Rigid Tapping Feeds/Speeds in AL6061 - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 56
  1. #21
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,744
    Post Thanks / Like
    Likes (Given)
    494
    Likes (Received)
    273

    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)

  2. #22
    Join Date
    May 2005
    Location
    CA
    Posts
    950
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    169

    Default

    ProjectZero,

    If you're using Fusion360, this should be absolute cake. I tap all the time and have never had a single issue, and have *never* had to manually edit code (on Haas SMM).

    The thread pitch is set in your tool definition. (see image below). I don't like to be in a big hurry tapping, so on something like a 1/4-20 in aluminum, which is my example here, I'll have the RPM set at 1000 in the tool definition.

    Select "Drilling" from the toolbar at the top, select your tool/tap in the first tab, and make sure you select "Right Tapping" from the drop-down in the 4th tab. -- (note: you may be selecting "Tapping" instead or "Right Tapping"? If so, that's the setting used for a tapping head, not for rigid tapping).

    That's pretty much it.

    PM

    1.jpg

    2.jpg

  3. #23
    Join Date
    Jun 2008
    Location
    Toronto, Canada
    Posts
    255
    Post Thanks / Like
    Likes (Given)
    69
    Likes (Received)
    60

    Default

    It is my understanding that Fadal likes to tap in high gear. So if your rpm is under 2500, make sure you enter it like SXXX.2

  4. #24
    Join Date
    Nov 2012
    Location
    Phoenix,AZ.
    Posts
    96
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    60

    Default

    What Format are you using on your Fadal?
    Format 1 uses a "Q" value. Format 2 doesn't. It uses "S" and "F"(F = RPM/TPI). 5000 rpm seems pretty fast for a Fadal.

  5. #25
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    2,670
    Post Thanks / Like
    Likes (Given)
    739
    Likes (Received)
    1433

    Default

    CALLING ALL Jalapeño eaters!!! Or growers or whatever you do down there Bob.

  6. #26
    Join Date
    Jun 2007
    Location
    Garland TX
    Posts
    364
    Post Thanks / Like
    Likes (Given)
    138
    Likes (Received)
    89

    Default

    Quote Originally Posted by ProjectZero View Post
    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?
    G99 G84 X-2.4958 Y-2.5082 Z-0.5 R0.25 F15.63 The Q should make the cycle peck, I'd leave that out

  7. #27
    Join Date
    Oct 2005
    Location
    Wilmington DE USA
    Posts
    1,833
    Post Thanks / Like
    Likes (Given)
    271
    Likes (Received)
    358

    Default

    Thought I'd share this since it surprised me.
    I have a 95 NTC vmc that sometime real soon I need to replace the spindle drive belt.
    Been putting it off, have it planned for Christmas shutdown (vacation, whats that)
    Sheet metal, rigging the motor....

    Haven't tapped with the machine probably in a year.
    Have a job that requires (16) 1/4-20 holes in 1/2" 6061, customer supplied material, already has work done to it. (18" square plate)
    Since the belt had me worried and after reading some of the above post I decided to do a test run to make sure the belt wasn't going to be a problem.
    In the past I've been running 800rpm F40.00 for a G84 tapping cycle w/form tap. Its always worked.
    In a test today the tap was coming up short and machine was not happy at the retract.
    Looked into a few tap manufactures web sites and most mentioned additional hp needed to run form taps...and they like to run faster than cutting taps.

    Set up a sample to run 2000rpm F100 and made great threads with smaller entry burr, machine is happy.
    Not sure if I want to venture into 4k rpm range but I now believe being conservative is not always a good thing.

  8. #28
    Join Date
    Nov 2003
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    1,311
    Post Thanks / Like
    Likes (Given)
    172
    Likes (Received)
    229

    Default

    Assuming your Fadal has the rigid tap option.

    Is your CAM outputting the G84.2 call to slave the Z travel to the spindle rotation? I'm a bit of a Fadal newbie, but at least in the CNC-88 control, the synchronization is not automatic - if your gcode doesn't include the G84.2 line, it's going to shave the thread or break the tap.

    The Fadal manual recommends rigid tapping in the high speed range, e.g. S1000.2, and at 1000 to 2000 rpm for best results. It isn't clearly stated in the manual but I think that has to do with accuracy of the synchronization.

    Example of rigid tapping M2, 1998 Fadal 4020, CNC 88, Format 2:

    (TOOL #14 M2 form tap)
    N2615 T14 M06
    N2620 G90 S2000.2 M05 G08
    N2625 G84.2
    N2630 G00 G90 X.125 Y-2.3913
    N2635 Z1.072 H14 D14 M08
    N2640 G84.1 G98 X.125 Y-2.3913 Z.6748 S2000.2 F31.496



    To date I've only broken taps in this machine due to my own oops, never to a fault of the machine.

    Bob

  9. #29
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    Thanks everyone. I have a part tomorrow where I need to tap both 2-56 (yikes) holes and 10-24 holes in aluminum 6061. The hole are quarter inch deep.

    I'm torn between going with G00 Proto and tapping all holes at F500 and taking my sweeeet time and hopefully not breaking a tap

    OR

    trying Toolbert's recommendation of S1000.2. The last time I tapped 6-32 I used this line:
    N230 G98 G84.1 X4.525 Y3. Z-0.5 R0+0.2 Q0.0312 F1250.2
    And it was FAST (after that F500 I did last time) and scared me. I definitely don't know about that for my 2-56 machine taps.

    Thoughts? Appreciate the advice already!
    Last edited by ProjectZero; 12-06-2017 at 12:25 PM.

  10. #30
    Join Date
    Feb 2013
    Location
    Northern Mn
    Posts
    414
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    463

    Default

    Take what I said with a grain of salt. I know almost nothing about Fadal machines, so they may have their own idiosyncrasies. That being said, I had to tap 50 3-48 holes yesterday on a batch of parts. I only had two taps that I borrowed from my neighbor... oops. I tapped them at 500 RPMs and (1/48 X 500 = 10.417 IMP). They all came out great with no broken taps.

    I can't remember all that has been pointed out earlier in this thread, so I'll lay out a few more of my ground rules (mostly applicable to expensive proto parts and molds). I apologize if some of them are overly basic.

    Always make the tap drill hole as deep as possible, especially with cut taps. I used to try and skank by with .050-.100 deeper than the tap. Any more, if I have the room I'll go even deeper. Those chips get shot forward and pack the hole. They can bust taps, be difficult to clean out, and can gum up or gall a screw. This is less important with roll taps or thread milling.

    Watch how deep the tapped hole is in relation to the size of the tap. The 10-24 hole 1/4" deep is no problem; 5/8" deep could be a problem. 1/4" deep on a 2-56 would start to have me be a little concerned. (I think 4x diameter might be a reasonable limit ???)

    If the part is expensive, or you are approaching a depth that has you concerned, or you aren't able to make the tap drill hole substantially deeper than the tap; don't be too proud. Rigid tap it 4-5 full rotations deep, and then finish it by hand. Make sure to use the same type of tap to finish it as you started... don't start with a roll tap and finish it with a cut tap. It won't gage out.

    Coolant concentration can make a big difference on tapping. If it is mixed a little thin, or of questionable quality don't be afraid to stop the machine with an M00 in the program and use a brush to put on some Tap Magic, Moly-Dee or similar cutting fluid. It seems like a waste of time, but it can save a tap. I used to do this all the time (M00 in my post), but I haven't needed to in the last ten years. I think it may be because of the new coolant I am using, or I've been lucky.

    Floating tap holders may or may not be required in your machine. This depends on if it has rigid tapping, and the machine dynamics. Big slow machines, and worn out machines may not have the fine motion and speed to do synchronized tapping. I haven't needed one for 20 years so I am no expert.

    Use gage pins on you tap drilled hole (especially on a 2-56 or smaller), there is an allowable range and you can cheat it towards the big side (<<75% thread engagement) and still pass and retain adequate strength; use the tolerance to your advantage. I once had a production batch of Mil parts in exotic material with very small tapped holes (something less than 2-56 I think). I was busting taps or failing with the thread gage, chasing the diameter of the tap drill. Fought it for better part of a day. I finally ended up having to buy reamers in .001" increment between the two tap drill sizes. Found the right one and the rest of the job ran with no issues.

    Lastly, confirm and re-confirm tap drill size. I had a new set-up guy once doing a series of parts with three different sized holes in them. The first set of 6-32 holes were marginal, but passed. The 8-32 holes had issues with getting them to gage out and the threads looked horrible, plus he broke a couple of taps. The last op had 10-24 holes and they worked fine. I was confused as hell why the 8-32's didn't work, but the 6's and 10's looked pretty good. So I asked him what tap drill size he was using. For the 6-32's he was using a #32 drill a little loose, but almost within range; for the 10-24 he was using a #24... reasonable; and the 8-32 he went back to the #32, way too small. I was like WTF, the set-up sheet says to use the 6-32 tap drill size... He looked at me point blank and said, he assumed that the second number in 6-32 was the tap drill size.

  11. #31
    Join Date
    Feb 2009
    Location
    Midwestern MN/Wi USA
    Posts
    1,260
    Post Thanks / Like
    Likes (Given)
    70
    Likes (Received)
    332

    Default

    Start slow....CHRYSLER MAN!!

    G84.1 G98 Z-1.25 R.2 S1280 F40.

    Your Fadal probably poops out like they all did at about 3000rpm. You cannot tap fast than 3000rpm on a Fadal without having to pull a broken tap out of your work piece.

  12. #32
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,086
    Post Thanks / Like
    Likes (Given)
    583
    Likes (Received)
    1568

    Default

    Quote Originally Posted by G00 Proto View Post
    ....... He looked at me point blank and said, he assumed that the second number in 6-32 was the tap drill size.
    He was working as a setup guy?!!!

  13. #33
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    This is a wealth of unfortunate, G00. Thank you for writing it all out!

    You know, I've put such a focus on machine-tapping because I kept breaking taps when I tried to tap by hand! In my workpiece. After milling the part out! Even when I reamed out the holes on the drill press to make sure they were to size. Eventually I said screw it, the CNC can tap better than I can. Going slow, all the Tap Magic in the world too...

    The 6-32 holes my CNC succeeded in tapping when I failed were .45" deep. I like your 4x rule of thumb but I'm hoping the mill can handle deeper.

    I think I'll just go F500 for the 6, 10, and 2-56 holes and hope for the best. And I will definitely check the size of my pretap drill bits!

  14. #34
    Join Date
    Feb 2013
    Location
    Northern Mn
    Posts
    414
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    463

    Default

    Quote Originally Posted by Vancbiker View Post
    He was working as a setup guy?!!!
    Yep, all the way until the end of the day. Paid him up, and sent him on his way It turns out some people aren't 100% truthful on their resume.

  15. #35
    Join Date
    Feb 2013
    Location
    Northern Mn
    Posts
    414
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    463

    Default

    Quote Originally Posted by ProjectZero View Post
    This is a wealth of unfortunate, G00. Thank you for writing it all out!

    You know, I've put such a focus on machine-tapping because I kept breaking taps when I tried to tap by hand! In my workpiece. After milling the part out! Even when I reamed out the holes on the drill press to make sure they were to size. Eventually I said screw it, the CNC can tap better than I can. Going slow, all the Tap Magic in the world too...

    The 6-32 holes my CNC succeeded in tapping when I failed were .45" deep. I like your 4x rule of thumb but I'm hoping the mill can handle deeper.

    I think I'll just go F500 for the 6, 10, and 2-56 holes and hope for the best. And I will definitely check the size of my pretap drill bits!
    You should never break a tap by hand (ok, I might have once). The key is to get them going straight from the start. I will often use a spring loaded guide if I am starting from scratch. It is basically a spring loaded center that goes either into a center drilled spot in the tap, you load it into a tool holder and bring it down. They are pretty cheap. High value projects get this treatment. But honestly, if you start the threads in a machine, and then use a hand tap, it is already started square and shouldn't be an issue. Use good cutting oil.

    .45 deep with a 6-32 is risky. There is such thing as peck tapping (depending on the machine). Never had to resort to it, but it is an option.

  16. #36
    Join Date
    May 2013
    Location
    wi usa
    Posts
    179
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    53

    Default

    my experiences over the years on many different brands of machines on aluminum is some machines we can run faster rpm 1000+ and runs with no problems, other can't go faster then 500rpm and make good threads. Some machines can't keep rpm and feed consistent if you get going to fast and end up with bad threads.
    It not really age of machine, we have old Mori that can tap faster then are newer Mazak and YCM and fine threads seem to be worse then course at times far as machine speeds and rpms. We run same programs on different brands of machines and some I need to slow them down when tapping.

    500 to 700 rpm is usually my starting point because I know it will normally run on all shops machines

    D

  17. #37
    Join Date
    Oct 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    6

    Default

    I'm shite at hand tapping. I might need to look into your spring loaded part. But my aesthetic right now is to do everything on machine because it's a more reliable beast than I am.

    My 2-56 and 10-24 holes came out great today. No taps broken! I set RPM to 500 for both. Seemed terribly fast on the 2-56 holes and I nearly had a heart attack but the tap didn't break, I guess the math worked out. The line of code was:

    N1285 G98 G84.1 X3.175 Y3.2313 Z-0.5 R0+0.075 Q0.0179 F500.
    Hurray! 500 for life.

  18. #38
    Join Date
    Feb 2009
    Location
    Midwestern MN/Wi USA
    Posts
    1,260
    Post Thanks / Like
    Likes (Given)
    70
    Likes (Received)
    332

    Default

    I have to wonder here...... you only ever broke one tap and think .45 is a risky depth for a 6-32.

    Quote Originally Posted by G00 Proto View Post
    You should never break a tap by hand (ok, I might have once). The key is to get them going straight from the start. I will often use a spring loaded guide if I am starting from scratch. It is basically a spring loaded center that goes either into a center drilled spot in the tap, you load it into a tool holder and bring it down. They are pretty cheap. High value projects get this treatment. But honestly, if you start the threads in a machine, and then use a hand tap, it is already started square and shouldn't be an issue. Use good cutting oil.

    .45 deep with a 6-32 is risky. There is such thing as peck tapping (depending on the machine). Never had to resort to it, but it is an option.

  19. Likes DavidScott liked this post
  20. #39
    Join Date
    Feb 2013
    Location
    Northern Mn
    Posts
    414
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    463

    Default

    Quote Originally Posted by Speedie View Post
    I have to wonder here...... you only ever broke one tap and think .45 is a risky depth for a 6-32.
    I may have typed faster than I can think... it happens. I think .450 deep with 6-32 is very risky rigid tapping in one shot. Too many things can go wrong, and you're going to break some. I think the max number of 4x the major diameter may be a pretty good number (even though I pulled it out of my ass), I might even go as far as say 3x major diameter is about max.

    I'm pretty sure I have only broken a couple of taps by hand... but I may be blocking out some of the more painful ones. I do recall one of my people breaking a handful of 10-32 taps by hand, but he weighed about 350 and had just retired from a reasonably successful football career, that destroyed any semblance of feeling in his hands. I finally told him that I would do all of the hand tapping for anything less than 1/4-20

    I'm pretty humble when it comes to rigid tapping. Most of the times it works for me... but when it doesn't, it really can bite you. I'm pretty confident that if the tap is started square with the work piece, I can tap as deep as needed by hand. I have needed to. It required relieving the tap (or using a pulley tap), and a judicious amount of cutting fluid.

    Anyhow, if I misspoke, I apologize. Oddly enough I have to get back to making parts with .400" deep 6-32 threaded holes. Running pretty good. Same tap for >1000 parts.

  21. #40
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    39
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    8

    Default

    I also remember using G84.2 (prepare for rigid tap on Fadal) Side note 6-32 cut taps are the worse one's . Pitch size to minor dia is the problem especially in tool steel.


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
  •