Cutting hard steels...
Close
Login to Your Account
Page 1 of 4 123 ... LastLast
Results 1 to 20 of 66
  1. #1
    Join Date
    Aug 2013
    Location
    Chandler, AZ
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    127

    Default Cutting hard steels...

    What feeds/speeds/tools/woc/doc/rpm/etc to you use? Tried my first cuts in hardened steel today and I'm pretty excited. I know my speeds and feeds were probably way off but this is something I would like to learn if at all possible from this forum. (even though I have no real need to cut lots of hardened steel)

    Feel free to criticize away!

    Okuma Genos M560-V with Volumill (hardened steel) - YouTube

  2. #2
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    5,105
    Post Thanks / Like
    Likes (Given)
    642
    Likes (Received)
    1016

    Default

    What material and just how hard is it?

  3. #3
    Join Date
    Aug 2013
    Location
    Chandler, AZ
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    127

    Default

    very good question most likely not that hard.

    its one of the vise jaws from orangevice, on their site looks to be 4140 Semi-Hard.

    I'm pretty interested in learning the hardness of steels what makes them hard, how to cut them etc...This is where im very green.

  4. #4
    Join Date
    Nov 2011
    Location
    Maryland, USA
    Posts
    231
    Post Thanks / Like
    Likes (Given)
    81
    Likes (Received)
    21

    Default

    When I was doing my first 4140 pH machining not too long ago utilizing info and support from the cutting companies was useful. Sandvik, horn, and sgs all had pretty good tech support

  5. #5
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    11,230
    Post Thanks / Like
    Likes (Given)
    41
    Likes (Received)
    8478

    Default

    Something is horribly wrong. You should not be seeing sparks. Sparks mean your RPMs are too high for the feedrate you are using.

    With good HSM tool paths and coated end mills, you can run 4140 HT pretty aggressively.

    I would run about 800 SFM, and at least .006 per tooth feed, 10% step over at 2XD. I run a 1/2" 4 flute HTC variable flute with TiAlN coating at 5800 RPM, 180IPM, and .05 step over.

  6. Likes Danthemann liked this post
  7. #6
    Join Date
    Aug 2013
    Location
    Chandler, AZ
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    127

    Default

    Guess I got lucky then

    11459rpm
    30ipm
    20% step over at 1x diameter
    .250" endmill 3 flute (its all I have on hand at the moment)
    put me at 750sfm and .001307 ipt

    So I was way off. Endmill is still sharp and the surface finish looks great. Ill have to pick up some 4140HT and some better endmills and make something.

  8. #7
    Join Date
    Dec 2007
    Location
    N.E. oHIo, USA
    Posts
    2,359
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1369

    Default

    Looks like a plasma cutter!


    Rex

  9. #8
    Join Date
    Jan 2013
    Location
    Louisville, KY
    Posts
    2,884
    Post Thanks / Like
    Likes (Given)
    6665
    Likes (Received)
    2422

    Default

    First up, 4140 at 40ish isn't hard. D2 at 62hrc is hard...

    Second, like Ewsley said, something is way wrong there. If what you are cutting is actually 4140, it shouldn't be too tough to cut. It is tougher than 1018 sure, but still plenty doable.

    You know, Sol (orange vise) is a member here. A quick PM to him about his jaws will get you much more reliable info than just guessing...

  10. #9
    Join Date
    Aug 2013
    Location
    Chandler, AZ
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    127

    Default

    Sol is a busy guy, I hate to bother him. I just needed a step milled and I accomplished this on 2 jaws without any broken bits. Next go around Ill know what im cutting and do a little better diligence before cutting.

    Back to cutting aluminum for me!

  11. #10
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,111
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    417

    Default

    Quote Originally Posted by Jashley73 View Post
    First up, 4140 at 40ish isn't hard. D2 at 62hrc is hard...

    Second, like Ewsley said, something is way wrong there. If what you are cutting is actually 4140, it shouldn't be too tough to cut. It is tougher than 1018 sure, but still plenty doable.

    You know, Sol (orange vise) is a member here. A quick PM to him about his jaws will get you much more reliable info than just guessing...
    Do you mean to say that D2 at 42rc would still be harder than 4041 at 42rc?
    Other than that i agree with everything you have said.
    In one of his last vids Sol is cutting his jaws and no sparks are seing there.
    Like everyone said too many sparks for 40 -ish RC steel.

  12. #11
    Join Date
    Aug 2013
    Location
    Chandler, AZ
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    17
    Likes (Received)
    127

    Default

    yep yep my speeds/feeds were all in the wrong place. way too big of a cut.

  13. #12
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,111
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    417

    Default

    Imo the chipload was ok for a 1/4" endmill. Tis why it did not break.
    But the sfm should have been around half of what you used.

    But hey, it worked fine, right? Then you were not wrong!

  14. #13
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,215
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2389

    Default

    depends on shape of what you are cutting. if it is easier to endmill rather than side mill then i would try
    200-300sfpm
    DOC low 0.005 to 0.030"
    Feed low at 0.001 to 0.003" ipt
    ........it has been my experience a hard steel will overload carbide and chip the corners away unless you reduce cutting load in particular DOC and Feed. I have cut hard steel dry and with coolant. If cutting dry the part can heat up and loose its hardness. i have seen many end mills nearing dullness throw sparks and glow red to orange. eventually they get hotter and hotter and part will turn blue (over 600 F). many hardened steels start to loose hardness at 400 F when they turn straw color.
    ....... i have cut hard steel with 3/4" dia carbide end mills and 2" dia cutter with carbide inserts. it is my belief the larger diameter helps cut faster compared to a smaller diameter cutter. i have cut a lot of parts with 60 Rockwell C scale case hardened parts. as long as you ease up on DOC and Feed it cuts relatively easy. I don't claim to be a expert but i have cut many dozens of hardened steel parts before.

  15. #14
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,077
    Post Thanks / Like
    Likes (Given)
    3582
    Likes (Received)
    2366

    Default

    If it's a vise jaw, I would guess that it's hardened to about 50-52 Rc.
    Even at that hardness, you shouldn't see a fireworks show.

  16. Likes Laurentian liked this post
  17. #15
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,200
    Post Thanks / Like
    Likes (Given)
    810
    Likes (Received)
    1280

    Default

    Our jaw plates are 4140 hardened to around 50 Rc.

    With HSM tool paths at 5% stepover for a 1/4" EM, try 300SFM and 0.004 IPT programmed feedrate for starters.

    -Sol

  18. #16
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    7,511
    Post Thanks / Like
    Likes (Given)
    708
    Likes (Received)
    1820

    Default

    Quote Originally Posted by vwfullcup View Post
    Guess I got lucky then

    11459rpm
    30ipm
    20% step over at 1x diameter
    .250" endmill 3 flute (its all I have on hand at the moment)
    put me at 750sfm and .001307 ipt

    So I was way off. Endmill is still sharp and the surface finish looks great. Ill have to pick up some 4140HT and some better endmills and make something.
    If that end mill still looked sharp after that fireworks display, I'd stick with those mills.

  19. #17
    Join Date
    Jan 2010
    Location
    Gilroy CA
    Posts
    4,314
    Post Thanks / Like
    Likes (Given)
    3102
    Likes (Received)
    2338

    Default

    Quote Originally Posted by Dave K View Post
    If that end mill still looked sharp after that fireworks display, I'd stick with those mills.
    Or get some new glasses

  20. Likes wrustle, evansmachine, Dave K, ihbuilder, NTM and 5 others liked this post
  21. #18
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    6,732
    Post Thanks / Like
    Likes (Given)
    290
    Likes (Received)
    5495

    Default

    Quote Originally Posted by Orange Vise View Post
    Our jaw plates are 4140 hardened to around 50 Rc.
    ....
    -Sol
    Thanks for real numbers.
    That would make much more sense than Semi-Hard, pH, or HT and would explain the "light show".
    One would expect a decent 4140 vise jaw to be in the low 50s.
    I'd start at 200-300 SFM here with TiALn, 60-80 uncoated, 100-150 with Tin.
    I'd also be in a C-5, C-6 tool but most off the shelf stuff nowadays is C-2 micro and the work is done with the coating.
    Thermal cracking is going to be a big problem and the extra TaC will help along with the hardness from the added TiC (which is why these are steel cutting base grades).

    The OP should at least invest in some hardness files so that he has some idea of what he is working in.

    The tool may still look "sharp", not much cutting time and don't know what the OP is using for a microscope.
    When it does begin to fail it is going to go to poop very,very fast. Probably much quicker than you can get to the big red button.
    Bob

  22. #19
    Join Date
    Feb 2011
    Location
    Grant Alabama USA
    Posts
    610
    Post Thanks / Like
    Likes (Given)
    173
    Likes (Received)
    216

    Default

    I have made quite a few specialty jaws from standard kurt vise jaws. For a 1/2" endmill 300sfm and .003 ipt with .02 radial works great. Hsm style machining without the high speed makes the endmills last. The trick is to limit the cutters exposure to heat. Also, sparks = bad is not always correct. It depends on the cutter, material, speeds and feeds and coating.

  23. #20
    Join Date
    Mar 2011
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    633
    Post Thanks / Like
    Likes (Given)
    240
    Likes (Received)
    245

    Default

    And I thought the 4th and Fireworks were in July


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
  •  
2