Tapping speeds?


Results 1 to 18 of 18

Thread: Tapping speeds?

  1. #1
    Registered
    Join Date
    Jan 2011
    Location
    South Africa
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default Tapping speeds?

    Hi Guys,

    I have a VF2 with rigid tapping, anywhere I can get some safe tapping speeds for M4 to say M16?

    I am still waiting for my tool supplier to give these to me.

    I have been using anything below 60rpm, used as slow as 10rpm today (M6),

    Haven't had too many problems with M8 and bigger, M4 and M6 snap like twigs!

    I only use mild steel and have been using Somta blue ring spiral flute taps (blind holes).

    I run edgecam which sorts outs feeds,

    thanks

    Similar Threads:


  2. #2
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    Run much faster than that. I use 1000rpm for nearly everything from 4mm up to 5/8"-18. I have found taps cut better at a good speed. The metal seems to flow easier and form a good chip. Lubrication is also important and I run mine at a 10 to 15% mix which gives better tap life.

    Small taps in mild steel a sometimes a bit of a problem and I always try to sneak the drill size up a bit somewhere between 65% and 75% full thread. Repeat Rigid Tapping also helps. Go in about two threads, back out and then go four, then six until you reach your depth. Make sure Repeat Rigid Tapping is turned on in both places in the Settings/Parameters.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  3. #3
    Registered WallyL7's Avatar
    Join Date
    Dec 2008
    Location
    USA
    Posts
    717
    Downloads
    0
    Uploads
    0

    Default

    Haas had a handy dandy little tap speed and feed chart (that I have hard copies of) but I can't seem to find it in the 10 seconds of googling I just did.

    But for reference:

    6-32 tap in 6061 alum = s2464 f77.0
    1018 steel = s1376 f43.0
    1/2-13 tap in 6061 = s676 f52.
    1018 = s377 f29.

    to give you a rough idea of what they recommend.

    Tim


  4. #4
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    Just like drilling, smaller the tap, faster the RPM. In stainless, I have run M4 as fast as 600 RPM. In aluminum, 2000.



  5. #5
    Registered
    Join Date
    Apr 2005
    Location
    Paradise, Ca, USA
    Posts
    713
    Downloads
    0
    Uploads
    0

    Default

    HSS is HSS, no matter if it's drilling a hole or tapping a thread. I've never understood the disconnect on this topic.



  6. #6
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    The disconnect probably comes in the fact that there is much more surface contact area and more cutting forces in play with tapping than in drilling.

    Also, the average machine with 10,000 RPM spindle is probably not going to be able tap a #4-40 at 10,000 RPM. Ya think?



  7. #7
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by txcncman View Post
    .......Also, the average machine with 10,000 RPM spindle is probably not going to be able tap a #4-40 at 10,000 RPM. Ya think?
    The feed would only be 250IPM so theoretically it should be possible.

    Maintaining synchronization during the stop and reverse out may be a challenge.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  8. #8
    Registered
    Join Date
    Apr 2005
    Location
    Paradise, Ca, USA
    Posts
    713
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by txcncman View Post
    The disconnect probably comes in the fact that there is much more surface contact area and more cutting forces in play with tapping than in drilling.
    I drill 1018 at 80 SFM with HSS drills. I tap 1018 at 80 SFM with form taps (talk about surface area!) with great results. This is with Blaser coolant at 8-10%, no tapping fluid.

    Also, the average machine with 10,000 RPM spindle is probably not going to be able tap a #4-40 at 10,000 RPM. Ya think?
    I was hoping some common sense would be applied to my post. Even then, I'm not all that far off of your example in one part I make. 360 brass, 4-40 form tap 2.375" deep.* Programmed at 8000 RPM and my VF-2ss get's pretty close to that by the bottom of the hole.

    *It's actually four separate tabs that are .250" thick with 2.375" between the opposing faces. By the third tab, it's hauling ass.



  9. #9
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    Most of the machines I work with are a little older with rapid rates at 200 IPM. Just sayin'



  10. #10
    Registered
    Join Date
    Jan 2011
    Location
    South Africa
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default

    wow I thought my 60rpm was high!

    I ran 200rpm with an M6 the other day and broke it as well,

    I must investigate the rigit tapping - back and forward etc like you mention, I check my software.

    I have the haas handbook, I'll check for the speeds they give.

    I also like the idea of going slightly bigger on the holes - I did this with the M6 tap yesterday, tap says go with 5mm, after breaking one I went to 5.2, little loose but its not bad!



  11. #11
    Registered
    Join Date
    Jan 2011
    Location
    South Africa
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default

    was just given this by a supplier:

    speed is 10000 or 16000/3.142/m6 0r m8


    feed is =s530*pitch=f


    speed 10000/3.142/6=530rpm speed 530 * = 530

    so M6 = 530rpm



  12. #12
    Registered l u k e's Avatar
    Join Date
    Apr 2005
    Location
    USA
    Posts
    903
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Geof View Post
    Lubrication is also important and I run mine at a 10 to 15% mix which gives better tap life.

    I didn't realize that coolant would work for tapping; I've been programming the coolant to shut off then oil the tap on each hole. (What a newbie!)

    2008 Haas VF2D
    OneCNC XR5 Mill Expert


  13. #13
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    Coolant or no, all depends on the circumstances. A lot of learning machining is trial and error. What works in one application may not work in another.



  14. #14
    Registered
    Join Date
    Jan 2011
    Location
    South Africa
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default

    ok Somta helped me here with a nice chart - see link for their PDF - pg 67,68 and 69

    http://www.somta.co.za/pdf/Somta%20T...er%20Guide.pdf

    Going to start with M16 today



  15. #15
    Registered WallyL7's Avatar
    Join Date
    Dec 2008
    Location
    USA
    Posts
    717
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Matt@RFR View Post
    HSS is HSS, no matter if it's drilling a hole or tapping a thread. I've never understood the disconnect on this topic.

    I can't seem to find where anyone said or implied HSS isn't HSS - where do you get the disconnect from?

    Tim


  16. #16
    Registered TheWidowsSon's Avatar
    Join Date
    Oct 2017
    Location
    United States
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default Re: Tapping speeds?

    hey sndsa

    i use a vf2 everyday and i also run m4 alot mainly drilling and tapping but sometimes milling and what i have found is that coated tools is your best bet when machining m4
    TiAlN for your drills TicN for your taps and AlCrN for your end mills with a .030 radius if possible also i have learned that with tool steel coolant hurts you more than helps
    but it can be used i use it while machining m4 on my drills and taps but its at 10 to 15 percent mix and i also use Hertel Cobalt drills OSG HSS taps and AmericanToolService(ATS) Carbide End mills great company
    and great end mills i run 312 sfm and .0031 chip load roughing 612 sfm and same chip load for finishing my drills i use 30-45 sfm and my taps i use 30-40 sfm main thing you need to know with these coatings they need heat to activate or oxidizes
    all my tools i get come from msc and there not that expensive i get great great tool life out of these numbers also do not peck and do not spot drill so if can get screw machine drills with at least a 135 degree split point this will help walking of the drill hope this help



  17. #17
    Member Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1852
    Downloads
    0
    Uploads
    0

    Default Re: Tapping speeds?

    Over 6 year old post.

    Two Haas VF-2's, Haas HA5C, Haas HRT-9, Hardinge CHNC 1, Bother HS-300 Wire EDM, BobCAD V23, BobCAD V28


  18. #18
    Registered
    Join Date
    Nov 2017
    Location
    United Kingdom
    Posts
    6
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by sndsa View Post
    wow I thought my 60rpm was high!

    I ran 200rpm with an M6 the other day and broke it as well,

    I must investigate the rigit tapping - back and forward etc like you mention, I check my software.

    I have the haas handbook, I'll check for the speeds they give.

    I also like the idea of going slightly bigger on the holes - I did this with the M6 tap yesterday, tap says go with 5mm, after breaking one I went to 5.2, little loose but its not bad!

    Hi i tap m6 all the time 600rpm 5mm drill make sure my coolant strength is alway 8% never have any problems at all



Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Tapping speeds?

Tapping speeds?