Rigid Tapping Feeds/Speeds in AL6061 - Page 3
Close
Login to Your Account
Page 3 of 3 FirstFirst 123
Results 41 to 56 of 56
  1. #41
    Join Date
    Jul 2012
    Location
    Washington
    Posts
    2,053
    Post Thanks / Like
    Likes (Given)
    744
    Likes (Received)
    808

    Default

    On the 1997 Fadal I worked on, until 2004, I never had machine related problems tapping, either ridged or tapping head. The installation tech said to limit rigid tapping to 2k even though it would do 3k because the spindle drive would not last, just not up to it, so that was my limit for ridged tapping. I tapped down to 00-80 with no problems in standard ER collets with decent coolant, almost all was form taps in aluminum. With form taps you should check the hole diamater the drill is drilling, size of drill just means it should be right, not that it is. I never peck tap and never have problems with deep threaded holes, even so deep I have to relieve the shank to get the thread depth. One thing I have found is it is worth getting the corect coating on the tap, which means you have to special order it. This is no big deal with Balax and only costs a dollar or so more and 1 or 2 days for chrome, which is what they suggest for 6061 aluminum. The coating really helps when you are form tapping 90-100% threads.

  2. #42
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    I'm lucky that my parts are aluminum. Probably makes this a lot less painful than steel.

  3. #43
    Join Date
    Oct 2005
    Location
    Wilmington DE USA
    Posts
    1,817
    Post Thanks / Like
    Likes (Given)
    268
    Likes (Received)
    357

    Default

    Followup of my earlier post.
    I had planned on replacing the spindle drive belt during Christmas break.
    Ran a test at 2000rpm for 1/4-20 F100.00 with a floating holder, form tap(new) and got good results
    2nd hole into the 18" square plate the tap attempts to become part of the plate.
    Feed hold won't work in tapping mode, aw shit, hit the big red button.
    Was able to remove the tap without breaking it, the "hole" came out with the tap.
    Customer allowed a thread insert for the one hole, finished out the tapping on the manual mill

    Last weekend became belt change time.
    I had ordered (using the manufacturers manual for a part# ) a belt 3 months ago in preparation as it was a 3 week lead.
    Saturday morning turn on the radio, fresh pot of coffee, no one to bug me, dig into the spindle and find out the belt I ordered wasn't evan close. (it did match what I ordered, the machine builders fault.)
    Lucked out and was able to measure the old belt, found 2 on ebay , nos, and reassembled today.
    Set up a test tap 33 holes in 1/2" 6061 using the S2000/F100, all 33 holes look great

    So if your having problems with tapping and everything else has been ruled out, check your spindle belt.
    Unless you have a gear drive.

    The slippage I was getting at reversing was enough to throw off the balance between the holder extending/floating a little and the limit

  4. #44
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    Sorry to bring this thread back yet again but I need help again. I've broken two 6-32 rigid taps this morning and I have no idea why. I thought I'd really gotten it down to a science with my 500 feed rate and my properly generated GCode. This is clearly not the case.

    I don't know what's wrong. I'm remachining a part I machined before and successfully rigid tapped. The only thing that has changed is the thickness by .050. I've made 100% certain that I'm using the right pre-drill (.1065, #36) and that the pre-drill hole is all the way through the stock. After I broke the first tap I dropped my speed from 500 to 300 but the tap still snapped when I tried again. There must be something I'm missing.

    N560 G98 G84.1 X2.125 Y1.5625 Z-0.525 R0+0.175 Q0.0312 F300.
    Does anyone see an error in this line of code? Or know what could be going wrong? It goes all the way down, and then snaps like a twig upon reverse.

    Here is the full block. The only thing I can think that has changed is that I added the G8 line to all blocks of code when I manipulated the post-processor so I didn't have to add it manually to every milling operation. Would it possibly cause an issue here?

    (DRILL6)
    N490 M9
    N495 M1
    N500 T3 M6
    N505 S300 M5
    N510 E1
    N515 M8
    N520 G84.2
    N530 G8
    N535 G0 X2.125 Y1.5625
    N540 H3 Z0.6
    N550 Z0.2
    N560 G98 G84.1 X2.125 Y1.5625 Z-0.525 R0+0.175 Q0.0312 F300.
    N565 X2.0375 Y1.3125
    N570 X1.4625
    N575 X1.375 Y1.5625
    N580 G80
    N585 Z0.6
    N595 G9
    N600 M5
    N605 H0 Z0.

  5. #45
    Join Date
    May 2005
    Location
    CA
    Posts
    928
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    163

    Default

    If you are roll tapping, that tap drill is WAAAY too small.

    See below:

    2.jpg

  6. #46
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    Quote Originally Posted by precisionmetal View Post
    If you are roll tapping, that tap drill is WAAAY too small.

    See below:

    2.jpg
    I'm making chips with a typical 6-32 machine tap from mcmaster! McMaster-Carr

  7. #47
    Join Date
    May 2005
    Location
    CA
    Posts
    928
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    163

    Default

    Well... did a quick test post for my Haas, and here is what I get:


    O01001 (6-32 test)
    (Using high feed G1 F500. instead of G0.)
    (T9 D=0.138 CR=0. - ZMIN=-0.525 - right hand tap)
    N10 G90 G94 G17
    N15 G20
    N20 G53 G0 Z0.

    (Drill1)
    N30 T9 M6
    N35 S2000 M3
    N40 G54
    N45 M8
    N55 G0 X0. Y0.
    N60 G43 Z0.6 H9
    N70 G0 Z0.2
    N75 G98 G84 X0. Y0. Z-0.525 R0.2 F62.5
    N80 G80
    N85 G0 Z0.6

    N90 M5
    N95 M9
    N100 G53 G0 Z0.
    N110 X0.
    N115 G53 Y0.
    N120 M30



    One quick question: how thick is the material you are tapping? Are you sure that you have full-depth cutting clean through the bottom of the hole? If not, then reversing with the tap having come to a stop not cutting clean through "might" have something to do with it, especially since a 6-32 is pretty much the weakest tap there is (strength to cutting depth ratio). Only guessing...

    1/2" (.525" to the tip I assume) is a fairly deep thread for a 6-32 cut tap, IMO.

    pM

  8. #48
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    Quote Originally Posted by precisionmetal View Post
    Well... did a quick test post for my Haas, and here is what I get:


    O01001 (6-32 test)
    (Using high feed G1 F500. instead of G0.)
    (T9 D=0.138 CR=0. - ZMIN=-0.525 - right hand tap)
    N10 G90 G94 G17
    N15 G20
    N20 G53 G0 Z0.

    (Drill1)
    N30 T9 M6
    N35 S2000 M3
    N40 G54
    N45 M8
    N55 G0 X0. Y0.
    N60 G43 Z0.6 H9
    N70 G0 Z0.2
    N75 G98 G84 X0. Y0. Z-0.525 R0.2 F62.5
    N80 G80
    N85 G0 Z0.6

    N90 M5
    N95 M9
    N100 G53 G0 Z0.
    N110 X0.
    N115 G53 Y0.
    N120 M30



    One quick question: how thick is the material you are tapping? Are you sure that you have full-depth cutting clean through the bottom of the hole? If not, then reversing with the tap having come to a stop not cutting clean through "might" have something to do with it, especially since a 6-32 is pretty much the weakest tap there is (strength to cutting depth ratio). Only guessing...

    1/2" (.525" to the tip I assume) is a fairly deep thread for a 6-32 cut tap, IMO.

    pM
    The second time around I double checked that the pre-drill hole had been drilled, full depth, all the way through the stock. I actually took a spare drill bit of the same size and stuck it through the hole to make sure there wasn't anything weird going on at the bottom of the hole.

    It's just weird because I breezed through four of these parts with the exact same parameters 6 weeks ago. I'm cutting AL6061. Maybe I should try tapping halfway down the hole and then doing the rest off machine.

  9. #49
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    2,199
    Post Thanks / Like
    Likes (Given)
    8945
    Likes (Received)
    2593

    Default

    Seems to me every time one of these "I did it fine last time, and now I can't get it to work" in aluminum threads comes up, the more experienced members here point out that Chinese aluminum has been of dubious quality/repeatability from batch to batch, as of late.

  10. Likes Limy Sami liked this post
  11. #50
    Join Date
    May 2004
    Location
    Paradise, Ca
    Posts
    2,110
    Post Thanks / Like
    Likes (Given)
    611
    Likes (Received)
    1030

    Default

    Quote Originally Posted by TeachMePlease View Post
    ...Chinese aluminum has been of dubious quality/repeatability from batch to batch, since the dawn of time.
    A slight correction.

  12. #51
    Join Date
    May 2005
    Location
    CA
    Posts
    928
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    163

    Default

    I suppose the latest batch of taps that ProjectZero purchased could also be Chinese and of dubious quality?


  13. #52
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    2,442
    Post Thanks / Like
    Likes (Given)
    673
    Likes (Received)
    1296

    Default

    Quote Originally Posted by ProjectZero View Post
    It's just weird because I breezed through four of these parts with the exact same parameters 6 weeks ago. I'm cutting AL6061. Maybe I should try tapping halfway down the hole and then doing the rest off machine.
    Or you could do the exact same thing--INSIDE the machine, called peck tapping, by adding a Q value to the G84 line adding a peck amount.

    @TMP, I have noticed that response a lot more lately also, but that response (chitty material) is dubious in itself IMO. Likened to the guys who respond to tough jobs with "can't do it, send it EDM"-(pussies)

    R

  14. #53
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    Quote Originally Posted by litlerob1 View Post
    Or you could do the exact same thing--INSIDE the machine, called peck tapping, by adding a Q value to the G84 line adding a peck amount.

    @TMP, I have noticed that response a lot more lately also, but that response (chitty material) is dubious in itself IMO. Likened to the guys who respond to tough jobs with "can't do it, send it EDM"-(pussies)

    R
    Definitely. HSMWorks has a "Tapping with Chip Breaking" function that I haven't used yet. I'm going to put some half inch thick test stock in and try to use this functionality, see if this helps. What would you recommend my Pecking Depth be?

  15. #54
    Join Date
    Oct 2013
    Location
    New Jersey
    Posts
    849
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    714

    Default

    Quote Originally Posted by ProjectZero View Post
    Sorry to bring this thread back yet again but I need help again. I've broken two 6-32 rigid taps this morning and I have no idea why. I thought I'd really gotten it down to a science with my 500 feed rate and my properly generated GCode. This is clearly not the case.

    I don't know what's wrong. I'm remachining a part I machined before and successfully rigid tapped. The only thing that has changed is the thickness by .050. I've made 100% certain that I'm using the right pre-drill (.1065, #36) and that the pre-drill hole is all the way through the stock. After I broke the first tap I dropped my speed from 500 to 300 but the tap still snapped when I tried again. There must be something I'm missing.



    Does anyone see an error in this line of code? Or know what could be going wrong? It goes all the way down, and then snaps like a twig upon reverse.

    Here is the full block. The only thing I can think that has changed is that I added the G8 line to all blocks of code when I manipulated the post-processor so I didn't have to add it manually to every milling operation. Would it possibly cause an issue here?
    Didn’t put the spindle in high range for rigid tapping.

  16. #55
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    Quote Originally Posted by garyhlucas View Post
    Didn’t put the spindle in high range for rigid tapping.
    Should I manually change it to S500.2, rather than S500. ?

  17. #56
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    2,442
    Post Thanks / Like
    Likes (Given)
    673
    Likes (Received)
    1296

    Default

    Quote Originally Posted by ProjectZero View Post
    Definitely. HSMWorks has a "Tapping with Chip Breaking" function that I haven't used yet. I'm going to put some half inch thick test stock in and try to use this functionality, see if this helps. What would you recommend my Pecking Depth be?
    The reason to use peck tapping is if A. the chip is what is messing with you. or B. too much torque for the tap. In really tough material I will peck 1 diameter. IF you peck make sure the runout on the tap is good, and the spindle is slow.

    I also agree with low gear, do whatever you need to to get it in low gear 500.2 or 499 or whatever. M41 sometimes.


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
  •