584,812 active members*
5,484 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking > MetalWork Discussion > Coated Carbide 4Flute Endmill, 3Flute Slot Drill, or 2Flute Slot Drill?
Results 1 to 8 of 8
  1. #1
    Join Date
    Jan 2007
    Posts
    35

    Coated Carbide 4Flute Endmill, 3Flute Slot Drill, or 2Flute Slot Drill?

    My preference has been to generally use a 4flute coated carbide endmill for almost all my machining and only use a 2flute slot drill when slotting or if shavings could be a problem. I never really used a 3flute slot drill.

    In my new company, they only really have 3flute slot drills and use 4flutes only for finishing aluminium jobs. I think the idea is to reduce tool inventory, as they can use the 3flute slot drill for all types of operations.

    Can anyone give me their opinions and preferences.

    Thanks.

  2. #2
    Join Date
    Aug 2006
    Posts
    246
    3 flutes give you the best of all worlds. They generally have enough flute clearance to cut the softer metals. 3 flutes also allow you to still maintain a decent feedrate and can give you better harmonics than a 2 or 4 flute because it they will tend to have a flute in the cut at all times (depending on depth of cut, etc.) The downside is that they're a little tricky to measure for cutter comp.....

    :cheers:
    I don't know much about anything but I know a little about everything....

  3. #3
    Join Date
    Jan 2007
    Posts
    35

    Thanks. (Harmonics?)

    Quote Originally Posted by cdlenterprises View Post
    3 flutes give you the best of all worlds.
    I suspected that this was the reasoning behind our company using 3flute tools. .[/QUOTE] give you better harmonics than a 2 or 4 flute because it they will tend to have a flute in the cut at all times [/QUOTE] Sorry for my lack of understanding but could you perhaps explain this concept a little further, in particular the phrase "better harmonics". I assume you are trying to say the the 3flute tool is better 'balanced' during machining than the 2 or 4 flute variety.

    Thanks

  4. #4
    Join Date
    Feb 2007
    Posts
    664
    the amount of flute engagement has to do with the angle of the helix

    the grater the angle the more engagement you have

    always having the tool engaged in the stock will keep it from relaxing in between flutes

    3 fluted tools or odd fluted tools tend to cancel out some of the vibrations

    data flute makes a really nice 3 flute end mill

  5. #5
    Join Date
    Apr 2006
    Posts
    82
    Quote Originally Posted by weaston View Post
    My preference has been to generally use a 4flute coated carbide endmill for almost all my machining and only use a 2flute slot drill when slotting or if shavings could be a problem. I never really used a 3flute slot drill.

    In my new company, they only really have 3flute slot drills and use 4flutes only for finishing aluminium jobs. I think the idea is to reduce tool inventory, as they can use the 3flute slot drill for all types of operations.

    Can anyone give me their opinions and preferences.

    Thanks.
    - 4 flutes with special design for roughing, slotting is very good when slotting material difficult to cut (steel, stainless steel, superalloy). You can have a very good productivity.
    The main problem is the shouldering:
    4 flutes produces easily chatter when you use roughing parameters. Either you use a special mill with differential pitch in order to avoid chattering, or you have a very rigid structure.
    Other solution:
    Use low ae (radial depth of cut) with high cutting speed and feedrate.

    - 3 flutes should be used for little diameter (diam 2...8mm) in slotting and shouldering of material difficult to cut (steel, stainless steel, superalloy, titanium). There is just a special case: It's the method drilling/slotting. These special mill (Nachi, NS tool) have 3 flutes whatever the diameter. Here is an exemple
    http://www.nachi-fujikoshi.co.jp/eng...eo/geoslot.ram

    - 2 flute should be only used for very little diameters (diameter 0.05... 2mm) for steel, stainless steel, titanium. 2 flutes is very good in slotting of material such plastics, aluminium, cooper whatever the diameter.

    Reason:
    - Aluminium, Plastic,...produce low cutting forces and the most important is the place for chip evacuation => 2-3 flutes maxi
    - Steel, stainless steel, ... produce high cutting force. The most important is the flute resistance and it's not the case with 2flutes end mills (for diameter 3mm or more).

  6. #6
    Join Date
    Mar 2007
    Posts
    7
    To sum it all up. If you have large chips (i.e. aluminum), you want less flutes when hogging it out so chips don't get caught in front of the post-ceding flute. More flutes are better when the material makes small chips (i.e. cast iron) so you can get a higher material removal rate when increasing rpm (increased heat) or travel feed rate (increased spindle load) will produce problems.

  7. #7
    Join Date
    Apr 2007
    Posts
    10
    I would recommend to use 4 flute for everything is possible.

    Centrecutting tool is not an issue, 4 flute cutter with Ramp or helical entry motions on all toolpathing. id usually recomment 2 to 3 degree entry angle

    feed fast with light cuts to avoid heat build up (heat should be ejected with chip if you do everything right)

    also trocoidial toolpath motion will give incredible chip evactuation

  8. #8
    Join Date
    Dec 2006
    Posts
    95
    My tool salesman got me hooked on 3-flute by Duramill, they call theirs "WhisperCut" . Big time tool life and feed rate. Only drawback is the corner is not a true 90. Dosen't matter much on the parts we run, and our Integrex smokes with'em.

Similar Threads

  1. Carbide drill VS indexable drill
    By kalmah in forum MetalWork Discussion
    Replies: 10
    Last Post: 02-21-2023, 08:09 AM
  2. Replies: 47
    Last Post: 02-01-2008, 08:32 PM
  3. Can I drill AISI 1020 plate steel with a drill bit?
    By Apples in forum MetalWork Discussion
    Replies: 2
    Last Post: 02-01-2006, 06:15 PM
  4. Breakchip drill then Endmill?
    By DennisCNC in forum Visual Mill
    Replies: 2
    Last Post: 01-05-2006, 03:10 AM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •