Newer machinist feeds and speeds question
Close
Login to Your Account
Results 1 to 9 of 9
  1. #1
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default Newer machinist feeds and speeds question

    Hi

    I know this has been hashed many times but I still haven't been able to nail settings down. I need to mill a .012" slot about .006" deep in 440C Stainless steel, non-hardened. My mill's max RPM is 2500. What depth of cut and feed rate do I need? I'll have a 2 flute end mill. I know from looking around I need about 100 fpm for free machining stainless. My pocket book will thank you, the endmills are about 20-25 bucks apiece.

    John

  2. #2
    Join Date
    May 2005
    Location
    CA
    Posts
    939
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    163

    Default

    If you're talking about a .012" diameter end mill at 2500, you will only see 7.8fpm.

    Would the part and slot lend itself to turning it sideways and cutting with with a narrowed-up keyway type cutter?

  3. Likes EnderDRM liked this post
  4. #3
    Join Date
    May 2004
    Location
    Paradise, Ca
    Posts
    2,136
    Post Thanks / Like
    Likes (Given)
    623
    Likes (Received)
    1073

    Default

    Practice this first: Make a 1/2" wide slot with a 1/2" endmill, 1/4" deep, but RPM can be no higher than 61. Yes, 61 RPM. Then you'll have a feel for what you're trying to do with your .012" endmill. Except it breaks a whole lot easier.

    Unless your machine has excellent motion control and you can get to near-zero runout at the end of the tool, sub this to somebody who is set up for it. If you're worried about a $25 endmill, you are not ready for this.

  5. Likes Bobw liked this post
  6. #4
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,543
    Post Thanks / Like
    Likes (Given)
    12067
    Likes (Received)
    9682

    Default

    Quote Originally Posted by big_i11580 View Post
    Hi

    I know this has been hashed many times but I still haven't been able to nail settings down. I need to mill a .012" slot about .006" deep in 440C Stainless steel, non-hardened. My mill's max RPM is 2500. What depth of cut and feed rate do I need? I'll have a 2 flute end mill. I know from looking around I need about 100 fpm for free machining stainless. My pocket book will thank you, the endmills are about 20-25 bucks apiece.

    John
    I'll give you credit for thinking in terms of Surface Feet..

    The answer is pretty simple.. Do your calculations for RPMs, using your intended
    SFM #... If the RPM your calculation gives you is higher than you have.. Then
    you use the RPM's you do have available to do your feed calculations.

    It happens a decent bit of the time, where your machine can't produce the #'s your
    calculations provide.. RPM's is a big one, especially on smaller endmills..

    Occasionally you have to figure backwards because your machine won't provide the
    feed rate you calculated..

    If on a low HP machine, sometimes you have to figure backwards because the spindle
    motor won't pull the cut you calculated...

    And I don't think 440C is a free machining stainless.. There is a 440F which I got to
    use ONCE, and it was kinda nice.. I haven't cut 440C in years (though I do have some
    to do tomorrow).. If I recall, its not horrible, but its not great either.. And it
    has a very distinct smell to it when you are cutting. (some people think I'm crazy with
    the smell thing, but I can SMELL 440 cutting).

  7. #5
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    2,585
    Post Thanks / Like
    Likes (Given)
    713
    Likes (Received)
    1380

    Default

    Quote Originally Posted by Bobw View Post
    I'll give you credit for thinking in terms of Surface Feet..

    The answer is pretty simple.. Do your calculations for RPMs, using your intended
    SFM #... If the RPM your calculation gives you is higher than you have.. Then
    you use the RPM's you do have available to do your feed calculations.

    It happens a decent bit of the time, where your machine can't produce the #'s your
    calculations provide.. RPM's is a big one, especially on smaller endmills..

    Occasionally you have to figure backwards because your machine won't provide the
    feed rate you calculated..

    If on a low HP machine, sometimes you have to figure backwards because the spindle
    motor won't pull the cut you calculated...

    And I don't think 440C is a free machining stainless.. There is a 440F which I got to
    use ONCE, and it was kinda nice.. I haven't cut 440C in years (though I do have some
    to do tomorrow).. If I recall, its not horrible, but its not great either.. And it
    has a very distinct smell to it when you are cutting. (some people think I'm crazy with
    the smell thing, but I can SMELL 440 cutting).
    This is right on the money. I would use a HSS 4 fluter if you can get it, not because it's cheaper or because you are going to F-up (both are realities though), but because it takes more of a beating. 440C is a little gummy, not terrible but...you don;t have enough RPM to utilize Carbide, so you need a tougher tool.

    I would start out with 2500 RPM, 1 IPM and full .006" depth. That will be .0001" chip load per flute IF it's a 4 fluter, if not 4 then run .5 IPM. Minimize runout as much as humanly possible. I mean, get your Tenths indicator on the very end of the Endmill, take your time.

    Bob, I can smell all kinds of different things cutting, 440c smells a little like clean fuel burning to me. 4140 I can smell from a mile away, Brass obviously. I'm sure others.

    R

  8. Likes Bobw, Vancbiker, aj liked this post
  9. #6
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,051
    Post Thanks / Like
    Likes (Given)
    581
    Likes (Received)
    1539

    Default

    Quote Originally Posted by litlerob1 View Post
    ....I would use a HSS 4 fluter if you can get it, not because it's cheaper or because you are going to F-up (both are realities though), but because it takes more of a beating. 440C is a little gummy, not terrible but...you don;t have enough RPM to utilize Carbide, so you need a tougher tool.
    +1 on this ^

    The first time I had to mill some small details in Inconel, I ordered in top of the line cobalt endmills. After watching them snap off, switched to cheap regular M2 HSS endmills from the toolroom and they made it through job. IIRC ~5 SFM.

  10. #7
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Thanks a ton. I sincerely appreciate the replies.

    John

    Sent from my SM-G900V using Tapatalk

  11. #8
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Just thought I would let people know the results. I bought 2 endmills, 4 flute both. Ran at 2500 rpm and at .1ipm feed rate. I took .0015" at a pass. Did both parts without a hitch. I eventually moved to .2 ipm after 1 pass. No issues. Probably can go faster but I broke one endmill during setup and only had the other. Thanks. Always am learning new stuff.

    John

    Sent from my SM-G900V using Tapatalk

  12. Likes exkenna liked this post
  13. #9
    Join Date
    Oct 2011
    Location
    West-Central Illinois, USA
    Posts
    1,014
    Post Thanks / Like
    Likes (Given)
    1549
    Likes (Received)
    441

    Default

    Glad it worked out for you! I just ran your settings through my calculator (just to reverse things). They amount to 7.85 surface feet per minute, at .2 inches per minute your feed load was 0.00002 inches per tooth (software reports 2E-5th! LOL).

    Further, your metal removal rate was 0.0000036 cubic inches per minute (3.6E-6th) and you needed 0.000004 horse power (4E-6th) to make the cut! Pretty sure those are record numbers I just ran through my ShellerPickerCombineChopper!

    Good luck,
    Matt

  14. Likes exkenna, Bobw 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
  •