finish with a 1/8 or 3/32 depending on features. very rarely break and endmill usually because its my stupid programming mistake. I leave about .002-.003 from the bottom and just snap them off, put in cut jaws and finish them.
    Theres no sense in cutting away more stock then you need to.

  10. #8
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    765
    Post Thanks / Like
    Likes (Given)
    172
    Likes (Received)
    881

    Default

    I'd turn it all to chips using a 3/8" cobalt rougher, full depth. Spin it as fast as you can, and run the feed at as high as you can. I have had far more problems with remnant popping up and breaking endmills, destroying way covers and binding my auger than I care to recall. Everything gets turned to chips in my shop (mostly). I also would optimize the spacing so the endmill never needs to plunge. I would rather have a few less parts per plate than deal with that.

  11. Likes sigmatero, eaglemike, mmurray70 liked this post
  12. #9
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,997
    Post Thanks / Like
    Likes (Given)
    1530
    Likes (Received)
    1463

    Default

    What is the plan for the backside?

  13. #10
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    1,175
    Post Thanks / Like
    Likes (Given)
    27
    Likes (Received)
    391

    Default

    Quote Originally Posted by 2outof3 View Post
    What is the plan for the backside?
    Im curious too, tough to fixture that.


    Sent from my iPhone using Tapatalk Pro

  14. #11
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    958
    Post Thanks / Like
    Likes (Given)
    84
    Likes (Received)
    348

    Default

    Quote Originally Posted by G00 Proto View Post
    I'd turn it all to chips using a 3/8" cobalt rougher, full depth. Spin it as fast as you can, and run the feed at as high as you can. I have had far more problems with remnant popping up and breaking endmills, destroying way covers and binding my auger than I care to recall. Everything gets turned to chips in my shop (mostly). I also would optimize the spacing so the endmill never needs to plunge. I would rather have a few less parts per plate than deal with that.
    I understand where your coming from , I used to do and think that way also. But using a vacuum plate you dont have that problem.

  15. #12
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    765
    Post Thanks / Like
    Likes (Given)
    172
    Likes (Received)
    881

    Default

    Quote Originally Posted by Delw View Post
    I understand where your coming from , I used to do and think that way also. But using a vacuum plate you dont have that problem.
    Agreed, vacuum plates are pretty freaking cool. I would certainly invest in one if I had lots of plate work to do... I still would have a deep seated dislike of traditional contour toolpaths and the associated issues, but I would need to come up with a better excuse not to use them

    In many cases, I think I could equal or even slightly improve upon my times using traditional contours, especially on parts like this. I just don't like the un-even tool wear from taking Z steps; the non-uniform tool load as they go into corners and bark; the need to plunge (or ramp) an endmill; the propensity to load up an endmill if the coolant sputters; and as stated earlier, dealing with the loose chunks of remnant that seem to float around the machine enclosure.

    Probably most of all, I just like watching them run. Adaptive toolpaths just look and sound cool. At the end of the day, I'm just a hobbiest that does this because I like it... luckily, my hobby pays the bills

  16. #13
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    958
    Post Thanks / Like
    Likes (Given)
    84
    Likes (Received)
    348

    Default

    Quote Originally Posted by G00 Proto View Post
    Agreed, vacuum plates are pretty freaking cool. I would certainly invest in one if I had lots of plate work to do... I still would have a deep seated dislike of traditional contour toolpaths and the associated issues, but I would need to come up with a better excuse not to use them

    In many cases, I think I could equal or even slightly improve upon my times using traditional contours, especially on parts like this. I just don't like the un-even tool wear from taking Z steps; the non-uniform tool load as they go into corners and bark; the need to plunge (or ramp) an endmill; the propensity to load up an endmill if the coolant sputters; and as stated earlier, dealing with the loose chunks of remnant that seem to float around the machine enclosure.

    Probably most of all, I just like watching them run. Adaptive toolpaths just look and sound cool. At the end of the day, I'm just a hobbiest that does this because I like it... luckily, my hobby pays the bills
    I do very little ramping and very little plunging if any. I drill a bigger hole where my tool starts. plunging breaks tools.

    I hear you on liking to watch them run when cutting chips, chips hitting the windows and the noise is cool LOL. thats funny on the hobbiest thing I'm in the same boat I love coming into work and making shit. would much rather do that then hit a bar or go home and sit on the couch and look at each other all day. Luckly I got a cool wife she dont want to look at me all day either. so she just works on weekdays at shop and leaves me to have my own time on weekends at the shop.
    here today nice and quiet getting lots done

  17. #14
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,208
    Post Thanks / Like
    Likes (Given)
    4788
    Likes (Received)
    3150

    Default

    It all depends on your machine. Is it capable of high ACCURATE feedrates? If not, then contour.

  18. #15
    Join Date
    Sep 2011
    Location
    Idaho
    Posts
    99
    Post Thanks / Like
    Likes (Given)
    28
    Likes (Received)
    16

    Default

    Just an update because it's the right thing to do... tried both methods and I like adaptive better for many of the reasons you folks stated already. Thanks


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •