Fly Cutter Rough Surface Finish on Carbon Steel
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 39
  1. #1
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    1

    Default Fly Cutter Rough Surface Finish on Carbon Steel

    I am having trouble obtaining a nice, smooth surface finish on carbon steel using an indexable fly cutter with my mill (pictures attached). The surface is very rough like sand paper and I can't figure out how to get a smooth finish. The fly cutter's cut diameter is 4in (2in radius) and I've tried running it at 600rpm starting with feeds from 2 Inches per minute up to 16 ipm, and then at 1300rpm with feeds from 6 ipm to 30 ipm and still no success. I tried depths of cuts from .002 to .010. I have been cutting with no lubrication and. I'm looking for what is causing this rough surface finish and how to possibly fix it.

    My observations are: I don't hear any chatter, I haven't seen any sparks, cutting insert is brand new and I don't see any signs of ware after use, my mill is sitting on 4x4's (vibration?).

    My machine's limits are 160-600rpm (low) and 1300-4600rpm (high) with feeds from 0-34 ipm in the x-axis only (all other axis's are manually adjusted). The mill is Kent USA KTM-5VK.

    I'd like to point out I am a novice in the machining world so I apologize if any of my terms seem odd. I am excited to learn as much as I can from you all and I appreciate all those who see this post and provide information. Also, can we please keep this discussion on this topic and avoid any unnecessary comments/off-topic discussions.

    Thanks!

    Cody
    Attached Thumbnails Attached Thumbnails img_0697.jpg   img_0696.jpg   img_0694.jpg   img_0695.jpg  

  2. #2
    Join Date
    Feb 2011
    Location
    BFE Nevada/San Marcos Tx
    Posts
    1,232
    Post Thanks / Like
    Likes (Given)
    1103
    Likes (Received)
    668

    Default

    In the last pic it appears your feed is too fast, you might also consider reducing the stick-out of the tool in the flycutter. Have you tried using HSS, interupted cuts are hell on carbide. Is material steel, or cast iron? Swarf in pics looks like cast iron.

  3. Likes atomarc, cfoxx911, Ray Behner liked this post
  4. #3
    Join Date
    May 2009
    Location
    Canandaigua, NY, USA
    Posts
    2,887
    Post Thanks / Like
    Likes (Given)
    141
    Likes (Received)
    1290

    Default

    Agree tool is way out there. Remember if you try HSS you have to check SFPM and probably slow way down. If it's cast iron, dry may be OK, but if it's some sort of CRS or something, you need oil. I'd probably do it with a 3/4" end mill and live with the pattern you'd get. Or get that grinder you always wanted.

  5. Likes cfoxx911 liked this post
  6. #4
    Join Date
    May 2003
    Country
    UNITED STATES
    State/Province
    Iowa
    Posts
    10,492
    Post Thanks / Like
    Likes (Given)
    3616
    Likes (Received)
    4273

    Default

    This is a first for me. I've never seen anybody use a turning tool in a fly cutter.
    JR

  7. Likes redlee, Matt_Maguire liked this post
  8. #5
    Join Date
    Apr 2007
    Country
    UNITED STATES
    State/Province
    West Virginia
    Posts
    1,047
    Post Thanks / Like
    Likes (Given)
    525
    Likes (Received)
    415

    Default

    I have always used either brazed carbide tipped tools or hss, very sharp.

  9. Likes cfoxx911 liked this post
  10. #6
    Join Date
    Feb 2006
    Location
    Minneapolis
    Posts
    208
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    27

    Default

    Hard to see but it looks like the cutting corner of your tool is quite worn. There's also a big exit burr which would indicate a dull tool.

  11. Likes Bobw liked this post
  12. #7
    Join Date
    Apr 2009
    Location
    Beaver County Alb. Canada
    Posts
    1,856
    Post Thanks / Like
    Likes (Given)
    533
    Likes (Received)
    906

    Default

    Try the same tool in a lathe with overhang the same and it will probably give the same results.3

  13. Likes JRIowa liked this post
  14. #8
    Join Date
    Jan 2008
    Location
    Mountains of Washington State, USA
    Posts
    434
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    135

    Default

    Fly cutter is way too small. Too much overhang with the tool. Wrong tool bit geometry. Feed to fast. Spindle RPM too fast.

    If you have much of this to do, buy a big fly cutter. Below, 3 inch A36 flat bar, the fly cutter is 3" in diameter. With a little tool projection the cut is made in one pass. I am using 3/8" HSS tool bits in the fly cutter. Note the cutting oil.

    dscn5713-1-.jpg2+

    For my operation in the photo:

    4 times the cutting speed divided by the diameter:

    A36 steel cutting speed is 100

    diameter of the tool about 3 1/2 inches say 4 for simplified calculations

    4 times 100 divide by 4 gives me about 100 RPM

    In addition to the 8 speeds in my mill I have a 3 hp DC motor on it with variable speed drive controller. I set the gearing/belts to approximate rpm and fine tune with the speed controller

    So I am saying your 1300 rpm is way too high.

  15. Likes digger doug, cfoxx911 liked this post
  16. #9
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    10,236
    Post Thanks / Like
    Likes (Given)
    1394
    Likes (Received)
    3688

    Default

    No tip clearance for the cutting edge. It's a lathe toolholder, so it would appear, and the way you're using it would be equivalent to having the tool set about 1/4" above centerline: it's going to rub like crazy beneath the cutting edge, because that's where the maximum sweep of the tool is.

  17. #10
    Join Date
    Jan 2008
    Location
    Mountains of Washington State, USA
    Posts
    434
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    135

    Default

    Quote Originally Posted by Pete Deal View Post
    I have always used either brazed carbide tipped tools or hss, very sharp.
    Yes Yes Yes. Tool bit grinding is the most important skill in a Machine Shop.

  18. #11
    Join Date
    Apr 2006
    Location
    Manchester, England
    Posts
    8,369
    Post Thanks / Like
    Likes (Given)
    1234
    Likes (Received)
    5319

    Default

    Quote Originally Posted by JRIowa View Post
    This is a first for me. I've never seen anybody use a turning tool in a fly cutter.
    JR
    You've never lived JR ! I have but normally it's not a throw away tip tool.

    Regards Tyrone.

  19. Likes JRIowa liked this post
  20. #12
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    2,280
    Post Thanks / Like
    Likes (Given)
    201
    Likes (Received)
    1249

    Default

    Head trammed? Really though who uses fly cutters anymore?

    Try running 300 ripems and an inch per minute. Copius quantities of cutting fluid of your choice brushed on the part.

  21. #13
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    South Carolina
    Posts
    475
    Post Thanks / Like
    Likes (Given)
    364
    Likes (Received)
    394

    Default

    Lathe tool will not work in a fly cutter. Geometry is all wrong. Also, I can't really tell from picture, your slot in the cutter needs to be offset from the centerline by whatever size tool you are using, so your tool tip will be on the centerline of the cutter.

  22. #14
    Join Date
    Jun 2006
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    1,883
    Post Thanks / Like
    Likes (Given)
    1089
    Likes (Received)
    738

    Default

    A lathe toolholder/insert will work Great, but you have to make the fly cutter!
    I made one a few years back, it worked amazing facing hardened 4130.

  23. #15
    Join Date
    Mar 2009
    Location
    Eureka, CA
    Posts
    3,772
    Post Thanks / Like
    Likes (Given)
    748
    Likes (Received)
    1303

    Default

    Agree, a lathe tool fixtured properly will work fine..but that picture sure looks like cast iron to me, and cast iron doesn't finish exactly like regular old carbon steel. If your feed speed was lower the finish would look much better.

    Stuart

  24. #16
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    441
    Post Thanks / Like
    Likes (Given)
    22
    Likes (Received)
    186

    Default

    That definitely appears to be cast Iron, which will not require lubrication. Your tool is sticking out way too far, reduce the cutting diameter as much as you can. It is in the fly-cutter head backwards (you will also need the reverse of that tool holder style). That fly cutter is meant to turn the other direction. Cutting edge of insert should be about centerline of the tool. Lower your RPM to between 100-200 rpm and you should be able to get a decent finish at about 2-4 i.p.m. With anywhere from .01 to .04 depth of cut.

  25. #17
    Join Date
    Sep 2009
    Location
    Apex, NC
    Posts
    1,489
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    739

    Default

    Iscar F45E face mill or equivalent, 3" diameter or smaller. The feed, and speed can be higher, and it doesn't beat up the wimpy R8 spindle like a flycutter. Works well on steel to aluminum.

  26. #18
    Join Date
    Apr 2006
    Location
    Manchester, England
    Posts
    8,369
    Post Thanks / Like
    Likes (Given)
    1234
    Likes (Received)
    5319

    Default

    I had a little 4 insert positive rake throw away tip milling cutter about 1-1/2" in dia on the " Bridgeport " I worked on. I can't recall the make now but it was great. Did everything I wanted and didn't beat up the machine.

    Regards Tyrone.

  27. #19
    Join Date
    Mar 2012
    Location
    Geilenkirchen, Germany
    Posts
    2,394
    Post Thanks / Like
    Likes (Given)
    1444
    Likes (Received)
    1222

    Default

    As others have stated, your tool geometry is wrong. You are rubbing not cutting. Just like on a lathe, your cutting edge must reside on the center line. You need adequate back rake and cutting clearances. You have neither. I assume you have an R8 spindle, is so, you have questionable stiffness at that diameter, this is especially true and aggravated by that extreme hang out of the bit. If you must use indexable carbide, there are inserts designed specifically for this. The one you are using isn't. Can this be done on an R8 machine? Yes, but you should be using HSS. You need a larger, stiffer fly cutter, you need to go slower with lighter DOC and slower feed (watch your tool loading). Also, your head tram must be spot on or your result will not be flat. if your tram is correct, you will have a very fine cross hatch pattern as a finish. If you don't, it ain't flat. The tool's nose radius should equal 1.5 times the advance rate per revolution for the best finish. The greater the nose radius, the greater the tool loading and the greater the tool deflection. It is a delicate balance. In any case, it's good training. Just as others have stated, you are better off using an end mill and living with the tool marks.........the machine will be happier and the end result will be achieved faster and better.

  28. #20
    Join Date
    May 2003
    Country
    UNITED STATES
    State/Province
    Iowa
    Posts
    10,492
    Post Thanks / Like
    Likes (Given)
    3616
    Likes (Received)
    4273

    Default

    Quote Originally Posted by Tyrone Shoelaces View Post
    You've never lived JR ! Regards Tyrone.
    Oh, I have lived. I have several flycutters that I use on very, very rare occasions. I learned many years ago how hard they are on BPs and that a good insert cutter will out perform them 99.9999% of the time.
    JR

  29. Likes Tyrone Shoelaces 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
  •