Rigid Tapping Feeds/Speeds in AL6061
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 26
  1. #1
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    60
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    4

    Question Rigid Tapping Feeds/Speeds in AL6061

    Hi guys,

    I'm attempting to rigid tap several 6-32 holes in half-inch thk al6061 on my 2005 Fadal VMC 3016. Problem is I have zero idea how to set the speed besides trusting what HSMworks auto-selects for me. Right now I put in HSMworks I'm tapping these holes with a thread-forming operation and it tells me to go at 5000 RPM (feed is not even an option to select). I've been trawling old posts on this forum and that seems a little fast. FSWizard, which I usually trust, tells me to tap at 5000 as well (well, 4985).


    How would I calculate or confirm that this is about right - or wrong?

  2. #2
    Join Date
    Jul 2012
    Location
    Washington
    Posts
    1,805
    Post Thanks / Like
    Likes (Given)
    618
    Likes (Received)
    677

    Default

    Tapping speed for a 6-32 form tap in aluminum is all about how fast you can go with your machine. With a Fadal I would start around 1000 rpm and go from there depending on how it sounded/worked. What is the max tapping rpm for your machine? Depending on your spindle inverter I may cut that speed in half as a general rule of thumb.

  3. #3
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    603
    Post Thanks / Like
    Likes (Given)
    351
    Likes (Received)
    613

    Default

    As long as the feed is calculated correctly to the programmed RPM you should be ok.
    Your machine is not going to reach 5000 RPM in 1/2 inch.

  4. #4
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,401
    Post Thanks / Like
    Likes (Given)
    2766
    Likes (Received)
    1954

    Default

    As said above, you can go as fast as your machine will allow.
    #6-32 tap at 5k is only 156.25 IPM feedrate. But the sync is the key here. Pay attention to the spindle reverse and how it acts.

  5. #5
    Join Date
    Aug 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    7

    Default

    A form tap in 6061 Aluminum should be at around 180-250 SFM so the 5,000 RPM recommended is right on and is a great starting point.

  6. #6
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    60
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    4

    Default

    Quote Originally Posted by ToolHIT View Post
    A form tap in 6061 Aluminum should be at around 180-250 SFM so the 5,000 RPM recommended is right on and is a great starting point.
    Great, thanks everyone. So just so I understand, these formulas for calculating feed and rpm hold true for taps as well. For all CNC tooling?

    SFM = RPM X .262 X Tool Diameter
    RPM = SFM X 3.82 ÷ Tool Diameter
    IPM = RPM X IPT (CLPT) X Number of Flutes
    IPT = IPM ÷ (RPM X Number of Flutes)

  7. Likes ToolHIT liked this post
  8. #7
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    710
    Post Thanks / Like
    Likes (Given)
    108
    Likes (Received)
    474

    Default

    Quote Originally Posted by ProjectZero View Post
    Great, thanks everyone. So just so I understand, these formulas for calculating feed and rpm hold true for taps as well. For all CNC tooling?
    Calculating speed is the same for anything- SFM/dia*.26=RPM

    Feedrate for taps is simply RPM*pitch. A 1/4-20 has 20TPI. 1/20=.05" pitch. So a 1/4-20 tap at 1000 RPM would feed at 50 IPM. (1000*.05)

  9. #8
    Join Date
    Jan 2014
    Location
    Vancouver, WA. USA
    Posts
    2,384
    Post Thanks / Like
    Likes (Given)
    507
    Likes (Received)
    1170

    Default

    I program all small threads at 6k for aluminum. Since small threads are never very deep, the spindle never gets there, but it is tapping as fast as it can. So far so good....

  10. #9
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    710
    Post Thanks / Like
    Likes (Given)
    108
    Likes (Received)
    474

    Default

    Setting the R plane a little farther above Z zero can help get the RPM's up before the tap starts cutting. I usually put the R at Z.5 on small taps.

  11. #10
    Join Date
    Feb 2013
    Location
    Northern Mn
    Posts
    311
    Post Thanks / Like
    Likes (Given)
    76
    Likes (Received)
    359

    Default

    You guys are crazy I have spent more time and grief in my life picking broken taps out of expensive parts than I ever spent on tap cycle time. This would be different if I had thousands of holes to tap, but generally, I have a couple of tapped holes in each part. I run my cut taps at 500 and my roll taps at 750... and I still pucker up on each tapped hole. I have all of the numbers memorized for these RPMs and just before that evil little tap starts his first hole, I push pause, I look at the code and look for a G84, and check my feed rate and rpms... then I close my eyes, and hit the green button. While it is tapping that first hole in an expensive complicated part, I stomp my right foot repeatedly so I can neither hear, nor see that little MOFO break off in the hole.

    Did I mention that I hate taps They are just waiting for an opportunity to ruin your day.

    6-32 Cut Tap 500 RPM/ 15.625 IPM

    [On fast and tight machines and any sort of volume I will bump up to 1000 RPM/ 31.25 IPM]

  12. #11
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    16,274
    Post Thanks / Like
    Likes (Given)
    11824
    Likes (Received)
    11208

    Default

    Quote Originally Posted by ProjectZero View Post
    Great, thanks everyone. So just so I understand, these formulas for calculating feed and rpm hold true for taps as well. For all CNC tooling?
    How can it? cutting speed and feed are 2 different parameters.

    Speed is based on material being machined and cutter material, with workpiece and cutter rigidity having considerable effects.

    When milling or drilling, feed boils down to so much per tooth per revolution.

    When tapping or threading, feed HAS to be in the Z axis and can ONLY be the pitch of the thread per revolution, .or you will NOT get a thread.

  13. Likes Illinoyance liked this post
  14. #12
    Join Date
    Jan 2014
    Location
    Vancouver, WA. USA
    Posts
    2,384
    Post Thanks / Like
    Likes (Given)
    507
    Likes (Received)
    1170

    Default

    Quote Originally Posted by G00 Proto View Post
    You guys are crazy .....
    Maybe sometimes . I rarely work on really expensive pieces so that helps the pucker factor. I almost always drill or interpolate the hole near the max minor diameter. On some of my parts that have a fair amount of surfacing, I'll get the drilling and tapping done as early as practical then do the time consuming surfacing. That way if I do break a tap, then it's no where near as big a loss.

  15. Likes Hazzert liked this post
  16. #13
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    60
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    4

    Default

    Damn. I just broke my tap.

    First my mill was throwing an error "Thread Lead Not Specified". I go into my fadal user manual and look up the line is question. Sure enough I find G84, and it turns out the "Q" is missing. I trusted you, Fusion 360 CAM module! So first I manually add in Q.03125. Now my line of CAM looks like this:

    N815 G98 G84.1 X2.125 Y1.5625 Z-0.535 R0+0.15 S5000.2 F156.25 Q.03125
    But my tool still broke! It seemed go down fine, then to break upon reverse. What did I do wrong? I pre-drilled using a brand new .1065 drill bit. I can try G00 Proto's advice and knock the RPM down to 500 (from 5000!). Thoughts?

  17. #14
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,401
    Post Thanks / Like
    Likes (Given)
    2766
    Likes (Received)
    1954

    Default

    Quote Originally Posted by ProjectZero View Post
    Thoughts?
    Always start out slow, and run it without a part in the vise (or tool offset way above part)to see if it's running correctly.
    Your Fadal might not be able to tap at high speeds.

  18. #15
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    60
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    4

    Default

    Quote Originally Posted by Mtndew View Post
    Always start out slow, and run it without a part in the vise (or tool offset way above part)to see if it's running correctly.
    Your Fadal might not be able to tap at high speeds.
    I'll knock it down and try again. I'm not in any rush.

    About eight months ago - the first and only other time I tried rigid tapping on this machine - I successfully tapped about 100 1/4-20 holes. I checked the operation and my feed was at 500! Granted it took hours to do that, but that's unimportant right now.

  19. #16
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    3,401
    Post Thanks / Like
    Likes (Given)
    2766
    Likes (Received)
    1954

    Default

    Quote Originally Posted by ProjectZero View Post
    I'll knock it down and try again. I'm not in any rush.

    About eight months ago - the first and only other time I tried rigid tapping on this machine - I successfully tapped about 100 1/4-20 holes. I checked the operation and my feed was at 500! Granted it took hours to do that, but that's unimportant right now.
    500 doesn't seem right for 1/4-20. Does it use decimals? Can you post that line of code?
    Granted I don't know Fadal language, but 20 tpi is .05 per rev, and without decimals it would be shown as 500

  20. #17
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    60
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    4

    Default

    Quote Originally Posted by Mtndew View Post
    500 doesn't seem right for 1/4-20. Does it use decimals? Can you post that line of code?
    Granted I don't know Fadal language, but 20 tpi is .05 per rev, and without decimals it would be shown as 500
    The code I'm about to try right now, with my 6-32 machine tap, is this:

    N815 G98 G84.1 X2.125 Y1.5625 Z-0.535 R0+0.15 S500 F15.63 Q.03125
    I don't have the original code I ran to make my fixture plate but I regenerated it and the code I got was:

    N85 G98 G84.1 X1. Y0.5 Z-1.2756 R0-0.3 S500 F25.
    Again - Fusion 360's fadal postprocessor seems to be broken and it is not including the Q (screw lead/pitch) code.

  21. #18
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    1,828
    Post Thanks / Like
    Likes (Given)
    532
    Likes (Received)
    909

    Default

    Quote Originally Posted by Mtndew View Post
    500 doesn't seem right for 1/4-20. Does it use decimals? Can you post that line of code?
    Granted I don't know Fadal language, but 20 tpi is .05 per rev, and without decimals it would be shown as 500
    10,000 RPM is right at F500.

  22. #19
    Join Date
    Feb 2012
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,075
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    397

    Default

    I think it would have problems rigid tapping such small hole at high RPM

    Most of the machines I worked on did OK up to 2000 RPM.

    If you had a compensation holder, you could tap no problem.

  23. #20
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,685
    Post Thanks / Like
    Likes (Given)
    446
    Likes (Received)
    260

    Default

    Quote Originally Posted by G00 Proto View Post
    just before that evil little tap starts his first hole, I push pause, I look at the code and look for a G84, and check my feed rate and rpms... then I close my eyes, and hit the green button. While it is tapping that first hole in an expensive complicated part, I stomp my right foot repeatedly so I can neither hear, nor see that little MOFO break off in the hole.
    I used to hide behind the control until the first hole was successfully tapped. Still get stressed when I hit the start button when tapping.

    (And I only use floating holders)


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
  •