Page 1 of 2 12 LastLast
Results 1 to 20 of 31
  1. #1
    jrdeahl is offline Plastic
    Join Date
    Sep 2005
    Location
    Iowa
    Posts
    19

    Post

    Hi all:

    I did a search but didn't come up with any good links.

    I am looking for a thread depth chart. Not the calc of .75 divided by threads/in. I mean the actual depth of the threads or the "minor external diamension" subtracted from the "major external dimension".

    I don't always cut with the compound, but just use the cross.

    Thanks,

    Jake

  2. #2
    Gary E is online now Diamond
    Join Date
    Jan 2006
    Location
    Houston, TX
    Posts
    5,821

    Post

    Do you have a "Machinery's Handbook" ?

    Invest in one... even an OLD one...

  3. #3
    lathefan's Avatar
    lathefan is offline Titanium
    Join Date
    Nov 2003
    Location
    Colorado
    Posts
    2,120

    Post

    Divide one by the threads per inch and then multiply by .866

    Example: 16 threads per inch

    1/16 = .0625

    .0625 x .866 = .054 single depth of thread

    If you need a chart, work the formula above for all the common threads and make your own chart.

  4. #4
    Mike K is offline Cast Iron
    Join Date
    Nov 2002
    Location
    Southern Indiana
    Posts
    465

    Post

    Hi Jake,
    I have a thread gage (sometimes called a fishtail)that has the double depths listed for most of the threads. If you don't have one, I suggest getting one. They're handy for grinding and setting up thread tools too.

    If that isn't available, I just work from the one that I have memorized; 20 TPI = .065 double depth.

    As an example, say that you want to cut 16 TPI.
    20/16 = 1.25
    1.25 X .065 = .081
    16 TPI = .081 double depth.

    Works for me anyway.

    Mike

  5. #5
    mklotz is offline Aluminum
    Join Date
    Oct 2002
    Location
    Los Angeles, CA, USA
    Posts
    140

    Post

    Go to my page, download DOT (Depth Of Thread), run it and you'll get an output
    that looks like this...

    ----------------------------
    DEPTH OF THREAD CALCULATIONS

    Threads angle [60 deg] ?
    Threads per inch [20] ? 16
    Compound rest angle [29 deg] ?

    thread angle = 60.00 deg
    threads per inch = 16.0 (pitch = 0.06250 in/thread)
    {compound feed at compound angle = 29.0 deg}

    (A) dot sharp crest - sharp root = 0.05413 in {0.06189 in}
    (B) dot flat crest - flat root = 0.03383 in {0.03868 in}
    (C) dot sharp crest - flat root = 0.04059 in {0.04641 in}
    (D) dot flat crest - sharp root = 0.04736 in {0.05415 in}
    (E) double dot sharp crest - sharp root = 0.10825 in

    For American National (60 deg) thread form, subtract 0.0406 in from
    major diameter (assumes p/8 flat on crest) to obtain pitch diameter

    use any line on threading dial
    ----------------------------


    Regards, Marv

    Home Shop Freeware - Tools for People Who Build Things
    http://www.myvirtualnetwork.com/mklotz

  6. #6
    Gary E is online now Diamond
    Join Date
    Jan 2006
    Location
    Houston, TX
    Posts
    5,821

    Post

    Wich one is right?.. Is EITHER RIGHT???

    Divide one by the threads per inch and then multiply by .866

    Example: 16 threads per inch

    1/16 = .0625

    .0625 x .866 = .054 single depth of thread
    OR.........
    As an example, say that you want to cut 16 TPI.
    20/16 = 1.25
    1.25 X .065 = .081
    16 TPI = .081 double depth.

  7. #7
    SND
    SND is offline Diamond
    Join Date
    Jan 2003
    Location
    Canada
    Posts
    9,221

    Post

    Well I'll add another one in there.

    I normaly use this little formula. I'm not sure exactly why its this number works. I think it takes care of the normal root and crest sizes. Anyway, simple as can be. Only 1 number to remember, .625

    .625 devided by whatever TPI #

    .625/16 = aprox .040" depth per side. These numbers are only meant to get you somewhere close, pretty much just like looking at it. When its getting close to a true V shape, you're almost there and should get out the 3wires/ gages, or the mating part.

    I also use this formula for undercuts and I add a bit more for clearance. I never had any complaints.

  8. #8
    Gary E is online now Diamond
    Join Date
    Jan 2006
    Location
    Houston, TX
    Posts
    5,821

    Post

    So far NOBODY agrees... this is NOT funny....
    but somehow I sorta expect it...

    Do any of you make threads to the BOOK ?

    Get a "Machinery's Handbook"

    Every one of you would be royally Pi$$ed if the spark plugs you bought were made using your methods...

  9. #9
    jrdeahl is offline Plastic
    Join Date
    Sep 2005
    Location
    Iowa
    Posts
    19

    Post

    So what does the Machinery Handbook say?

    Jake

  10. #10
    lathefan's Avatar
    lathefan is offline Titanium
    Join Date
    Nov 2003
    Location
    Colorado
    Posts
    2,120

    Post

    --------------------------------------------------------------------------------
    Wich one is right?.. Is EITHER RIGHT???


    quote:
    --------------------------------------------------------------------------------
    Divide one by the threads per inch and then multiply by .866

    Example: 16 threads per inch

    1/16 = .0625

    .0625 x .866 = .054 single depth of thread

    --------------------------------------------------------------------------------

    OR.........

    quote:
    --------------------------------------------------------------------------------
    As an example, say that you want to cut 16 TPI.
    20/16 = 1.25
    1.25 X .065 = .081
    16 TPI = .081 double depth.

    --------------------------------------------------------------------------------
    So far NOBODY agrees... this is NOT funny....
    but somehow I sorta expect it...

    Do any of you make threads to the BOOK ?

    Get a "Machinery's Handbook"

    Every one of you would be royally Pi$$ed if the spark plugs you bought were made using your methods...
    Why don't you get your BOOK out and see which one is right?

  11. #11
    Mike K is offline Cast Iron
    Join Date
    Nov 2002
    Location
    Southern Indiana
    Posts
    465

    Post

    Gary E,
    By the time you have the thread data found in the handbook, The thread could already be cut! It just isn't all that technical.

    I stand by my "formula". I use that because I happen to be able to remember it.

    Another way to do it:
    Pitch X 1.3 = double depth (Handbook worshippers will probably want to use 1.299 in place of 1.3)
    These numbers are not for a pointed tool, but rather for a tool that has a proper flat at the tip. I think that this is where the descrepency comes from. The single depth of a thread with a sharp root is indeed .866 X pitch. These threads are weaker though.

    Incidently, all this was derived from the "Greenfield Screw Thread Manual" which I believe is still in print.

    Mike

  12. #12
    jrdeahl is offline Plastic
    Join Date
    Sep 2005
    Location
    Iowa
    Posts
    19

    Post

    Well, I must say I have calculated each of your formulas including the DOT program and none of you are the same.

    Since I don't have a handbook, what does it say?

    Jake

  13. #13
    SND
    SND is offline Diamond
    Join Date
    Jan 2003
    Location
    Canada
    Posts
    9,221

    Post

    It says it doesn't matter how you want to calculate it as long as the end result is good.

    Going with only a calculated depth without checking with 3wires or a ring gage is NOT acceptable in normal production where many parts have to interchange.

  14. #14
    mklotz is offline Aluminum
    Join Date
    Oct 2002
    Location
    Los Angeles, CA, USA
    Posts
    140

    Post

    Here you go...

    http://homepages.tesco.net/~A10bsa/uncpro.htm

    Regards, Marv

    Home Shop Freeware - Tools for People Who Build Things
    http://www.myvirtualnetwork.com/mklotz

  15. #15
    mklotz is offline Aluminum
    Join Date
    Oct 2002
    Location
    Los Angeles, CA, USA
    Posts
    140

    Post

    Here you go...

    http://homepages.tesco.net/~A10bsa/uncpro.htm

    Addendum: Note that, from the above page,

    hn = 0.54127/16 = 0.033829

    which agrees exactly with what my program calculates for
    dot-flat crest to flat root.

    Regards, Marv

    Home Shop Freeware - Tools for People Who Build Things
    http://www.myvirtualnetwork.com/mklotz

  16. #16
    Mike K is offline Cast Iron
    Join Date
    Nov 2002
    Location
    Southern Indiana
    Posts
    465

    Post

    SND,

    Good point. A formula is only good for getting you in the ballpark. Always stop feeding in a few thou shy of the calculated position and start gaging for the last bit.

  17. #17
    JS's Avatar
    JS
    JS is offline Hot Rolled
    Join Date
    May 2005
    Location
    Republic of Arizonia
    Posts
    848

    Post

    .130 / number of threads per inch

    example .130 / 12 = .01083333333

    For 75% thread I believe

  18. #18
    jrdeahl is offline Plastic
    Join Date
    Sep 2005
    Location
    Iowa
    Posts
    19

    Post

    JS:

    That is sounding good. My fishscale says .93 for 14tpi.

    so 13/14 = .92857

    .92857/2 = cross slide depth

    Correct?

    Jake

  19. #19
    John Garner is offline Stainless
    Join Date
    Sep 2004
    Location
    south SF Bay area, California
    Posts
    1,368

    Post

    Jake --

    The Theoretical Single Depth of Thread for either the Unified or ISO Metric threadform -- which are both 60-degree threads with a 1/8 Pitch flat at the Major Diameter and a 1/4 Pitch flat at the Minor Diameter -- can be calculated easily from the Thread Pitch:

    Theoretical Single Depth = (5/8) x Pitch x Cos (30 degrees)

    Working a numerical example for a Unified threadform of 1/16 inch Pitch:

    Theoretical Single Depth = (5/8) x 1/16 inch x Cos (30 degrees)

    = 0.625 x 0.0625 inch x 0.866

    = 0.0338 inch

    Working a numerical example for an ISO Metric threadform of 1.25 millimeter Pitch:

    Theoretical Single Depth = (5/8) x 1.25 millimeter x Cos (30 degrees)

    = 0.625 x 1.25 millimeter x 0.866

    = 0.677 millimeter

    The Unified and ISO Metric threadforms are modified (truncated) V screwthreads with a 60-degree included angle between the flanks. In a 60-degree Sharp-V screwthread, the measured-along-the-flank length would be exactly equal to the Pitch. The flats at the Major and Minor Diameters on the Unified and ISO Metric threadforms result in a reduction of the measured-along-flank length to 5/8 that of a same-pitch Sharp-V screwthread. [This means that the Theoretical Along-Flank Infeed of a compound / top slide set at 30 degrees to feed along the flank can be calculated as (5/8) x Pitch, which for a Unified threadform is exactly equal to (5/8) / Number of Threads per Inch.]

    The Single Depth of the screwthread is the measured-along-flank length of the screwthread times the Cosine of one-half of the V angle.

    Ok, the arithmetic says you can combine the 5/8 and Cos (30 degree) factors to create a "magic number", but doing so is a BAD idea. It would be far better to learn the fundamental geometry of the Unified / ISO Metric threadform well enough that you can re-derive the equations whenever you need them.

    That geometry really is pretty straight-forward, and once your understand it, the terms 5/8 and Cosine (30 degree) will come to mind far more readily and reliably than will magic numbers.

    John

  20. #20
    Forrest Addy is online now Diamond
    Join Date
    Dec 2000
    Location
    Bremerton WA USA
    Posts
    9,218

    Post

    I'm the only right one here. I hardly ever calculate thread data. I cut threads until they look like a thread then gage them with the nut or male thread, mike them over wires, or thread mike them if they're in range of the thread mikes I have.

    I also cut threads with the standard root flat P/4 to P/6) on the tool tip. Never cut threads with a pointy tool.

    All the thread data and the NIST formulae it takes to derive it from scratch are in Machinery's Handbook.

Page 1 of 2 12 LastLast

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
  •