Breaking 1/2" Kennametal HARVI I TE ENDMILL while plunging
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 51
  1. #1
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    28

    Default Breaking 1/2" Kennametal HARVI I TE ENDMILL while plunging

    I have a 1/2" Kennametal HARVI I TE endmill in a live tool position on an Emco 365MC lathe. I am short on positions/holders in the turret so want to use this endmill to plunge (i.e., drill) the end of a 4140 part before boring an id. Kennametal has a video demo of the tool showing it plunge/drill 4140 at 1.5D (1.5" deep). They give F&S as 590 SFM, 4500 RPM, .002 IPT. (video is here: HARVI™ I TE - The Magic Solid End Mill From Kennametal - YouTube)

    My turret live tools max out at 4000 RPM so 0.002 IPT (4 flute) at 4000 rpm is 32 IPM. Which is 0.008" IPR.

    I set my F&S to 3000 RPM, 0.006 IPR (thought I was being a little conservative) and plunged in to a depth of 0.25" with coolant on. Seemed to be going ok at the start but about 1/8" in the endmill stalled. I immediately hit reset (stop) backed the EM out and see I broke two flutes off the end of the endmill. Not really sure why this was a problem or what F&S I should be using?

    -Tom

  2. #2
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,710
    Post Thanks / Like
    Likes (Given)
    287
    Likes (Received)
    1924

    Default

    Those Kennametal parameters seem pretty "Magical" indeed, in 4140. Not saying it can't be done, but I do think everything has to be totally squared away -- toolholding, workholding, everything.

    Live tool isn't the most rigid, AFAIK, so there is one problem.

    Coolant may be hurting you -- the thermal shock may cause microchipping which leads to macrochipping. The demo shows the tool doing this dry, maybe try that?

    BTW, "1.5D" doesn't mean 1.5" deep, it means 1.5 times the diameter, so 3/4".

    Regards.

    Mike

  3. #3
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    28

    Default

    Quote Originally Posted by Finegrain View Post
    Those Kennametal parameters seem pretty "Magical" indeed, in 4140. Not saying it can't be done, but I do think everything has to be totally squared away -- toolholding, workholding, everything.

    Live tool isn't the most rigid, AFAIK, so there is one problem.

    Coolant may be hurting you -- the thermal shock may cause microchipping which leads to macrochipping. The demo shows the tool doing this dry, maybe try that?
    So for a live tool that isn't as rigid as one might like does slowing the feed rate help compensate? I don't want to rub either so I am always hesitant to go slow but not sure where the transition is between cutting and rubbing...

    Hmm, I suppose coolant causing the failure is possible, but I don't think I want to wager a another tool on that fixing the problem!

    Quote Originally Posted by Finegrain View Post
    BTW, "1.5D" doesn't mean 1.5" deep, it means 1.5 times the diameter, so 3/4".

    Regards.

    Mike
    Yes, you are right, thanks for that correction.
    -Tom

  4. #4
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    10,893
    Post Thanks / Like
    Likes (Given)
    640
    Likes (Received)
    8742

    Default

    Video is a VMC. How much HP in your live tool?

  5. #5
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,547
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    973

    Default

    Sometimes when you watch videos like that your bullshit meters pegs out. You know that shit is not possible but maybe 1 time and the next time in it’s toast but hey it was in the video.
    Don


    Sent from my iPhone using Tapatalk Pro

  6. Likes Bobw, Ox, empwoer, Radar987, doug925 and 1 others liked this post
  7. #6
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    241
    Post Thanks / Like
    Likes (Given)
    622
    Likes (Received)
    69

    Default

    You can't treat the live tool of a lathe as if it is the same as milling in a VMC. It's nowhere close. I am not surprised that the spindle stalled with a 1/2" endmill trying to just plunge 3/4" in 4140.

  8. Likes Winterfalke liked this post
  9. #7
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    28

    Default

    Quote Originally Posted by CarbideBob View Post
    Video is a VMC. How much HP in your live tool?
    I believe the live tool is 9 HP.
    -Tom

  10. #8
    Join Date
    May 2020
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    Why not try some helical interpolation using the C axis? Make a bigger hole or use a smaller tool to make the hole. You should be able to ramp at 10-15 degrees if the machine can handle it. Endmills are much better at making holes this way than drilling.

  11. Likes charlie gary liked this post
  12. #9
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    28

    Default

    Quote Originally Posted by Nagol View Post
    Why not try some helical interpolation using the C axis? Make a bigger hole or use a smaller tool to make the hole. You should be able to ramp at 10-15 degrees if the machine can handle it. Endmills are much better at making holes this way than drilling.
    That is plan B. But the endmill is supposed to be able to do this. Perhaps the machine cannot, but I’d like to get it to work if possible….

  13. #10
    Join Date
    May 2020
    Country
    UNITED STATES
    State/Province
    Indiana
    Posts
    52
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    Even if you get it to do it tool life would most likely be better interpolating. At the least a lot of pecking may be in order.

  14. #11
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    1,296
    Post Thanks / Like
    Likes (Given)
    935
    Likes (Received)
    517

    Default

    How does the first 1/8” look? Is it all chattery? Maybe do another one only going .100” into it so you can examine the part to see what the surface finish looks like. If it’s all chattery and ugly you know rigidity is a problem. How big is the part and how far is it sticking out? What are you holding the 1/2” em in? ER20?

    Good luck!

  15. #12
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    28

    Default

    Quote Originally Posted by Nerdlinger View Post
    How does the first 1/8” look? Is it all chattery? Maybe do another one only going .100” into it so you can examine the part to see what the surface finish looks like. If it’s all chattery and ugly you know rigidity is a problem. How big is the part and how far is it sticking out? What are you holding the 1/2” em in? ER20?

    Good luck!
    I’ll look at it more closely today but it looked pretty good while I was picking out the carbide chips. The part is a 3” dia, 3” lg round and is sticking out only about an inch. The live holder uses a ER25 collet.
    -Tom

  16. #13
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    28

    Default

    Attached are some images of the hole and setup. Surface finish isn't great but I don't see signs of horrible chatter...

    img_2007.jpg
    img_2010.jpg
    img_2024.jpg
    img_2027.jpg
    img_2033.jpg

  17. #14
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    28

    Default

    After talking with pcasanova (who has the same machine) and looking at the machine specs I am pretty sure the problem I encountered is the torque limit on the VDI-30 live tool holders in my machine. The spindle on the live tools is 9HP but it is torque limited so as to not break the gearing/spindles that drive the tool holders. The specs say the Torque is only 12 lb-ft. For the main spindle it is 141 lb-ft! If you crash a live tool a clutch disengages (done that a couple times). I think I was able to hit reset when I saw the endmill stall just before the clutch let go.

    I suspect I will need to slow my feed and/or ramp/spiral the hole to keep the torque down.

    -Tom

  18. #15
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    241
    Post Thanks / Like
    Likes (Given)
    622
    Likes (Received)
    69

    Default

    Any reason why you are not using an insert drill for that hole?

  19. #16
    Join Date
    Jul 2015
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    222
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    82

    Default

    Why not drill and bore with an indexable drill? Those videos are always done on a 50 taper and probably switch the endmill out after every cut.

  20. Likes Bobw, Garwood liked this post
  21. #17
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    176
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    28

    Default

    Quote Originally Posted by Fancuku View Post
    Any reason why you are not using an insert drill for that hole?
    Two reasons. I don’t have one :-) , and I only have so many tool positions and live toolholders. I was hoping to have an endmill do double duty…..
    -Tom

  22. #18
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    241
    Post Thanks / Like
    Likes (Given)
    622
    Likes (Received)
    69

    Default

    Quote Originally Posted by MaxPrairie View Post
    Those videos are always done on a 50 taper and probably switch the endmill out after every cut.
    Too many people have watched the Titans of CNC videos on youtube and think that his bullshit is real.

  23. Likes cgrim3, empwoer liked this post
  24. #19
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,547
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    973

    Default

    Put a tool block on the turret that holds 2 drill bits and go to town
    Don


    Sent from my iPhone using Tapatalk Pro

  25. #20
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,547
    Post Thanks / Like
    Likes (Given)
    233
    Likes (Received)
    973

    Default

    here you go like this
    Don


    Sent from my iPhone using Tapatalk Pro

  26. Likes empwoer, Garwood liked this post

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
  •