No announcement yet.

???Threading tool difference

  • Filter
  • Time
  • Show
Clear All
new posts

  • ???Threading tool difference

    Ok I have two threading charts and they both show two different depths of thread for a V form tool and a UN *(unified) form tool. My question is do you consider a lay down threading insert. That is a (16) tpi non UN insert a V form tool?*

  • #2
    Well, if you wanna get REALLY into it, theres diffrent thread classes (tollerance ranges) for verious fits.

    That might explain the diffrence in the charts.

    Does not matter if its lay down or stand up, If its got a sharp point, its V thread.

    If its an insert speced for only a small range of threads (like 16~20tpi), then its UN form.

    If its a sharp V thats been rounded off, Who knows exactly how deep you gotta cut for the TPI at hand, Best to have a test nut/bolt!
    Play Brutal Nature, Black Moons free to play highly realistic voxel sandbox game.


    • #3
      Your question is ambiguous.

      V threads are obsolete. You don't use a V thread chart just because you are (incorrectly) attempting to make a UN thread with a sharp V tool. More changed than the tip of the tool between V threads and various editions of UN threads.

      Ignore thread depth charts, they are useless for most purposes. You cut a thread based on pitch diameter (thread wires or thread micrometer), not depth. with an adjustment for clearance based on the thread class.

      You can cut an external thread with any thread radius that insures the thread flanks are fully cut everywhere but within the bottom 1/4H of the theoretical V thread (1/8H for an internal thread) but the smaller the radius the weaker the bolt. For professional work where strength is an issue you should ideally have a different nose radius tool for each thread pitch. For most home shop stuff you can use a smaller selection of nose radii.
      Add an extra line to that graph at 1/8H from the theoretical V root of the external thread. Your tool isn't allowed to remove any metal below that line.

      For UN threads, you are allowed to have a flat tip or a radius. For UNR threads, you are required to have a radius not less than 0.10825 times thread pitch (but not so large it doesn't fully cut the thread flanks at 1/4H from the imaginary V root).

      p=thread pitch (1/TPI), same as lead for single start threads
      H=0.86603p Height of fundamental triangle 0.86603=sin(60degrees)

      Your nose radius should be such that (for zero clearance and external threads) the tool profile falls inside the 1/4H triangle but not in the 1/8H triangle at the theoretical point of the tool. This implies that the tool can't be used for more than a 2:1 range of thread sizes (and less when you allow For grinding error, clearances, and tool wear).

      You can almost meet the specs by grinding tools with almost the maximum allowed tip radiuses for the following sizes:
      80TPI use for 41-80TPI
      40TPI use for 21-40TPI
      20TPI use for 11-20TPI
      10TPI use for 6-10TPI
      Leave a little for tool wear and thread class clearance. Adding 7, 14, 28, and 56 and you should be able to meet specs. When a tip becomes too worn, regrind it for the next coarsest size.
      Last edited by whitis; 07-31-2011, 01:28 AM.


      • #4
        Originally posted by whitis
        When a tip becomes too worn, regrind it for the next coarsest size.
        Better yet, Grind bits to the job at hand (Or rather, to the spec of one of the 8 thread pitchs you listed), from one of your least used, finer threading bits

        This way you only grind the bits you need, And your bits stay sharp. No need to grind em all at once.
        Play Brutal Nature, Black Moons free to play highly realistic voxel sandbox game.


        • #5
          I understand about using wires and thread mikes. I guess I will have to look into some new tools. And just perches some UN threading inserts for the most common threads I make. I don't think there is a go-nogo gauge for the threads I usually turn.


          • #6
            jeremy13, I have a stand up insert threading holder and I just buy a standard insert for it and it has the same radius or flat on the tip for every thread it will cut up to the length of the sides of the insert. After that you need a wider insert for a coarser thread. I also cut a lot of threads with a HSS cobalt ground cutter.

            In all the job shops I have worked no one considered putting a radius on the tip of the threading cutter. Sometimes we may put a flat on the tip to keep the tip from wearing or breaking off and ruining the thread. For most the threading you will do you don't have to concern yourself with a tip radius or flat but you can if you want to.

            Everything that whitis said is right and is the correct way to do it. The truth is that is seldom done in job shops and most often done when specified by the customer or required by the shop.

            If you grind a threading tool with a sharp tip the strength of the threaded part is degraded but in most cases it does not matter. It only matters when full strength is required.

            A threading chart that gives depth of cut can be used as a guide ONLY and I do that most the time. You should stop before it gets to the recommended depth and start measuring or testing the thread.

            There is no way I could count the threads I have cut with a threading tool with a sharp point and to my knowledge none of them came back with a failure. For anything up to 10 tpi I used a sharp point, above that I usually put a flat on the tip, not a radius.

            You really have to consider what the thread will be doing and how much strength it needs. You also have to know if both internal and external will have a sharp V. If so they may interfere with each other. Generally I cut an internal thread with a sharp V and on the external thread I use a sharp V and will file a flat on the thread after I cut it to size.
            Last edited by Carld; 08-01-2011, 05:37 PM.
            It's only ink and paper


            • #7
              I once had threads that measured the EXACT right pitch diamiter to fit, And the crests where the EXACT OD that the height of the female threads to match...

              My problem? Much too exact. The crests where not rounded so the unrounded crests would bind in the rounded female vallys, Thankfuly... I just jammed it in insted of threading it deeper (Rounded the crests by forming), because it would of had to of been threaded so deep that the crests would become sharp V's before it would of fit. (After one insertion, it threads in/out with no binding)

              The aluminum test plug I made rounded much easyer then the steel part I made to duplicate it. Took till the steel part to realise what I was doing wrong.

              Proper solution would of been turn the OD down more to make up for the unrounded crests, Or use a proper toping insert for that TPI.

              Sometimes, the numbers lie and the form really does matter!
              Play Brutal Nature, Black Moons free to play highly realistic voxel sandbox game.


              • #8
                I purity much figured that the numbers have a lot of room for interruption. I turn motley 1/2 X28tpi and 5/8X 24tpi for gun barrels. And the occasional 9/16X32tpi. I usually turn the OD down to the maximum allowable diameter and go from there. I just would like to be able to touch the insert to the barrel. And go from there and end up with a perfect thread. I like the inserts better they let me thread closer to a shoulder and in a run out grove. Threading a barrel for a muzzle break runs $100.00. And that includes taking the gun apart and back together. So speed is the money maker.


                • #9
                  I don't think that's going to happen. There's no way to know when the thread is cut to the exact correct depth without measuring or testing it. A barrel thread has to be a fairly good fit to the receiver and I suspect your using the receiver as a test thread to fit the barrel to. In that case you don't have to measure the thread as you cut it but you do have to know when to stop taking off metal and start testing after each pass.

                  That's where a thread depth chart comes in handy. I look at my chart and if it says the thread depth is, say .050" then when I get to .040" feed in with the compound I start testing the thread fit with the internal test thread piece. When the fit is what I want I stop and clean up the thread and I am done.

                  For the threading I do I seldom have to measure the PD, I just use test nuts or the part I am trying to fit it to. The only time I use wires or a thread mic is when I don't have a test part and then your depending on who ever cut the internal thread cut it to a standard with a test thread.

                  Since I bought my insert threading holder I have got to liking it a lot and one good part is if the insert breaks and nothing moves changing the insert gets you back in business. Most the time if the insert breaks it knocks everything out and I have to set up on the thread again and that's a bugger. I also use HSS Cobalt for threading and I have a few ground off on the side to get close to a shoulder.
                  Last edited by Carld; 08-01-2011, 09:56 PM.
                  It's only ink and paper