Trochoidal milling and other milling technique paths
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 27
  1. #1
    Join Date
    Jan 2010
    Location
    FL,USA
    Posts
    673
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    49

    Default Trochoidal milling and other milling technique paths

    What is every bodies opinion on trochoidal milling? I personally don't like it for the 2 facts of your engaged 50% of the time in th cut and every time you come engage into the cut you have a spike in stress when the cut is entered.

    For a pocket about 3.25" length and 1.375 in width and .750" depth in 4140 steel what is every bodies opinion on the best milling pocket?

  2. #2
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    11,523
    Post Thanks / Like
    Likes (Given)
    48
    Likes (Received)
    8784

    Default

    Trochoidal is usually faster, and usually easier on tooling. What's not to like?

    Who cares if you have a spike in stress? If the end mill doesn't break, you're fine. This a roughing tool path.


    Some old machines can't handle these paths. They don't have the memory, block speed, or feed rates to make it viable. Anything built in the last 20 years should be fine.

  3. #3
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,784
    Post Thanks / Like
    Likes (Given)
    2759
    Likes (Received)
    2410

    Default

    with the right speeds feeds DOC's and angle of engagement, they can be very efficient. i dont use troch paths exclusivley, but i do use a lot of the dynamic milling cycles in my cad software. awesome stuff.

  4. #4
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,731
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2526

    Default milling paths

    Quote Originally Posted by MBG View Post
    What is every bodies opinion on trochoidal milling? I personally don't like it for the 2 facts of your engaged 50% of the time in th cut and every time you come engage into the cut you have a spike in stress when the cut is entered.

    For a pocket about 3.25" length and 1.375 in width and .750" depth in 4140 steel what is every bodies opinion on the best milling pocket?
    .
    if you have a machine where you do 100% conversational programming at the machine and it does not come with trochoidal milling then you have little choice. most older machines just use the biggest shortest length cutter and with raw power the most they can at a time. for pockets we drill a hole and let end mill down into pocket short 0.014" for finish cut and just cut it with 1" end mill at 0.250 to 0.375 depth of cut. shorter the end mill the more depth of cut you can do at higher sfpm and feed.
    .
    99% of the time you can program at machine in 30 seconds at start cutting and finish it by the time you even have it on a computer to even start programming it on a computer with cam software

  5. #5
    Join Date
    Apr 2013
    Location
    Oregon
    Posts
    188
    Post Thanks / Like
    Likes (Given)
    202
    Likes (Received)
    144

    Default Trochoidal milling and other milling technique paths

    I agree with the above posts, what's not to like? We also don't use it exclusively on every part but when we do, the results are fantastic. We machine a lot of 13-8, 15-5, and 17-4 heat treated stainless. We've made the same parts for over 10 years. Honestly we have been able to double our output in those years. Yes machines and tooling have contributed to that but new milling techniques have been the biggest reason for the increased output. The short in and out rapid, cutting air moves used to bug me but its a non issue once you can get over it!

  6. #6
    Join Date
    May 2004
    Country
    UNITED STATES
    State/Province
    California
    Posts
    2,474
    Post Thanks / Like
    Likes (Given)
    863
    Likes (Received)
    1565

    Default

    Quote Originally Posted by DMF_TomB View Post
    99% of the time you can program at machine in 30 seconds at start cutting and finish it by the time you even have it on a computer to even start programming it on a computer with cam software
    You have to keep in mind that not everybody makes the same types of parts. By your statement, you are making incredibly simple parts. That's not what I make, and I can tell you that HSM saves me a LOT of time, even considering programming time, which really isn't any different for me since the parts I tend to make can not be hand programmed efficiently or at all. Not to mention tooling costs drop substantially via extended life with HSM.

  7. Likes John Welden, dylskee, gregormarwick liked this post
  8. #7
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,274
    Post Thanks / Like
    Likes (Given)
    841
    Likes (Received)
    1352

    Default

    Quote Originally Posted by MBG View Post
    For a pocket about 3.25" length and 1.375 in width and .750" depth in 4140 steel what is every bodies opinion on the best milling pocket?
    An HSM path will allow you to cut the pocket full depth with a cheap 1/2" endmill and spread the wear evenly over 3/4" of flute length.

    Trochoidal loops only account for a portion of the HSM path, so the 50% engagement is only true part of the time.

  9. #8
    Join Date
    Feb 2004
    Location
    Napa, CA
    Posts
    2,589
    Post Thanks / Like
    Likes (Given)
    43
    Likes (Received)
    687

    Default

    Quote Originally Posted by MBG View Post
    I personally don't like it for the 2 facts of your engaged 50% of the time in th cut ....
    An efficient trochoidal program should spend far more of the TIME in the cut, the loop backs should be done at very high speed slowing down only for the cutting portion. I might be cutting 100 ipm in the cut, but the loop around might be programmed at 700 ipm. If equal distances, that's 87% of the time in the cut.

  10. Likes gregormarwick liked this post
  11. #9
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,116
    Post Thanks / Like
    Likes (Given)
    88
    Likes (Received)
    422

    Default

    At 3/4 depth its called not HSM, but HEM - high efficiency milling.
    Get a 1/2" cheapo endmill and cut 1/4" stepover full depth of cut.
    You only need a proper toolpath (Trumeill,Volumill,DynamicMilling )that controls the Tool Engagement Angle and prevents tool from burying up.
    Generally its safe to assume that sidecuttimg endmill will take out as much material cross section as slotting.
    So calculate stepover accordingly.
    Ie you can slot 3/8" deep with a 1/2" HPEM.
    For 3/4 deep pass your WOC can to be atleast 1/4"

  12. #10
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,731
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2526

    Default simple parts

    Quote Originally Posted by [email protected] View Post
    You have to keep in mind that not everybody makes the same types of parts. By your statement, you are making incredibly simple parts. That's not what I make, and I can tell you that HSM saves me a LOT of time, even considering programming time, which really isn't any different for me since the parts I tend to make can not be hand programmed efficiently or at all. Not to mention tooling costs drop substantially via extended life with HSM.
    .
    yes i make mostly simple parts using conversational programing Cam software that comes with a Mazak CNC VMC. It is designed with cycles or toolpaths that 99% of the time is the same as what Cam software on a computer will do. It is designed to be easy and fast to program at the machine. describe shape and roughing depth and width and finish passes are automatically setup. it also shows tool path simulations in multiple views. basically it is a Cam option that is built into controller and purchased with the machine
    .
    in general learning from others using the machine from decades of use is to use the biggest cutter possible and with a 20 hp machine the chips come off quick at 20 - 50 ipm especially using big dia cutters.
    .
    we resharpen our cutters so a 1" carbide end mill at $300 is reused at least 3-10 times so cost is closer to $50 each 60 minutes of use and thats a lot of cubic inches per minute removed. normally if possible i use at least a 2" carbide insert end mill at 0.25" DOC going 20-40 ipm or a 4 or 5" dia facemill at 0.150" DOC going 20-50 ipm. like i said raw hp can make up for a lot is as i found out as i tried what others have used successfully for decades and found out it works pretty good.
    .
    if the older Mazak controller came with trochoidal cycles i would use them. it does come with many cylces like pockets with steps (islands) etc and many many other cycles. it does take time learning them similar to learning any Cam software it just happens to be built into the control and is a one time purchase.
    .
    the mazak also will do 3d shapes. for example it can do a beveled edge with a ball end mill. the 3d cam package that came with it is little used as we do simple parts but i know it can also do swept, revolved and other 3d shapes.

  13. #11
    Join Date
    Jan 2010
    Location
    FL,USA
    Posts
    673
    Post Thanks / Like
    Likes (Given)
    54
    Likes (Received)
    49

    Default

    Quote Originally Posted by swarf_rat View Post
    An efficient trochoidal program should spend far more of the TIME in the cut, the loop backs should be done at very high speed slowing down only for the cutting portion. I might be cutting 100 ipm in the cut, but the loop around might be programmed at 700 ipm. If equal distances, that's 87% of the time in the cut.
    I don't know what kind of machine you have but that would never slow down in time for the next cut..??

  14. #12
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,950
    Post Thanks / Like
    Likes (Given)
    13136
    Likes (Received)
    10312

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    in general learning from others using the machine from decades of use is to use the biggest cutter possible and with a 20 hp machine the chips come off quick at 20 - 50 ipm especially using big dia cutters.
    The "thats how we've always done it" excuse.

    I've spent a lot of time finger banging some 3 axis Mazatrol. Its handy for simple holes, and simple parts, beyond that, its really pretty crappy.
    Its really a 2axis interface trying its best to work in a 3D work space.
    I'd say its perfectly fast and functional for 25% of parts (in my experience), the rest.. hello CAM.

    You don't need a big cutter to pull big HP #s. I was screwing around with some high speed type paths a few months ago, annealed
    4140. I figure my spindle is rated 22.5hp for 15(or is it 30) minutes. So ignoring the fact that I know it will start to bog at
    23 cubic inches a minute(old spindle drive), I shot for 27. Ended up backing it down into the 18 cubic inch a minute range, I
    didn't get to play much, only had 6 parts to do, and that is with a 1/2" $50 endmill.

    I too was taught, biggest cutter, on the manual mills with R8's that meant 3/4" tooling all the time, when I got into the world
    of real machines, it was still biggest cutter...

    I've completely changed my tune on that. Why use a big $150 cutter when I
    can simply change the way I attack a part (more efficient tool paths and use of the endmill),
    use a much cheaper and smaller cutter and get insane amounts of tool life, and get the parts out the door quicker.

    I apparently haven't ordered any tools since January, and we've been moving a good bit of metal, 13-8 304 4140, 4340 etc..
    And apparently I didn't even need the tools I ordered then, and it was only 8 endmills, 2 of which are still in the package.

    From January 17th.
    Hi Curtis.

    I need some APKTs, 16mm.

    3 boxes, Whatever will work well in 4140 and 4340 at around a 38-40C.

    All the other stuff showed up Monday and Tuesday, just in time... BUT the tools I already had were so damn good I didn't even need them.
    1/2" Titan, previously used, then chewed on 304 for 2 days, then still pulled out 300pounds of 4140 at 900sfm and 150ipm before calling it quits.
    Really quite amazing what going at a part in a slightly non-conventional/more modern way can accomplish. Crazy metal removal and crazy tool life.

    I'm sure I could have gone a little faster and eaten up a bunch more tools, but I always try to find that magic sweet spot. Basically just
    a stable process that I can leave running and not worry about.

  15. #13
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,731
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2526

    Default Mazak

    Quote Originally Posted by Bobw View Post
    The "thats how we've always done it" excuse.

    I've spent a lot of time finger banging some 3 axis Mazatrol. Its handy for simple holes, and simple parts, beyond that, its really pretty crappy.
    Its really a 2axis interface trying its best to work in a 3D work space.
    I'd say its perfectly fast and functional for 25% of parts (in my experience), the rest.. hello CAM.
    .
    the Mazatrol Cam can do a lot if you know how to use it. I read how expensive Cam software will slow feed in corners. Like that is basic parameter in a Mazak to automatically slow feed in corners and it can be adjusted from original 70%
    .
    my point is Cam software is expensive and if purchased upgrades are done every 3 years that adds up. If Cam software is $10,000 or more thats a lot of cutting tools that could have been purchased not to mention the time wasted by a lot of machinist who prefer sitting at a computer rather than standing at a CNC running it.

  16. #14
    Join Date
    May 2010
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    443
    Post Thanks / Like
    Likes (Given)
    123
    Likes (Received)
    296

    Default Trochoidal milling and other milling technique paths

    I'm really kicking myself, I should have bought cutters, not software.

  17. #15
    Join Date
    May 2010
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    443
    Post Thanks / Like
    Likes (Given)
    123
    Likes (Received)
    296

    Default Trochoidal milling and other milling technique paths

    And I should be standing, not sitting. Man, I'm doing everything wrong.

  18. #16
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,731
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2526

    Default

    Quote Originally Posted by cellardoor7 View Post
    I'm really kicking myself, I should have bought cutters, not software.
    .
    software costs money. a Mazak is designed to run making parts AND allowing programming at the same time. like i said too many machinist prefer sitting down at a computer with Cam software rather than making parts at a CNC and programming at the CNC at the same time.
    .
    the Mazak Cam built into control can do a lot even 20 years old. newer CNC machines are starting to come with built in Cam software that inports Cad files like DXF and others. if a company spends $70,000+ on software over 20 years most would say it is worth it paying an extra $10,000 to have it built into the CNC control and never have to purchase upgrades every 3 years.
    .
    reading about feed reduced cutting in corners is standard and automatically reduced on the mazak (and amount can be adjusted)and even the angle considered a corner (<135 degrees) is adjustable.
    .
    sometimes you have to take what salesman say trying to sell you stuff with a little a grain of salt. that is you have to tell the bullshit from the truth and that is not always easy to do.

  19. #17
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,731
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2526

    Default

    Quote Originally Posted by cellardoor7 View Post
    And I should be standing, not sitting. Man, I'm doing everything wrong.
    .
    use a chair (stool or higher type) at the CNC control at the machine thats making parts while you are also programming if you really want to sit.

  20. #18
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,731
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2526

    Default

    the 20 year old mazak vmc i run comes with over 1000 pages of manuals not too much different that the pdf file manuals that come with a lot of cam software.
    .
    i don't claim to be a mazak expert with only 1 year of mazak experience (30 yrs experience on other machines) but the more i read on programming it the more i recognize it comes with cam software built in and that it is asking for the same info any other cam software would be asking.

  21. #19
    Join Date
    May 2010
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    443
    Post Thanks / Like
    Likes (Given)
    123
    Likes (Received)
    296

    Default Trochoidal milling and other milling technique paths

    Even if you were standing on top of the 1000 page manual, you could not make anything I make finger banging your 20 year old mazak.

  22. Likes allloutmx, jrmach liked this post
  23. #20
    Join Date
    May 2010
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    443
    Post Thanks / Like
    Likes (Given)
    123
    Likes (Received)
    296

    Default Trochoidal milling and other milling technique paths

    To imply that PC based cam is unnecessary is absurd.

  24. Likes dstryr liked this post

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
  •