First try on D2 62Rc(video)
Close
Login to Your Account
Page 1 of 3 123 LastLast
Results 1 to 20 of 44
  1. #1
    Join Date
    Feb 2011
    Location
    Grant Alabama USA
    Posts
    599
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    214

    Default First try on D2 62Rc(video)

    In an effort to perfect our speeds and feeds while hardmilling, this is the first try. Its not right yet, but far from a failure. I apologize for the language at the end, but I do not edit my videos. The endmill was a reground garr VRX at .353 diameter. Parameters were 750 sfm, .018 radial, .300 axial and .004 ipt.
    The next run will be at 650 sfm, .006 ipt using a mist sprayer. Also, any small areas will be blocked off to be ran at lower speeds to allow cooling time for the cutter. Just a note for anyone using a Mag Fadal, The E-stop button is not quick enough, use feed hold. The endmill was badly worn on the corners, but not broken, and will be resharpened and used again.


    Hsm on heat treated D2 - YouTube

  2. Likes jdj, solidworkscadman liked this post
  3. #2
    Join Date
    Feb 2003
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    4,728
    Post Thanks / Like
    Likes (Given)
    3706
    Likes (Received)
    1452

    Default

    Nice vid!

    Your Fadal seems to move pretty good. Is it a FX with Fanuc control?

  4. Likes jdj liked this post
  5. #3
    Join Date
    Jul 2013
    Location
    Indianapolis
    Posts
    62
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    9

    Default Re: First try on D2 62Rc(video)

    Why not use a ceramic insert cutter?

  6. #4
    Join Date
    Jun 2006
    Location
    Near Seattle
    Posts
    4,213
    Post Thanks / Like
    Likes (Given)
    2140
    Likes (Received)
    965

    Default

    A general question (maybe there's a good thread on this somewhere) - how to decide where flood coolant is and is not a good idea? Is air blast always suitable when flood coolant is not?

    It would be nice to see a closeup of the resulting part, if allowed.

  7. Likes jdj liked this post
  8. #5
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,133
    Post Thanks / Like
    Likes (Given)
    756
    Likes (Received)
    1196

    Default

    Quote Originally Posted by bryan_machine View Post
    A general question (maybe there's a good thread on this somewhere) - how to decide where flood coolant is and is not a good idea? Is air blast always suitable when flood coolant is not?
    When milling low carbon or annealed alloy steel, the flood coolant threshold is typically around 300 SFM on an inserted cutter. That's when the cutting edge gets too hot and thermal shock from flood coolant can damage the cutting edge. This threshold lowers as the cutting edge dulls. The threshold can also change significantly depending on material hardness and cutter geometry, so it's best to gage cutting zone temperature by chip color. When chips start changing color from silver to bronze, it's time to turn off the coolant. When chips are blue/purple, it's just about guaranteed that flood coolant will damage the carbide.

    Fresh, solid carbide endmills with HSM toolpaths can cut much faster than 300SFM without generating much heat, but most folks will crank up the speed and turn off the coolant anyway. High feed mills also generate less heat.

    Air blast is optional. Its primary purpose is clear chips to prevent recutting. During long, dry cycles, air blast can also significantly cool the toolholder body. We machine hardened materials on a regular basis and air blast will keep the toolholders around 100 degrees F, compared to 150+ without the air blast. Good for the spindle and good for holding tolerance. Makes no difference to cutter life, however.

    -Sol

  9. Likes John Welden, Nick Mueller, Hertz, Bobw liked this post
  10. #6
    Join Date
    Feb 2011
    Location
    Grant Alabama USA
    Posts
    599
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    214

    Default

    I agree with Orange vise up until the part about air blast not helping cutter life. Maybe tis is due to how fast we generally run. The coating on the endmills used in my videos is heat tolerant, not heat activated, so any temp drop is welcomed. Even the fan effect of the cutter spinning at high rpm helps. A mist sprayer used with the cutter in this video may only lower the running temp by a hundred or so degrees, but that will allow extended engagement time without overheating. This also helps with TiAln coatings.

  11. Likes jdj liked this post
  12. #7
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    7,415
    Post Thanks / Like
    Likes (Given)
    686
    Likes (Received)
    1780

    Default

    I gotta ask, even though this is a rookie question when it comes to high speed machining like this. If the material is heat treated D2, are these standard off the shelf endmills you use for something like this? Is it a special type of carbide that allows this much sparking off the cutter? Is it the coating, tool grind geometry?

    And if heat treated tool steels can be cut at this type of feed and speed, then can't soft cold roll steel be cut even faster? Frankly, I've seen this before but never attempt to try this type of cutting myself unless I'm on aluminum.

    I too, would have liked to have seen the finished product of that run.

  13. #8
    Join Date
    Feb 2011
    Location
    Grant Alabama USA
    Posts
    599
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    214

    Default

    Quote Originally Posted by Dave K View Post
    I gotta ask, even though this is a rookie question when it comes to high speed machining like this. If the material is heat treated D2, are these standard off the shelf endmills you use for something like this? Is it a special type of carbide that allows this much sparking off the cutter? Is it the coating, tool grind geometry?

    And if heat treated tool steels can be cut at this type of feed and speed, then can't soft cold roll steel be cut even faster? Frankly, I've seen this before but never attempt to try this type of cutting myself unless I'm on aluminum.

    I too, would have liked to have seen the finished product of that run.

    The basic endmill is common, just C4 carbide. The grind and coating is what makes the difference. Othe materials are machined like this on a regular basis, only larger cuts and faster. It will be two weeks befofe I get back to where I left the block, but it was ( D 2) machined in block letters. It did not finish the inside of the D because of my programming error. I'm not sure the endmill could have entered the cut, the corners were in bad shape. I am working on this because ceramic cutters arent always the best way to machine intricate details.

  14. Likes jdj liked this post
  15. #9
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    7,518
    Post Thanks / Like
    Likes (Given)
    2209
    Likes (Received)
    2449

    Default

    Sure beats grinding.
    How many parts (estimate) with one end mill?

    Buck

  16. #10
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,049
    Post Thanks / Like
    Likes (Given)
    80
    Likes (Received)
    369

    Default

    Quote Originally Posted by michiganbuck View Post
    Sure beats grinding.
    How many parts (estimate) with one end mill?

    Buck
    Lol, one!
    Seriously though I bet if you reduce the speed a bit it could help with tool life a lot.
    For hard stuff like that AlTin nano-coating works pretty good.

    Imo when I see sparks it generally means "slow down"
    I have machined 60rc D2 before at half the speed and no sparks.
    Not sure how it would affect the cutter life though -only ran for 2minutes or so.

  17. #11
    Join Date
    Feb 2011
    Location
    Grant Alabama USA
    Posts
    599
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    214

    Default

    Quote Originally Posted by michiganbuck View Post
    Sure beats grinding.
    How many parts (estimate) with one end mill?

    Buck
    I am trying to get 15 minutes actual "in cut time" at this speed, or as Zero said, twice as long at 50% of what I was doing here. Also in his post he said 2 minutes, this had around 6 without breaking. A 1/2" would have done better in this situation because of its thicker core absorbing the heat slower. As mentioned, it beats grinding. This regrind cost $17.22 delivered. I will have this worked out before the end of the year. The next run will have a koolmist sprayer and just a bit less sfm, higher feed. I will probably use a 1/2" also.

  18. #12
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    5,948
    Post Thanks / Like
    Likes (Given)
    230
    Likes (Received)
    4785

    Default

    Quote Originally Posted by jamesu229 View Post
    The basic endmill is common, just C4 carbide. .
    C4???
    Are you sure?
    Who the heck is making C4 rod for end mills and why would you run c-4 on hard D-2?

    Bob

  19. #13
    Join Date
    Apr 2011
    Location
    NJ, USA
    Posts
    444
    Post Thanks / Like
    Likes (Given)
    94
    Likes (Received)
    98

    Default

    What kind of thought process goes into grinding a cutting tool like this? Do you start with a standard set of angles and reliefs and then make adjustments from there?

    If so, what factors would allow you better tool life, or faster cutting speeds?

    Im sure its heavily dependent on what material is being cut, but maybe there are some generalizations?

  20. #14
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,049
    Post Thanks / Like
    Likes (Given)
    80
    Likes (Received)
    369

    Default

    Quote Originally Posted by jamesu229 View Post
    I am trying to get 15 minutes actual "in cut time" at this speed, or as Zero said, twice as long at 50% of what I was doing here. Also in his post he said 2 minutes, this had around 6 without breaking. A 1/2" would have done better in this situation because of its thicker core absorbing the heat slower. As mentioned, it beats grinding. This regrind cost $17.22 delivered. I will have this worked out before the end of the year. The next run will have a koolmist sprayer and just a bit less sfm, higher feed. I will probably use a 1/2" also.
    We often machine 50-55RC tool steel dry.
    At 150 SFM we get 1 hour of tool life slotting.

    In your HSM application i bet 10$ your tool will survive for at least an hour at 350 SFM

    We don't bother with regrinds so our target is usually at least an hour.

  21. Likes 5 axis Fidia guy liked this post
  22. #15
    Join Date
    Oct 2007
    Location
    detroit,mich.
    Posts
    4,707
    Post Thanks / Like
    Likes (Given)
    4710
    Likes (Received)
    411

    Default

    Quote Originally Posted by zero_divide View Post
    Imo when I see sparks it generally means "slow down"
    I have machined 60rc D2 before at half the speed and no sparks.

    When you get to machining 58Rc and over, hard steel, at higher speeds, the small chips incinerate in the air. It isn't QUITE the same type of spark as if a dull tool was cutting/rubbing. When turning hardened steel, it sometimes appears that a fountain of fire is coming off the tool/part interface. D.O.C. plays a big part (among other things!) in these unusual situations.

  23. Likes Oldwrench liked this post
  24. #16
    Join Date
    Feb 2011
    Location
    Grant Alabama USA
    Posts
    599
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    214

    Default

    Quote Originally Posted by bryan_machine View Post
    A general question (maybe there's a good thread on this somewhere) - how to decide where flood coolant is and is not a good idea? Is air blast always suitable when flood coolant is not?

    It would be nice to see a closeup of the resulting part, if allowed.

    Heres a picture of the part. I have made the needed modifications to the endmill and tool path that should give the results I'm looking for. The new parameters are 650 sfm , .015 radial and .010 ipt. All small areas are blocked off, and will be machined at the end of the program using 350 sfm at .015 z steps at .004 ipt. The customer that asked me do develop this cutter/path was very pleased with the initial results and will be using them quite often after a successful run.





    d2.jpg

  25. Likes Ray Behner, jdj, bryan_machine liked this post
  26. #17
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,049
    Post Thanks / Like
    Likes (Given)
    80
    Likes (Received)
    369

    Default

    Quote Originally Posted by jamesu229 View Post
    Heres a picture of the part. I have made the needed modifications to the endmill and tool path that should give the results I'm looking for. The new parameters are 650 sfm , .015 radial and .010 ipt. All small areas are blocked off, and will be machined at the end of the program using 350 sfm at .015 z steps at .004 ipt. The customer that asked me do develop this cutter/path was very pleased with the initial results and will be using them quite often after a successful run.





    d2.jpg
    0.01 ipt!
    Wow 0.004 ipt for slotting seems like alot.
    Do you have some sort of radius on the corners?

    Becase i dont see how it will not chip.

  27. #18
    Join Date
    Feb 2011
    Location
    Grant Alabama USA
    Posts
    599
    Post Thanks / Like
    Likes (Given)
    167
    Likes (Received)
    214

    Default

    .004 ipt should be no problem. The end grind I chose is basically a modified feed mill. I understand 30Rc is very different, but using a 3/4 endmill with my normal grind, I can face at .015 deep, 7500 rpm and 175 ipm, reliably. The new end grind is much tougher. I have 3 prototype cutters and plenty of material to play with. DLC coating with a protective outer coating is also an option, as $75 is the customers upper limit for a 1/2 that will run at the rates we are looking at. The endmill in the video was under $20, and I want to keep the cost low like this, better for business.

  28. Likes jdj liked this post
  29. #19
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    7,415
    Post Thanks / Like
    Likes (Given)
    686
    Likes (Received)
    1780

    Default

    I understand 30Rc is very different, but using a 3/4 endmill with my normal grind, I can face at .015 deep, 7500 rpm and 175 ipm, reliably.
    Am I reading this correctly? That's about a 1470 SFM. With a normal ground endmill, this is the speed you run on D2?

  30. #20
    Join Date
    Oct 2007
    Location
    detroit,mich.
    Posts
    4,707
    Post Thanks / Like
    Likes (Given)
    4710
    Likes (Received)
    411

    Default

    Quote Originally Posted by Dave K View Post
    Am I reading this correctly? That's about a 1470 SFM. With a normal ground endmill, this is the speed you run on D2?

    Soft D2 isn't as bad as some people make it out to be. You have a point however! That is pretty damn fast. I am guessing that the grind is Jamesu229's, NOT regular. The low D.O.C. also helps.


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
  •