Need help - Hogging a large circular pocket in 1045
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 24
  1. #1
    Join Date
    Apr 2017
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    21
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    10

    Default Need help - Hogging a large circular pocket in 1045

    Hey guys, I just got my BP VMC1000/22 up and running after a few weeks of literal crash course in all things CNC. My backround is 10+ years of manual machining, so I'm familiar enough with the basics and theories. But as anyone who's made the transition can attest, cnc speeds/feeds are terrifying (at first) to any manual machinist LOL.

    The part I'm trying to make is in 1045 CRS. Normally, it would be a lathe part, but for my small run, it doesn't make sense to farm out. I acquired the mill for scrap price because people couldn't diagnose a $15 part so I might as well use it for something. Cycle time is the absolute lowest priority, tool life and least amount of junk parts trump all. I have plenty of other things to keep me busy in the shop while the mill hums away.

    I cut this part using an HTC 4 flute 1/2x2 LOC solid carbide mill with flood coolant in a solid holder. Sadly, the length is needed due to part depth and finishing the shaft OD. Speeds and feeds are posted in the attached screenshots which sounded good and didn't chatter. I was rather shocked to see the endmill so destroyed. I'm not remotely opposed to buying some good tooling like this, but I cant afford to kill $100 endmills figuring this part out. A $32 endmill was within the crash course budget. Looking at the mill, it obviously ran hot at the corners despite running in a bowl of coolant. So I know I need to get more heat into the chips instead of the tool.

    A couple thoughts beyond solely stepping up to the 5/8 endmill were - #1 there are .75" holes that go all the way through this part on the same Z axis that I'm working on, so I could drill a hole to drop into and radial out in a morhped pattern with ~.75" DOC and ~.060" radial stepover. #2 was to switch over to a 5/8 rougher or 3/4 indexable end mill for hogging and just use the 5 flute 5/8 for finishing.


    If anyone has any suggestions of what to try or what worked for them, I'm all ears! Thanks guys!













  2. #2
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,355
    Post Thanks / Like
    Likes (Given)
    877
    Likes (Received)
    1451

    Default

    To get max tool life, use a 5/8" EM, predrill, 2D adaptive toolpath, 5% stepover.

  3. #3
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    550
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    190

    Default

    I use the HTC Hotmills everyday in 3/8s and 1/2" on mainly 321 stainless. They cut alloy steels like butter,
    I would rough it all out with a shorter one, use the extended length to finish it.
    also make sure you get those chips out of there its will kill your endmill.

  4. #4
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,018
    Post Thanks / Like
    Likes (Given)
    13662
    Likes (Received)
    10663

    Default

    Looking at the mill, it obviously ran hot at the corners despite running in a bowl of coolant. So I know I need to get more heat into the chips instead of the tool.
    Could that bowl possibly be full of "Re-Cut Chip Soup"???

    That's why you lost your corners. Nothing kills a cutter quicker than re-cutting chips.

    Dry with an air blast. Shorter tools. Only use the long flute stuff when you
    absolutely NEED to.. There is a world of difference in hanging out 2" when its
    all flute, and hanging out 2 inches when 3/4" of that is Solid Shank.

  5. Likes Jashley73, Larry Dickman, Garwood liked this post
  6. #5
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,588
    Post Thanks / Like
    Likes (Given)
    4199
    Likes (Received)
    2755

    Default

    What are your speeds,feeds, d.o.c. and stepover?

  7. #6
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    830
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    362

    Default

    Most of what is needed to be successful has been stated above. You need to understand the theories about it beyond being able to say you were told to do it on the internet.

    Obviously the recut chip soup is self explanatory other than how easily and often it can happen. Chip management in that situation is key as Bob suggested. Look up Minimum Quantity Lubricant and a quick way to set up something similar for this is a mist sprayer turned way down. They sell on Amazon with mag bases.

    From there I suggest you take an hour and watch you tube videos about adaptive milling. Search adaptive milling as well as tricordial milling. Its a world that many machinists know nothing about. There are a lot of videos on it. Look up MQL coolant strategies as well. You tube is your friend.

  8. #7
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,431
    Post Thanks / Like
    Likes (Given)
    1480
    Likes (Received)
    1621

    Default

    ALso I would use a stub flute extended reach endmill to rough, then switch to long flute to finish, even though that is not always needed. You can step down, or spiral down with stub flutes and get acceptable surface finishes. If permissible, a bit of a corner radius helps on the endmill too.

  9. #8
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    830
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    362

    Default

    Quote Originally Posted by Mtndew View Post
    What are your speeds,feeds, d.o.c. and stepover?
    By looking at his toolpaths I'd say horrible is the easiest way to quantify it at this point. No judgement to the OP. He is learning as I did and people here guided me along.

    All joking aside. They are posted in the first and second photo. I don't know exact tool being used but assuming that his EM is typical 1/2 CB EM, his RPMs are low by about 500 rpm, Feed is low by about 10IPM giving him a lower chip load. He also has manual stepover mode checked and its hard to see the actual tool path but it looks like he is working the tip of the mill in heavy step overs with lower speeds and feeds.

    With that said... My opinion and I can't hold a candle to most of you folks here.

  10. #9
    Join Date
    Jan 2009
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    830
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    362

    Default

    Quote Originally Posted by Bobw View Post
    Could that bowl possibly be full of "Re-Cut Chip Soup"???

    That's why you lost your corners. Nothing kills a cutter quicker than re-cutting chips.

    Dry with an air blast. Shorter tools. Only use the long flute stuff when you
    absolutely NEED to.. There is a world of difference in hanging out 2" when its
    all flute, and hanging out 2 inches when 3/4" of that is Solid Shank.
    I'm posting this photo to give a very similar scenario to what BobW is suggesting.

    YouTube

  11. #10
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,749
    Post Thanks / Like
    Likes (Given)
    1246
    Likes (Received)
    3568

    Default

    In addition to what's already been said, use a 5 flute neck em. A short flute length makes a huge difference. A corner radius will help too.

  12. Likes countryboy1966 liked this post
  13. #11
    Join Date
    Oct 2009
    Location
    Oregon
    Posts
    4,085
    Post Thanks / Like
    Likes (Given)
    4385
    Likes (Received)
    2054

    Default

    2" LOC with 1/2 diameter is not going to rough very well.

    I do 90% of my steel milling with 1/2" dia 1.25 loc 4 fl coated carbide with a corner radius. I have a couple step cut long endmills that can step finish well or some big 3/4 and 1" carbide finishers, but those generally aren't in the machines so if I'm making on part I try to use something already in there.

    I found I can slot 3/8" mild steel plate full depth at 60 IPM with a 1/2" 4FL 1/2" LOC. Just have to bolt the stuff down well.

    I usually run 1/2" carbide at 1800 in steel with heavy airblast, no coolant. For heavy cuts and slotting I'll be 30-40 IPM. For high speed toolpaths I'll step over about 15% and run at 100-140 IPM. Finishing in steel I'll leave 005-01 and 20-30 IPM.

    My mills are mostly 25-35 years old so I don't get to try the 500 IPM feedrates

  14. Likes memphisjed liked this post
  15. #12
    Join Date
    Sep 2016
    Country
    UNITED KINGDOM
    Posts
    24
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    2

    Default

    Heres a helical borin macro we use

    %
    :8002( HELICAL BORING )

    ( TOOL DIA D )
    ( BORE DIA B )
    ( RETRACT R )
    ( BORE DEPTH Z )
    ( PITCH U )
    ( FEED F )

    #11 =[#2-#7]/2 ( #2 = B #7 = D )
    #16 =#18-#26 ( #18 = R #26 = Z )
    #17 =#16/#21 ( #21 = U )
    #18 =FUP [#17] ( #18 = R )
    #19 =#26+[#18*#21] ( #19 = Z POSITION )
    #149 =#18
    G0 Z#19
    G91 G1 X#11 F400.
    N1 WHILE [#149GT0 ]DO1
    G3 I-#11 Z-#21 F#9
    #149 =[#149-1]
    END1
    G3 I-#11 F#9
    G0 G91 X-#11
    G0 G90 Z#19
    M99


    This is the program that uses it

    %
    O1000

    M6 T24
    (MSG, 80 MM HELICAL MILL )
    (MSG, HELICAL MILL OUT TO 175 )
    G94 G54 G90 G0 X0. Y0.
    S750 M3
    M16
    ( TOOL DIA D )
    ( BORE DIA B )
    ( RETRACT R )
    ( BORE DEPTH Z )
    ( PITCH U FEED )
    ( FEED F )
    (MSG,80 MM HELICAL BORING TOOL )
    (MSG,ROUGH BORE )

    G43 H24 Z10
    G66 P8002 D80 B175 R3 Z-152 U.5 F1000.
    X0. Y0.
    G67
    G0 Z5. M17
    Z20.
    M5
    M98 P1
    M30
    %

    We use this a lot with 50 or 80 mm helical plunge mill. We have used udrills to do the same thing.
    PS: just be careful as it was taken from our unproven file.
    We use this all the time. Make sure if you are using x100. y100. at the start, you change it to x100. y100. at then end

  16. #13
    Join Date
    Apr 2017
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    21
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    10

    Default

    Thanks for all the pointers guys!!!

    I bought a 5/8"x1.5" altin coated 4 variable flute 30 thou corner rad mill from PCG as suggested by another member here for the roughing. I swore at fusion enough and finally got it to generate an adaptive path for clearing the bulk of the part. Also drilled a 7/8" hole to drop into to save ramping into the part. Set cutting parameters to .970" DOC, .035" stepover, 540sfm/3305rpm, 36in/min feed, and .00274 chip per tooth. Turned off coolant and will use air blast instead. I used kennemetal's calculator for their equivalent 4 flute coated harvi 1 end mill to check numbers against.

    Sound good enough to run?


  17. #14
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,033
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2610

    Default

    i wouldnt start any job without extra end mills.
    .
    and doing small lot or short run jobs it rarely pays to push feeds and speeds and sacrifice reliability. sudden tool failure can damage not only tooling but also the part. feeds and speeds charts are based on short length setups, short tool holders and rigid machines with high hp available and often flood coolant. very common to have feeds and speeds work fine on one machine and setup and work very badly on another machine and setup
    .
    just saying i have used recommended settings and have had end mill get red hot in less than 2 minutes throwing sparks and white hot and melt in less than 4 minutes on recommended settings before. obviously adjust settings to what is happening to your setup

  18. Likes Bobw liked this post
  19. #15
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,431
    Post Thanks / Like
    Likes (Given)
    1480
    Likes (Received)
    1621

    Default

    Quote Originally Posted by Whitbread View Post
    Thanks for all the pointers guys!!!

    I bought a 5/8"x1.5" altin coated 4 variable flute 30 thou corner rad mill from PCG as suggested by another member here for the roughing. I swore at fusion enough and finally got it to generate an adaptive path for clearing the bulk of the part. Also drilled a 7/8" hole to drop into to save ramping into the part. Set cutting parameters to .970" DOC, .035" stepover, 540sfm/3305rpm, 36in/min feed, and .00274 chip per tooth. Turned off coolant and will use air blast instead. I used kennemetal's calculator for their equivalent 4 flute coated harvi 1 end mill to check numbers against.

    Sound good enough to run?

    Can't speak to your software, but if you are using an adaptive path and it is indeed doing it correctly, you *should* up your feed for the chip thinning effect, if your setup is rigid enough. I would be at least .005"ipt, but again rigidity will be the biggest factor here.

    ++ on using air blast!

  20. Likes Bobw liked this post
  21. #16
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    387
    Post Thanks / Like
    Likes (Given)
    126
    Likes (Received)
    216

    Default

    Quote Originally Posted by Mike1974 View Post
    Can't speak to your software, but if you are using an adaptive path and it is indeed doing it correctly, you *should* up your feed for the chip thinning effect, if your setup is rigid enough. I would be at least .005"ipt, but again rigidity will be the biggest factor here.

    ++ on using air blast!
    He did say time was not an issue, but I'm not sure where the crossover point of taking it easy on the tool and wearing out tooling from rubbing would be.

  22. #17
    Join Date
    Aug 2010
    Location
    Minnesota
    Posts
    1,984
    Post Thanks / Like
    Likes (Given)
    150
    Likes (Received)
    1464

    Default

    Long shot but this isn't Matt Whitbread is it? Sorry not contribute to your question just curious hahaha

  23. #18
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,018
    Post Thanks / Like
    Likes (Given)
    13662
    Likes (Received)
    10663

    Default

    I'll second, or third the motion that you need to up your feed rate a bit.

    a 5/8 endmill at a .035 stepover. Your chip thickness multiplier is
    about 2.2, so your chip is really only about .001"..

    I'm not one that believes every chipload needs to be huge, but
    you are getting to that point of "Rubbing", and except for
    re-cut chip soup, nothing burns an endmill up quicker than
    far too small of a chipload.

    As for knowing what your actual chip thickness is, I've got a handy
    little chart on the wall behind my computer.. I have no idea where
    it came from and I can't find it on line again. I should
    just take a pic and post it.

    There are also handy little calculators out there for a few bucks
    that go on your phone.

  24. #19
    Join Date
    Apr 2017
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    21
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    10

    Default

    First part was a success! I'll bump the feed to 45 in/min for the next one per the suggestions. Chips looked good and mill sounded great on this part.

    Thanks again guys!


  25. Likes lastrada, Bobw, memphisjed, Garwood, Mtndew and 1 others liked this post
  26. #20
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,018
    Post Thanks / Like
    Likes (Given)
    13662
    Likes (Received)
    10663

    Default

    What size are the lug studs that press into those holes????


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
  •