Slotting 1045
Close
Login to Your Account
Results 1 to 10 of 10

Thread: Slotting 1045

  1. #1
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    0

    Default Slotting 1045

    Heya all! I have a project I am working on with the Fadal 4020. Shortening and cutting lightening slots in these 1045 steel gear blanks.

    2019-11-20_06-32-34 by Jackson Edwards

    The problem I am having is short tool life on the end mill I am cutting these slots with. I am getting roughly 60 parts per tool (600 slots) after swapping feeds, speeds, ramp angles and even a few different kinds of tools,

    The best combination I have found is:

    .3125 Maritool variable 4fl TiAlN for tool steel w .02 radius

    Running Mobil soluble oil 100 at a fairly high concentration.

    340sfm 4200rpm 7IPM .0004ipt (seems light, but breaks if I lower spindle speed, and breaks if I increase feed rate)

    4° profile ramp, this does roughly five zigzags to the bottom. Slot is .340" deep, about 1.2xD

    6ipm 14 thou radial finish pass, as the ramping cut leaves a bit to be desired.

    Things I have tried:

    A straight plunge to 100% depth and slot works some of the time, but depending on coolant stream angle, it will chip load and fail randomly.

    Plunge to 1/2 depth and slot works ok, but The tip .150 wears and fails faster than the ramping pass does.

    I pulled an end mill after ~50 parts and you can see the degradation on the cutting edges on the bottom edges, as well as the sides about ~.130" up the flute.


    2019-11-20_06-55-36 by Jackson Edwards



    2019-11-20_06-55-48 by Jackson Edwards

    Thanks!

  2. #2
    Join Date
    Jan 2003
    Location
    Posts
    355
    Post Thanks / Like
    Likes (Given)
    47
    Likes (Received)
    95

    Default

    Be careful holding multiple parts like that in a vice. Really not a good idea, eventually you will get 2 slightly different size parts and the small one will go flying taking god knows what with it. Could loose a tool? Part? Spindle? Maybe your head after the part passes though those rinky dink fadal doors (I have a 4020 too lol).

    In terms of cutter life id be tempted to try a faster feed and lower ramp depth if you need too. Not sure if you will gain much. 600 slots dont seem too bad.

  3. #3
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,910
    Post Thanks / Like
    Likes (Given)
    1302
    Likes (Received)
    3748

    Default

    600 slots doesn't sound awful. You'll see an improvement if you drill a start hole

  4. Likes Mtndew, SIM liked this post
  5. #4
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    479
    Post Thanks / Like
    Likes (Given)
    129
    Likes (Received)
    179

    Default

    Quote Originally Posted by Larry Dickman View Post
    600 slots doesn't sound awful. You'll see an improvement if you drill a start hole
    I'll second that!

    Also get a coolant nozzle right at the cut blowing the chips out. I'll often close a couple nozzles to get more coolant where it is needed.

  6. #5
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,031
    Post Thanks / Like
    Likes (Given)
    1138
    Likes (Received)
    673

    Default

    600 slots doesn't sound bad, but I would think you should be able to go quite a bit faster. I would be ramping at about 15-20% cutter diameter and feeding about .002ipt. How is the runout of the cutter? Can you get away with machining dry with an air blast?

  7. Likes mmurray70, FARFLE liked this post
  8. #6
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,759
    Post Thanks / Like
    Likes (Given)
    4368
    Likes (Received)
    2884

    Default

    Drill a start hole,ditch the ramping.

  9. Likes FARFLE, SIM, Larry Dickman liked this post
  10. #7
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    0

    Default

    Quote Originally Posted by mmurray70 View Post
    Be careful holding multiple parts like that in a vice. Really not a good idea, eventually you will get 2 slightly different size parts and the small one will go flying taking god knows what with it. Could loose a tool? Part? Spindle? Maybe your head after the part passes though those rinky dink fadal doors (I have a 4020 too lol).

    In terms of cutter life id be tempted to try a faster feed and lower ramp depth if you need too. Not sure if you will gain much. 600 slots dont seem too bad.


    Luckily these are precision ground, and should be a consistent OD, But I do have my guy watching out to see if one tightens up before the other does. I'll give a faster shallower ramp a shot and see what I get.


    The Fadal isn'tset up for air blast at the moment, But the facing op is done dry and works amazingly with a fast adaptive on a 7fl mill.



    I'll try snagging a carbide drill and bashing out a series of holes, I am wondering if the super interrupted cut would be better than continuous plunging.

  11. #8
    Join Date
    Feb 2004
    Location
    Staten Island NewYork USA
    Posts
    3,766
    Post Thanks / Like
    Likes (Given)
    1106
    Likes (Received)
    1803

    Default

    Looks like you have a common suggestion going through the responses.

    Drills drill better then Endmills.

    Looks like you can get two, maybe three holes in each of those slots.

    Drilling would remove alot of material quickly.

    With less to remove the endmill lasts longer, less chips to recut.
    Ramping an endmill has alot of tool engagement, lots of heat with poor chip evacuation.

    A nice Cobalt Stub Drill will make short work of the holes. With much of the material hogged out you should be able to bring up the feed by a good amount.

    It's one of those add an operation and save time and tool things.

  12. Likes FARFLE liked this post
  13. #9
    Join Date
    Oct 2008
    Location
    Baltimore
    Posts
    106
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    42

    Default

    Drill starter hole
    Use modern tool path (Volumil)
    Switch to a better toolholder like Emuge FPC

  14. #10
    Join Date
    Feb 2011
    Location
    Grant Alabama USA
    Posts
    611
    Post Thanks / Like
    Likes (Given)
    174
    Likes (Received)
    221

    Default

    Is this an ongoing job? A few changes in tooling and processing methods would help greatly. Slotting this material should be no problem. Drill an entry hole. Speeds and feeds should be 400 sfm and.0012 ipt. Run dry.


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
  •