Results 1 to 13 of 13
  1. #1
    Karl B. is offline Plastic
    Join Date
    Jul 2007
    Location
    Curtice, Ohio
    Posts
    6

    Default Roll Tap Tap Drill Size

    Hi everyone,

    I'm going to use a roll tap or thread forming tap on some spacers. The material is 1 1/4" round 6061 Aluminum. I'm expected to use a #10-32 go-nogo gage to check the threads. Some time ago, on this board, a few people suggested a roll tap to get the thread fit I need. i know you have to move up in tap drill size, but am at a loss for the tap drill size for a #10-32 thread. Can anyone give me some guidance on this one? Is there a table in the machinist handbook for example?

    Thanks all.......

  2. #2
    scojen's Avatar
    scojen is offline Stainless
    Join Date
    May 2004
    Location
    Zellwood, Fl.
    Posts
    1,117

    Default

    Look in the Machinist Handbook under Cold formed threads.

    Scott

  3. #3
    Gordon Long's Avatar
    Gordon Long is online now Hot Rolled
    Join Date
    Oct 2006
    Location
    San Leandro, California
    Posts
    515

    Default cold form tapping

    Hi Karl,
    Here's an online calculator to plug your numbers into.
    http://academic.evergreen.edu/projec...s-tap.htm#cold
    A #10 is .190" dia. so that figures to be .174" for the tap drill dia. if you use the figures for a standard 75% thread. A #17 drill would be the closest size.

  4. #4
    Jackmo is offline Hot Rolled
    Join Date
    May 2006
    Location
    South of Boston, MA. USA
    Posts
    773

    Default

    Hole size is critical to get 75% thread, check before tapping. You might need to go up or down in hole size to get the right fit for the gauge. If you use the tailstock make sure it aligned with the pc.

    Jackmo

  5. #5
    cncmoldman is offline Aluminum
    Join Date
    Apr 2006
    Location
    Tempe Az.
    Posts
    155

    Default

    OSG has a nice online calculator also.

    http://www.osgtool.com/Technical.asp?tid=1&id=1

    Good for cut taps and form taps in both inch and mm.

  6. #6
    Forrest Addy is offline Diamond
    Join Date
    Dec 2000
    Location
    Bremerton WA USA
    Posts
    9,385

    Default

    Careful there. The Karl is using a thread forming tap. It displaces metal from the hole walls to form the threads. A standard nominal dia minus thread pitch tap drill leaves too much stock. The metal will flow into the tap thread space, jamming the tap, and possibly breaking it.

    The starter hole for a thread forming tap has to be larger than for a thread cutting tap. The displaced metal fills the tap's thread space to about 75% or so. I suggest you try a few tapped holes in scrap starting with a tap drill = nominal dia minus 40% of the pitch. Most makers offer charts.

  7. #7
    Peter Neill is online now Hot Rolled
    Join Date
    Apr 2006
    Location
    Suffolk, England
    Posts
    825

    Default

    My Dormer Drills wall chart gives the following formula for calculating the tapping drill size for roll forming taps:

    D(inches) - 0.0068 x H / Threads per Inch
    Where H is the percentage of thread depth required (usually 65%)

    Peter

  8. #8
    Metalcutter's Avatar
    Metalcutter is offline Titanium
    Join Date
    Sep 2005
    Location
    San Diego
    Posts
    2,878

    Default

    Roll taps (thread forming)

    Make the pitch diameter good because they don't cut. It's the minor diameter you have to watch. Way lube works pretty well with them.

    Regards,

    Stan-

  9. #9
    John Garner is offline Stainless
    Join Date
    Sep 2004
    Location
    south SF Bay area, California
    Posts
    1,423

    Default

    Good Evening, Good People --

    This evening's sermon is given from high atop one of my very favorite soapboxes -- that understanding the fundamental geometry of the two most common threadforms, the Unified and ISO Metric threadforms, enables we of the proletariat to calculate thread-chart values for ourselves, in the absence sufficient reference material, without resort to memorized "magic numbers":

    As Forrest Addy describes, the rule of thumb to calculate the diameter of a hole to be threaded by material-removing methods (a cutting tap, single-pointing, or milling) for single-start US Standard, Unified, and ISO Metric threadforms is "Nominal Major Diameter minus Pitch". Either metric or imperial units may be used, but the same unit must be used for both Major Diameter and Pitch.

    A corresponding rule of thumb to calculate the diameter of a hole to be single-start threaded with a Unified or ISO Metric threadform forming tap is "Nominal Major Diameter minus the Single Depth of Thread", which is itself calculated from the basic threadform as "5/8 Pitch times Cosine 30 degrees". (Remember that the basic forms of the Unified and ISO Metric screwthreads are IDENTICAL . . . they both have a 60 degree flank angle, a 1/8 Pitch flat at the Major Diameter, and a 1/4 Pitch flat at the Minor Diameter.)

    I'll use a #10-32 Unified screwthread for a worked example:

    Nominal Major Diameter = 0.190 inch;

    5/8 = 0.625;

    Pitch = 1/32 inch = 0.03125 inch;

    Cosine 30 degrees = 0.866025.

    Hole Diameter = Nominal Major Diameter - 5/8 Pitch x Cosine 30 degrees

    Hole Diameter = 0.190 inch - 0.625 x 0.03125 inch x 0.866025

    Hole Diameter = 0.190 inch - 0.016915 inch

    Hole Diameter = 0.173 inch after rounding to 3 decimal places.

  10. #10
    SND
    SND is offline Diamond
    Join Date
    Jan 2003
    Location
    Canada
    Posts
    9,337

    Default

    I didn't read the whole thread but I've usually heard TDS for roll taps is right around pitch diameter. Usually best to try one in a piece of scrap first and see what the final ID is, it usually has a fairly open tolerance anyway.

  11. #11
    Question Boy's Avatar
    Question Boy is offline Hot Rolled
    Join Date
    May 2005
    Location
    Napa, California
    Posts
    946

  12. #12
    CharlieBiler is offline Hot Rolled
    Join Date
    Mar 2005
    Location
    Connellsville PA
    Posts
    560

    Default

    Karl B.
    Here is a simple chart that has percentage of threads for cut and formed threads. This data is from several sources and is one of those long hair academic exercises; There is source material that was traced. This chart is updated and expanded about once a year to include the latest bastard and obsolete information.

    Hey; its free.................http://www.molineparts.com/images/36x96.pdf

    Break out the magnifying glass if you print it out normally. This chart is 24" by 70" in normal size. When it prints you can hear the ink being sucked down as the plotter grinds on.

  13. #13
    CoolHand's Avatar
    CoolHand is offline Hot Rolled
    Join Date
    Sep 2005
    Location
    Missouri . . . Near the Middle.
    Posts
    522

    Default

    For thread forming #10-32 holes in 6061 T-6 aluminum stock, I usually use a 0.177" drill (IIRC that's a #16). If your fit class is tight, I'd start in scrap with John Garner's info in post #9 and start out with a 0.173" (#17) and then check it against your gage.

    Gotta love them roll forming taps. It's been years since I broke a tiny tap.

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
  •